NI Ultiboard User Manual NI Ultiboard User Manual May 2008 374488C-01 TM
Support Worldwide Technical Support and Product Information ni.
Important Information Warranty The media on which you receive National Instruments software are warranted not to fail to execute programming instructions, due to defects in materials and workmanship, for a period of 90 days from date of shipment, as evidenced by receipts or other documentation. National Instruments will, at its option, repair or replace software media that do not execute programming instructions if National Instruments receives notice of such defects during the warranty period.
WARNING REGARDING USE OF NATIONAL INSTRUMENTS PRODUCTS (1) NATIONAL INSTRUMENTS PRODUCTS ARE NOT DESIGNED WITH COMPONENTS AND TESTING FOR A LEVEL OF RELIABILITY SUITABLE FOR USE IN OR IN CONNECTION WITH SURGICAL IMPLANTS OR AS CRITICAL COMPONENTS IN ANY LIFE SUPPORT SYSTEMS WHOSE FAILURE TO PERFORM CAN REASONABLY BE EXPECTED TO CAUSE SIGNIFICANT INJURY TO A HUMAN.
Conventions The following conventions are used in this manual: » The » symbol leads you through nested menu items and dialog box options to a final action. The sequence File»Page Setup»Options directs you to pull down the File menu, select the Page Setup item, and select Options from the last dialog box. This icon denotes a tip, which alerts you to advisory information. This icon denotes a note, which alerts you to important information.
Contents Chapter 1 User Interface Introduction to the Ultiboard Interface ..........................................................................1-1 Toolbars .........................................................................................................................1-1 Standard Toolbar .............................................................................................1-1 View Toolbar...................................................................................................
Contents Spreadsheet View: SMT Pads Tab.................................................................. 1-39 Spreadsheet View: THT Pads Tab .................................................................. 1-40 Spreadsheet View: Vias Tab ........................................................................... 1-42 Spreadsheet View: Copper Areas Tab ............................................................ 1-43 Spreadsheet View: Keep-ins/Keep-outs Tab ...............................................
Contents Working with the Board Outline ...................................................................................3-5 Using the Drawing Tools to Create a Board Outline ......................................3-5 Importing a DXF File ......................................................................................3-6 Using a Pre-Defined Board Outline ................................................................3-6 Using the Board Wizard ........................................................
Contents Placing Other Elements ................................................................................................. 4-20 Placing Mounting Holes and Connectors........................................................ 4-21 Placing Holes .................................................................................................. 4-21 Placing Shapes and Graphics .......................................................................... 4-21 Working with Jumpers ..............................
Contents Placing a Bus ...................................................................................................5-5 Working with Density Bars .............................................................................5-6 Working with Keep-in/Keep-out Areas...........................................................5-7 Placing Keep-in/Keep-out Areas ......................................................5-7 Viewing and Editing Keep-in/Keep-out Properties ..........................
Contents Chapter 6 PCB Calculators PCB Transmission Line Calculator ............................................................................... 6-1 Microstrip Trace Calculations......................................................................... 6-2 Embedded Microstrip Trace Calculations....................................................... 6-3 Centered Stripline Trace Calculations ............................................................ 6-4 Asymmetric Stripline Trace Calculations ...........
Contents Chapter 8 Preparing for Manufacturing/Assembly Placing and Editing Text................................................................................................8-1 Capturing Screen Area...................................................................................................8-2 Placing a Comment ........................................................................................................8-3 Renumbering Parts................................................................
Contents Setting Mechanical CAD Colors..................................................................... 10-3 Controlling Workspace Elements for Mechanical CAD................................. 10-4 Setting Paths for Mechanical CAD ................................................................. 10-5 Setting Mechanical CAD Dimensions ........................................................... 10-5 Appendix A Menus and Commands File Menu...................................................................
Contents Edit»Selection Filter........................................................................................A-6 Edit»Orientation ..............................................................................................A-6 Edit»Align .......................................................................................................A-6 Edit»Vertex......................................................................................................A-7 Edit»In-Place Part Edit ...............
Contents Place»Jumper .................................................................................................. A-13 Place»Net Bridge ............................................................................................ A-13 Place»Hole ...................................................................................................... A-13 Place»Automatic Test Points .......................................................................... A-14 Place»Unplace Parts........................
Contents Tools»View 3D Position .................................................................................A-19 Tools»Show or Hide Height............................................................................A-19 Options Menu ................................................................................................................A-20 Options»Global Preferences............................................................................A-20 Options»PCB Properties............................
1 User Interface The following sections explain the basic components of the Ultiboard Graphical User Interface (GUI) and show how to set up user preferences and PCB properties. Some of the described features may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition.
Chapter 1 User Interface Button Description New File button. Creates a new project (if none are currently open) or a new design if a project is currently open. Refer to the Creating a Project and Creating a Design sections of Chapter 2, Beginning a Design, for more information. Open File button. Opens an existing project. Refer to the Opening an Existing File section of Chapter 2, Beginning a Design, for more information. Open Sample button. Opens the samples folder. Save File button.
Chapter 1 User Interface View Toolbar The View toolbar contains buttons for modifying the way the screen is displayed, and appears by default when you run Ultiboard. The View toolbar buttons are explained in the table below. Button Description Redraw the Screen button. Redraws the currently active design workspace. Refer to the Refreshing the Design section of Chapter 2, Beginning a Design, for more information. Toggle Full Screen button.
Chapter 1 User Interface Main Toolbar The Main toolbar contains buttons for common board design functions. Its buttons are described in the table below. Button Description Select button. De-activates any selected mode (for example, for placing traces) and allows you to select an element on the board. Show or Hide Design Toolbox button. Shows or hides the Design Toolbox. Refer to the Design Toolbox section for more information. Show or Hide Spreadsheet button. Shows or hides the Spreadsheet View.
Chapter 1 Button User Interface Description Place Via button. Places a via on the design. Refer to the Working with Vias section of Chapter 5, Working with Traces and Copper, for more information. Place Copper Area button. Places a copper area on the design. Create Power Plane button. Places a powerplane on the design. Refer to the Placing Powerplanes section of Chapter 5, Working with Traces and Copper, for more information. Design Rule Check button.
Chapter 1 User Interface Button Description Enable Selecting Copper Areas button. Use to allow or prevent selection of copper areas. Enable Selecting Vias button. Use to allow or prevent selection of vias. Enable Selecting Pads button. Use to allow or prevent selection of pads. Enable Selecting SMD Pads button. Use to allow or prevent selection of Surface Mount Device pads. Enable Selecting Attributes button. Use to allow or prevent selection of attributes. Enable Selecting Other Objects button.
Chapter 1 Button User Interface Description Fill Style button. Sets the fill style, either transparent or solid. Line Color button. Sets the color of the layer’s line. Line Type button. Sets the lines style, for example, solid, dashed. Edit Toolbar The Edit toolbar contains the functions used for editing specific elements, including in-place editing and orientation. The Edit toolbar buttons are explained in the table below. Button Description Toggle “In-Place” PCB Part Edit button.
Chapter 1 User Interface Align Toolbar The Align toolbar contains the functions used to align and space design elements. Refer to the Aligning Shapes and Partsand Spacing Shapes and Parts sections of Chapter 4, Working with Parts, for more information. The Align toolbar buttons are explained in the table below. Button Description Align Left button. Aligns the left sides of the selected parts. Align Right button. Aligns the right sides of the selected parts. Align Top button.
Chapter 1 Button User Interface Description Space Down Plus button. Increases vertical space between two or more objects. Space Down Min button. Decreases vertical space between two or more objects. Place Toolbar The Place toolbar contains the functions used to place elements such as traces, lines and polygons on the design. The Place toolbar buttons are explained in the table below. Button Description Place Comment button. Places a comment on the design.
Chapter 1 User Interface Button Description Place Ellipse button. Places an ellipse on the design. Refer to the Placing Shapes and Graphics section of Chapter 4, Working with Parts, for more information. Place Pie button. Places a pie-shape on the design. Refer to the Placing Shapes and Graphics section of Chapter 4, Working with Parts, for more information. Place Rounded Rectangle button. Places a rectangle with rounded corners.
Chapter 1 Button User Interface Description Place Text button. Places text on the design. Useful for annotation purposes. Refer to the Placing and Editing Text section of Chapter 8, Preparing for Manufacturing/Assembly, for more information. Place a Standard Dimension button. Places a dimension between any two selected points. Refer to the Working with Dimensions section of Chapter 4, Working with Parts, for more information. Place a Horizontal Dimension button.
Chapter 1 User Interface Button Description Polygon Splitter button. Splits copper areas and powerplanes. Refer to the Splitting Copper section of Chapter 5, Working with Traces and Copper, for more information. Remove Copper Islands button. Removes copper islands. Refer to the Placing Copper Areas section of Chapter 5, Working with Traces and Copper, for more information. Wizard Toolbar The Wizard toolbar contains the wizard functions supported by Ultiboard.
Chapter 1 Button User Interface Description Start/Resume Autorouting button. Starts automatically placing traces. Stop/Pause Autorouter button. Setting Preferences This section explains general procedures for setting preferences. The following sections describe details of setting specific options. Complete the following steps to set your user preferences: 1. Choose Options»Global Preferences.
Chapter 1 User Interface 4. • Line width cache size—The number of recently used line widths Ultiboard keeps in memory. Minimum cache size is 5. • Undo buffer size—The number of undo actions allowed. • Load last file on startup—Enable if you would like to continue working on the last file you had open in your previous Ultiboard session. • Unicode Settings box—If desired, enable the Save .TXT files as plain text checkbox. • Language—Select the desired language from the list.
Chapter 1 User Interface Colors Tab Ultiboard allows you to set up color schemes for the workspace background and other displayed elements. Complete the following steps to set up color schemes: 1. Choose Options»Global Preferences. The Preferences dialog box appears. 2. Select the Colors tab and complete the following as required: • To apply an existing color scheme, either the default or one you have created, choose from the Color scheme drop-down list.
Chapter 1 User Interface 3. 4. Set the viewing options in the View area: • Show pin 1 mark—Enable to display pin 1 of a device with a unique marking. • Show Copper Areas—Enable to display copper areas. This applies to copper areas only, not regular polygon shapes on non-copper layers. • Show pin info in pin—Enable to display the pin number and hole size when zoomed in. In the On select entire trace area: • 5. In the Part Drag area: • 6. 7. 8.
Chapter 1 9. User Interface In the On trace placement area: • Auto trace narrowing—Enable to allow traces to narrow as necessary during routing. • Auto add teardrop—Enable to add a teardrop when a trace is placed. 10. In the DRC & Net check area: • No Realtime Check—Enable to prevent a DRC and netcheck in “real time” as you place objects, for example, parts. • Check on action end—Enable to perform a DRC and netcheck after each action, for example, part placement.
Chapter 1 User Interface 14. To apply your changes but leave the Preferences dialog box open, click Apply. To apply your changes and close the Preferences dialog box, click OK. Dimensions Tab Use the Dimensions tab of the Preferences dialog box to define the characteristics to be used for any dimensions placed in the board. Refer to the Working with Dimensions section of Chapter 4, Working with Parts, for information about placing dimensions.
Chapter 1 User Interface • Displayed Unit—Select the unit of measure to be displayed with the dimension. If you select Use Design Settings, the unit of measure selected in the Design Units field of the Grids & Units tab of the PCB Properties dialog box are used. This setting also appears in the Draw Settings toolbar. • Alignment and Position—These are where you set how the text appears in relation to the arrow. • Orientation—This is where you select the angle at which the dimension displays.
Chapter 1 User Interface Setting PCB Properties Many characteristics of your PCB design are controlled through the PCB Properties dialog box including the number of layers, design rules and grid settings. These settings are saved with the design and will be in effect when the design is reopened.
Chapter 1 3. User Interface • Degree Step—This field becomes active when Polar Grid is selected in the Grid Type field. Enter the desired distance between the grid’s elements (dots, lines or crosses). Select the unit of measure in the drop-down list to the right of this field—choices are: degrees, radians, or grads. • Grid start offset—This field becomes active when Polar Grid is selected in the Grid Type field.
Chapter 1 User Interface 4. As you make changes to the layer settings, the Allowed Vias pane shows the acceptable layer combinations for blind and buried vias or microvias. Use the checkboxes to select the layer combinations you want to allow in your design as shown in the example in the figure below. 5.
Chapter 1 User Interface Through Hole Pad Annular Ring Footprints in the database have been designed with pad sizes in accordance with the manufacturers’ recommendations. To change these settings you can edit the footprint in the database or directly on the design using the In-place Part Edit command. Alternatively, you can apply a set of design rules to specific footprints or to the entire design.
Chapter 1 User Interface The Capture Land Diameter field determines the land diameter where the microvia starts, while Target Land Diameter determines the diameter where the microvia ends. These terms are in accordance with the IPC and JPCA joint standard IPC/JPCA-2315, Design Guide for High Density Interconnects (HDI) and Microvias. The Maximum Layer Span is either one or two layers. Maximum Vias Per Net The Nets area is where you set up the maximum number of vias allowed per net.
Chapter 1 User Interface Complete the following steps to rename layers: 1. Click Rename in the Layer Names area. The Select Layer for Renaming dialog box appears. 2. Select the layer that you wish to rename and click OK. The Layer dialog box appears. 3. Enter the new Layer Name and click OK. Design Rules Tab Complete the following steps to set the design rules for the PCB: 1. Click on the Design Rules tab. 2.
Chapter 1 User Interface Setting Favorite Layers You can assign shortcuts for up to ten layers using the Favorite layers tab. These shortcuts can then be used to make a layer active. The active layer is the layer where any new elements will be placed, or where any deletions will be made. Complete the following steps to assign shortcut numbers to layers: 1. Click on the Favorite layers tab. 2. Select the desired layer from the drop-down list beside each layer number.
Chapter 1 User Interface Design Toolbox The Design Toolbox, shown in the figure below, is a vital part of the user interface. You will use it often to manage your design efforts by controlling major parts of Ultiboard’s functionality. To toggle it on or off, select View»Design Toolbox. The Design Toolbox is made up of two tabs: • The Projects tab lets you view the projects that are currently open. Each project may contain one or more designs. Double-click to make a particular design the current view.
Chapter 1 User Interface Birds Eye View The Birds Eye View shows you the design at a glance and lets you easily navigate around the workspace. To magnify a specific area on the design, drag a rectangle around the desired area on the Birds Eye View. The rectangle snaps to the same ratio as the design space. Note All layers appear in the Birds Eye View, whether or not they have been disabled in the Layers tab of the Design Toolbox.
Chapter 1 User Interface Spreadsheet View The Spreadsheet View allows fast advanced viewing and editing of parameters including part details such as footprints, Reference Designators, attributes and design constraints. By default, the Spreadsheet View does not appear until you have opened a project. To toggle the Spreadsheet View on and off, select View»Spreadsheet View. The following buttons are available in the Spreadsheet View. Note The buttons do not appear in all tabs.
Chapter 1 User Interface Button Description Find and Select the Part button. Zooms in on the selected part. Refer to the Using the Parts Tab for Other Functions section of Chapter 4, Working with Parts, for more information. Lock the Selected Part button. Locks the selected unlocked parts or unlocks the selected locked parts. Refer to the Using the Parts Tab for Other Functions section of Chapter 4, Working with Parts, for more information. Start Placing the Unpositioned Parts button.
Chapter 1 User Interface When you right-click on an item in the DRC tab, a pop-up menu displays with the following available selections: • Copy—Copies all items in the DRC tab and places them on the clipboard. • Go to Error/Tag—Click to go to the highlighted error or warning on the workspace. • Add to Filter—Click to filter out the selected error/warning type. This type of error/warning will no longer show in the DRC tab. • Remove all filters—Click to remove all error/warning types from the filter.
Chapter 1 User Interface 3. Select the error type(s) to add to the filter. You can use the Ctrl and Shift keys to select multiple items. 4. Click OK to close the Add Filter(s) dialog box and add the selected items to the Filter Manager. 5. Click Close to close the Filter Manager dialog box. The selected error types no longer display in the DRC tab. To remove an error type from the Filter Manager, select the error type and click Remove Filter. To remove all error types, click Remove All.
Chapter 1 User Interface You can also right-click an item to display a popup that contains Copy; Clear Results; Go to. Spreadsheet View: Parts Tab Use the Parts tab to work with the parts in your design. Refer to the Using the Parts Tab in the Spreadsheet View section of Chapter 4, Working with Parts, for more information.
Chapter 1 User Interface Column Description Pin Swap If enabled, allows like-pins to be swapped during the routing process. You can choose either No (not enabled), Yes or Use Group Settings. Refer to the Working with the Group Editor section of Chapter 3, Setting Up a Design, for more information. Gate Swap If enabled, allows like-gates, to be swapped during the routing process.
Chapter 1 Column User Interface Description Pin Swap If enabled, allows pins for like-parts to be swapped during the routing process. Gate Swap If enabled, allows like-gates, to be swapped during the routing process. You can choose Internal Gates Only, which will swap gates within the same IC; No Swapping; or Advanced Swapping, which will swap gates between ICs (both devices must be set to Advanced Swapping). Locked Yes indicates that the part cannot be moved.
Chapter 1 User Interface Column NI Ultiboard User Manual Description Min Width The minimum width to which a trace will be laid during routing. You can enter a value here, or use the Group Editor. Refer to the Working with the Group Editor of Chapter 3, Setting Up a Design, section for more information. Topology The topology of the net as set in the Netlist Editor. Choices are Shortest, Daisy Chain and Star.
Chapter 1 Column © National Instruments Corporation User Interface Description Bus Group This is the bus group in which the net is contained. You can either enter the group name here, or use the Group Editor. Refer to the Working with the Group Editor section of Chapter 3, Setting Up a Design, for more information. Differential Pair This is the differential pair to which the net belongs. Refer to the Working with the Group Editor section of Chapter 3, Setting Up a Design, for more information.
Chapter 1 User Interface Spreadsheet View: Nets Groups Tab Use the Net Groups tab to work with net groups. Column NI Ultiboard User Manual Description Net Group This is the group in which the net is contained. You can either enter the group name here, or use the Group Editor. Refer to the Working with the Group Editor section of Chapter 3, Setting Up a Design, for more information. Trace Width The “default” width of the traces in the group that are placed during routing.
Chapter 1 Column User Interface Description Routing Priority The routing priority for the selected net group. 1 is the highest priority, 2 the second highest, etc. Leave as None if priority routing is not required. This feature is not available in all versions of Ultiboard. Locked Yes indicates that the part cannot be moved. No indicates that the part can be moved. Max Via Count This is the maximum number of vias allowed in the net group.
Chapter 1 User Interface Column Description Trace Clearance The clearance of the trace to parts. You can use net settings, or as set in the SMT Pin Properties dialog box. Refer to the Viewing and Editing SMT Pin Properties section of Chapter 4, Working with Parts, for more information. Neck Length The default length of the neck where the trace attaches to the pin, as set in the SMT Pin Properties dialog box. You can also enter the value here.
Chapter 1 Column © National Instruments Corporation User Interface Description Inner Pad Shape The shape of the inner layer pad as set in the Through Hole Pin Properties dialog box. Refer to the Viewing and Editing Through Hole Pin Properties section of Chapter 4, Working with Parts, for more information. Bottom Pad Shape The shape of the bottom layer pad as set in the Through Hole Pin Properties dialog box.
Chapter 1 User Interface Spreadsheet View: Vias Tab Use the Vias tab to work with via information. Column Description Assume Net The unique identifier for the net to which the via is connected. Can be changed by using the drop-down list. Lamination Double-click to display the Select the lamination that is to be used for this via dialog box, where you select the layers that the via is to run between. This setting cannot be changed for micro vias.
Chapter 1 User Interface Spreadsheet View: Copper Areas Tab Use the Copper Areas tab to work with information for copper areas. Column © National Instruments Corporation Description Layer The layer on which the copper area is found, as set in the Copper Area Properties dialog box. Refer to the Viewing and Editing Copper Properties section of Chapter 5, Working with Traces and Copper, for more information. Locked Yes indicates that the copper area cannot be moved.
Chapter 1 User Interface Spreadsheet View: Keep-ins/Keep-outs Tab Use the Keep-ins/Keep-outs tab to work with information for Keep-in or Keep-out areas. Column NI Ultiboard User Manual Description Name Name of the Keep-in or Keep-out. Can be entered here, or in the Keep-in/Keep-out Properties dialog box. Refer to the Working with Keep-in/Keep-out Areas section of Chapter 5, Working with Traces and Copper, for more information. Type Indicates whether the area is a Keep-in or a Keep-out.
Chapter 1 Column User Interface Description Part Group Double-click to display the Select Groups dialog box, where you select the part group to which you wish to assign the Keep-in/out. You can also set this in Keep-in/Keep-out Properties dialog box. Refer to the Working with Keep-in/Keep-out Areas section of Chapter 5, Working with Traces and Copper, for more information. Heights Bigger Than Assign a height (z-axis) value to theKeep-in/out.
Chapter 1 User Interface Spreadsheet View: Statistics Tab This tab displays the following statistics: • Total number of pins. • Pins in a net. • Not connected pins. • Test pins. • Jumpers. • Total number of vias. • Total number of connections. • Unrouted connections. • Completion. • Total number of parts. • Total number of nets. Customizing the Interface The Ultiboard user interface is highly customizable. Toolbars can be docked in various positions and orientations.
Chapter 1 User Interface Commands Tab The Commands tab in the Customize dialog box is used to add commands to menus and toolbar. Complete the following steps to add a command to a menu or toolbar: 1. Drag the desired command from the Commands list to the desired menu or toolbar. When a command is selected in the Command list, its description is displayed in the Description field. 2.
Chapter 1 User Interface 3. 4. The buttons in this tab function as follows: • Reset All—Displays the Reset Toolbars dialog box, where you select whether to reset the currently selected toolbars, or all toolbars. You are prompted to select the configuration file you wish to use, for example, “default.ewcfg”. • New—Displays the Toolbar Name dialog box, where you enter the name for a new toolbar. When you click OK, a new toolbar with the name that you entered is created.
Chapter 1 User Interface Options Tab Use the Options tab in the Customize dialog box to set up the appear of Ultiboard’s toolbars—switch the checkboxes on or off as desired. Customization of Pop-up Menus To customize the appearance of toolbar buttons and menu items, a pop-up menu is available when the Customize dialog box is open. Complete the following steps to display the pop-up: 1. Be sure you have the Customize dialog box open. 2.
2 Beginning a Design The following sections explain how to start a design in Ultiboard. Some of the described features may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition. About Designs and Projects Designs are stored inside projects, allowing you to group them together for easy access.
Chapter 2 Beginning a Design Creating a Design A design is created automatically when you create a project file. You can also create a design and assign it to an existing project file. Remember that a design must always be associated with a project. Complete the following steps to create a design file: 1. Choose File»Open and open the project to which the design is to be added. 2. Choose File»New Design. The New Design dialog box appears. 3. Type the design name in the Design Name field. 4.
Chapter 2 Beginning a Design (tracklength_max "-1.000000000000") (tracklength_min "-1.000000000000") (clearance_to_trace "-1.000000000000") (clearance_to_pad "-1.000000000000") (clearance_to_via "-1.000000000000") (clearance_to_copper "-1.000000000000") (routing_layer "") (settings_locked "0") (net_group "") ) The following is an example of component information from a netlist file.
Chapter 2 Beginning a Design Complete the following steps to import a netlist file: 1. Select File»Import»UB Netlist, navigate to the desired file (for example, Getting Started 2.EWNET) and click Open. The Default Trace Width and Clearance dialog box appears. 2. Enter the desired Units, Width, and Clearances values and click OK. The Import Netlist Action Selection dialog box appears. 3. Select the desired actions, for example, Add New Net: VCC and click OK.
Chapter 2 Beginning a Design Opening an Existing File Complete the following steps to open an existing file: 1. Choose File»Open. A standard file section dialog box appears, with the Files of Type list defaulted to Ultiboard files. 2. In the Files of type list, choose the kind of file to open. You can open the following: • Ultiboard files (*.ewprj). • Orcad files (*.max, *.llb). • Protel files (*.pcb, *.ddb). • Gerber files (*.g). • DXF files (*.dxf). • Ultiboard 4 & 5 design files (*.ddf).
Chapter 2 Beginning a Design To save all open file and designs, choose File»Save All. To close the current file and its designs, choose File»Close. If you have any unsaved changes in the file or designs, you are prompted to save the file and/or designs. To close all open projects and designs, choose File»Close All. If you have any unsaved changes in the projects or designs, you are prompted to save the projects and/or designs.
Chapter 2 Beginning a Design Selecting and Unselecting Elements You can select and unselect single and multiple elements in a design such as parts, holes, and traces. To select a single element on a board, click the element. A dotted line around the element, or running through the trace, indicates that it has been selected. Complete the following to select multiple elements on a board: Hold down the Shift key while clicking the elements that you want to select.
Chapter 2 Beginning a Design Place and Select Modes Ultiboard assumes that placing shapes, parts, or traces on a board are actions you are likely to repeat. As a result, when you place items on the board, you remain in “place mode” (the cursor has a small icon attached, indicating what is being placed) so that you can continue to place the same type of item repeatedly.
Chapter 2 Beginning a Design 3. To constrain your search to only certain attributes, choose from the Find special drop-down list. For example, if you enter “test” in the Find what field, you will find all elements with the string “test” in any of their attributes. However, if you choose Name from the Find special drop-down list, you will find only elements with “test” in their name. 4. Optionally, enable the Match case and/or Match whole word check boxes. 5. Click Find.
Chapter 2 Beginning a Design When you display a design on the full screen, everything except the design disappears (depending on your settings in the Preferences dialog box, scrollbars may or may not appear). Menu functions can still be used through their keyboard shortcuts—for example, you can use F8 to zoom in, and F9 to zoom out. Again, depending on the Preferences dialog box settings, you may be able to pan through the design by moving your cursor over the outside edges.
Chapter 2 Beginning a Design Refreshing the Design After adding and changing elements, the design can begin to look a little confusing, with bits and pieces of elements looking like they have been left behind on the design after being moved, for example. This can be for many reasons, including the limitations of the computer monitor being used, although it does not affect the design. Complete the following to clean up the design, removing any extraneous images that should not be there: 1.
3 Setting Up a Design The following sections explain the basic functions you must perform to get your board set up. These tasks should be performed before you begin placing parts and/or traces. Some of the described features may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition.
Chapter 3 Setting Up a Design • The other method typically uses a layered pair as a core to which single layers of copper foil are added to build up the board. Prepreg is also used to bond the layers. Build-up layers are usually added in equal numbers to the top and bottom of the core to prevent warping of the final product. A via is a plated through-hole in a printed circuit board used to connect two or more layers, as well as the top and bottom surfaces of the board.
Chapter 3 Setting Up a Design Accessing Layers The Layers tab of the Design Toolbox allows you to move through the layers of your PCB design, and control their appearance. To display the Layers tab, click the Layers tab in the Design Toolbox. The tab appears, as shown in the figure below: Layers with a check mark are displayed on the workspace. Layers with a check mark in a grey box are displayed in the workspace, but are dimmed.
Chapter 3 Setting Up a Design The Layers tab is divided into four sections: • PCB—These are the working layers of your design. Refer to the Setting PCB Properties section of Chapter 1, User Interface, for more information about setting up the properties of the PCB layers. • Assembly—These are the layers associated with production of your board. These are useful whenever you are using paste to hold joints or glue (adhesive) to hold components on the board (mostly on SMDs).
Chapter 3 Setting Up a Design Tip You can show or hide individual ratsnests from the Show Ratsnest column in the Nets tab of the Spreadsheet View, and also from the Net Edit dialog box. Refer to the Using the Netlist Editor section of Chapter 5, Working with Traces and Copper, for more information. To change the color of the elements in a layer, click the color box beside the layer name and, from the dialog box that appears, choose a color.
Chapter 3 Setting Up a Design To edit the properties of the placed board outline, select the outline and select Edit»Properties. (You must be on the Board Outline layer). Importing a DXF File Complete the following steps to import a DXF board outline from a CAD program such as AutoCAD®: 1. Choose File»Import»DXF. A standard file selector appears. 2. Navigate to the correct location for the .dxf file, select it and click OK. 3. The DXF import settings dialog box appears. 4.
Chapter 3 Setting Up a Design Using the Board Wizard Complete the following steps to use the Board Wizard: 1. Choose Tools»Board Wizard. The Board Wizard... Board Technology dialog box appears. 2. Enable the Change the layer technology option. Choose the board technology and click Next. Refer to the Defining Copper Layers section for more information about board technology. The next step of the wizard depends on which type of technology you chose. 3.
Chapter 3 Setting Up a Design 4. 5. If you chose Single Sided or Double Sided, or upon clicking Next after defining the lamination settings for a multi-layer board: • Define the default Units of measurement for the design. • Define the board Reference Point. This can be changed later. Refer to the Setting the Board’s Reference Point section for more information. • Define the Board Shape and Size.
Chapter 3 Setting Up a Design Enter coordinate dialog box Complete the following steps to set the reference point at precise X, Y coordinates: 1. Press the asterisk key (*) or to display the Enter coordinate dialog box. 2. Enter the X and Y coordinates and the desired units of measure. 3. Optionally, select Snap to grid to have the reference point snap to the closest grid on the workspace.
Chapter 3 Setting Up a Design Design Rule Errors Design rule errors appear in the DRC tab of the Spreadsheet View as they occur, and disappear as they are corrected. Double-click on an error in the DRC tab to zoom in on the affected area on the design, which will be indicated with a red circle, as shown in the example below.
Chapter 3 Setting Up a Design • Pin “[Pin number]” from Part “[refdes]”(value) in Net “[Net name]” is missing from shape “[shape name]”— A pin belonging to the specified part was given in the netlist but does not exist in the shape that was given for the part. • Unused Pin [Pin name] is {close to, connected to} {Unused Pin, Copper}—The given pin that was not assigned to a net is close to or connected to another unused pin or copper, for example, a trace, powerplane, or copper area.
Chapter 3 Setting Up a Design Working with Net Groups Complete the following steps to create a net group: 1. Select Tools»Group Editor to display the Edit Groups dialog box. 2. Click the Net Groups tab. 3. Click Add. The Add group dialog box appears. 4. Enter the desired name and click OK. The Change group settings dialog box appears. 5. Change the settings in the Group Settings area as desired. Refer to the Change Group Settings dialog box and Net Group Settings sections for more information.
Chapter 3 8. Setting Up a Design Click checkboxes beside the desired nets in the Assign Nets list and click Apply to add them to the group. You cannot assign a net to more than one group. Therefore, nets that are already assigned to another net group do not appear in the Assign Nets list. Note 9. Click OK to close the Edit Groups dialog box. Complete the following steps to edit a net group: 1. Select Tools»Group Editor to display the Edit Groups dialog box. 2. Select the Net Groups tab. 3.
Chapter 3 Setting Up a Design 6. Click OK to return to the Part Groups tab. The newly created group appears in the Groups list. 7. Highlight the new group to display a list of parts you can add to the group in the Assign Parts list, as shown in the example below. 8. Click checkboxes beside the desired parts in the Assign Parts list and click Apply to add them to the group. Note You cannot assign a part to more than one group.
Chapter 3 Setting Up a Design Complete the following steps to edit a part group: 1. Select Tools»Group Editor to display the Edit Groups dialog box. 2. Select the Part Groups tab. 3. Highlight the desired group in the Groups list. 4. Change the part assignments as desired and click Apply. 5. Optionally, highlight the desired group in the Groups list and click the Properties button to display the Change group settings dialog box. 6.
Chapter 3 Setting Up a Design 7. Click checkboxes beside the desired nets in the Assign Nets list and click Apply to add them to the group. You cannot assign a net to more than one group. Therefore, nets that are already assigned to another bus group do not appear in the Assign Nets list. Note 8. Click OK to close the Edit Groups dialog box. Complete the following steps to edit a bus group: 1. Select Tools»Group Editor to display the Edit Groups dialog box. 2. Select the Bus Groups tab. 3.
Chapter 3 Setting Up a Design Working with Differential Pairs Complete the following steps to create a differential pair: 1. Select Tools»Group Editor to display the Edit Groups dialog box. 2. Click the Differential Pairs tab. 3. Click Add. The Add group dialog box appears. 4. Enter the desired name and click OK. The Change group settings dialog box appears. 5. Change the settings in the Group Settings area as desired.
Chapter 3 Setting Up a Design 8. Click two checkboxes beside the desired nets in the Assign Nets list and click Apply to add them to the group. Note You cannot assign a net to more than one differential pair. Therefore, nets that are already assigned to another differential pair do not appear in the Assign Nets list. 9. Click OK to close the Edit Groups dialog box. Complete the following steps to edit a bus group: 1. Select Tools»Group Editor to display the Edit Groups dialog box. 2.
Chapter 3 Setting Up a Design Net Group Settings For net groups, the following Group Settings are available: • Group Name • Clearance Settings • Trace Width Settings • Trace Length Settings • Routing Layers • Routing Priority • Locked As well as setting the clearance for a net group, you can set clearances for individual nets within that group. You can, for example, set the clearance for the net group to 10 mils, and the clearance for two or more nets within that group to 5 mils.
Chapter 3 Setting Up a Design For information on any setting, select it in the Group Settings list. A description appears in the field at the bottom of the dialog. You may need to make the dialog box larger to view some of the descriptions. Do this by dragging the dialog’s lower-right corner. Differential Pair Settings For differential pairs, the following Group Settings are available: • Length Constraints • Space Constraints For information on any setting, select it in the Group Settings list.
4 Working with Parts The following sections explain how to work with parts as you create and edit designs. It covers the ways that you can place parts on the board, as well as the tools included to help you with part location and placement. It also includes information on Ultiboard’s parts database, and editing the parts in the database and on the board. Some of the described features may not be available in your edition of Ultiboard.
Chapter 4 Working with Parts Complete the following steps to drag a part from outside the board outline: 1. Click on the part and drag it to the appropriate location. The placed part remains highlighted. 2. Click anywhere on the workspace, or right-click, to de-select the part. Using the Parts Tab in the Spreadsheet View The Parts tab in the Spreadsheet View shows a list of all the parts in your design.
Chapter 4 Working with Parts The selected part (4) appears in the preview area (5). Deselect the Show or Hide Preview button (6) if you do not wish to see the preview. Use the Start Placing the Unpositioned Parts button (7) to place unplaced parts. Use the Lock Selected Parts button (8) if you do not want a part to be moved. Use the Find and Select Part button (9) to quickly locate a part on the design.
Chapter 4 Working with Parts Using the Parts Tab for Other Functions The Parts tab of the Spreadsheet View can also be used to select a part, lock parts in their current position, find and select a part, or preview a part. To select a part using the Parts tab, double-click the part in the list. The part appears selected in the design. Complete the following steps to lock and unlock parts: 1. Click a part in the list to select it.
Chapter 4 Working with Parts Tools to Assist Part Placement The following sections tell you how to use the tools that Ultiboard provides to help you place parts and other elements on the design. Working with Ratsnests A ratsnest is a straight line connection between pads, indicating their connectivity. The ratsnest identifies the pads which should be connected according to the netlist, but which are not yet connected with traces.
Chapter 4 Working with Parts Working with Force Vectors Force vectors are powerful aids that help you place parts on the PCB. When you place a part manually on the board, you should pay careful attention to the force vectors coming from that part. They allow you to place the part as close as possible to other parts that are attached to the same net. Try to minimize the ratsnest distances from that part to other pads on the board.
Chapter 4 Working with Parts Dragging Parts To drag a part, click and drag it to the location where you want it placed, and release the mouse button. To specify the x/y coordinates to which the part is to move, press the * key on the numeric keypad or use the x/y coordinates on the status bar to get a precise reading on the location of the cursor. When you are on the exact location of the part, release the mouse button.
Chapter 4 Working with Parts Complete the following steps to adjust the shove spacing around a part: 1. Select the part. 2. Choose Edit»Properties. The Part Properties dialog box for the part appears. 3. Click the Part tab. This tab allows you to adjust the distance of part shove spacing. 4. Change the Part shove spacing as desired. If you choose Use Design Rule Defaults, the setting from the Design Rules tab of the PCB Properties dialog box is used. 5.
Chapter 4 Working with Parts 2. Your selections show in the preview area. 3. To manipulate the view of the part, click in the Dimensions area and use any of the following: © National Instruments Corporation • Zoom In button—Click to zoom in on the part for more detail. You can also press the F8 key. • Zoom Out button—Click to zoom out. Shows less detail and more of the whole part. You can also press the F9 key.
Chapter 4 Working with Parts Using Ruler Bars and Guides Use the ruler bars to place guides on the design, or to measure distances. Elements on the design will snap to the dotted lines representing the guides on the design. To toggle the ruler bars off or on, choose View»Ruler bars. Complete the following steps to place a ruler guide on the workspace: 1. 1 Click in the ruler bar at the measurement where you want the guide placed, shown in (1) in the figure below.
Chapter 4 Working with Parts Orienting Parts Parts are placed on the board in a certain orientation, which may not be the orientation in which you need them. You can, however, orient them by rotating them, or by swapping them to another layer. Complete the following steps to orient a part: 1. Select the part to be oriented. 2. Choose one of the following commands from the Edit»Orientation menu: • Flip Horizontal—Flips the part from left to right. • Flip Vertical—Flips the part from top to bottom.
Chapter 4 Working with Parts Spacing Shapes and Parts Shapes and parts can be spaced relative to each other on the board. Complete the following steps to space shapes and/or parts: 1. Select the elements to be spaced. 2. Choose the following commands from the Edit»Align menu to space the elements: • Space Across—Spaces three or more objects beside each other evenly. • Space Across Plus—Increases horizontal space between two or more objects.
Chapter 4 5. Working with Parts Begin selecting and dragging parts. As they are placed, the parts snap to the array. Place the part in the top left cell. The other parts will be placed at the same relative position in the other cells, beginning in the top left row and working to the right. 6. © National Instruments Corporation Continue placing parts.
Chapter 4 Working with Parts Replicating a Group The Group Replica Place function allows you to automatically apply the relative placement of parts in one group to another group. This is especially useful when duplicating the layout of channels in multi-channel PCBs. This example uses the following design: Refer to the Working with the Group Editor section of Chapter 3, Setting Up a Design, for information about group creation.
Chapter 4 5. Working with Parts Drag your mouse to the desired location and click to place the group. Unplacing Parts Complete the following steps to unplace all non-locked parts: 1. Select Place»Unplace Parts. A dialog displays asking if you wish to remove any left over copper after the unplace command. 2. Select either Yes or No. All unlocked parts are removed from the PCB and positioned outside of the board outline.
Chapter 4 Working with Parts Note You can sort attribute information by clicking on the column header. If you are looking at the attributes of a part that was imported from Multisim, and that part has variants assigned, the tab will also have a variant attribute as shown below. Note For complete information on variants, refer to the Multisim help file. Complete the following steps to modify or add an attribute: 1. Select the attribute you want to modify and click Change.
Chapter 4 Working with Parts Viewing and Editing Part Properties Complete the following steps to view and edit the properties of a part: 1. Select the part. 2. Choose Edit»Properties. The part’s Part Properties dialog box appears, consisting of four tabs: Attributes, Position, 3D Data, and Part. The Position tab is the default, and appears when you choose Edit»Properties. It displays the coordinates of the selected part: • X—The x-axis coordinate. • Y—The y-axis coordinate.
Chapter 4 Working with Parts 2. Choose the type of object to be created: • For a hole, enable the Hole option (the hole extends from the Offset to the Height)—If you want to make the selected part a hole in the 3D view, the part must be completely enclosed (for example, a circle or rectangle) and be contained within another larger object. For example, this could be used to create a notch or dimple in a DIP (dual-in-line package.
Chapter 4 Working with Parts 3. To place a band to indicate polarization (for example, for a diode), enable the Polarization marking option and choose the pin to mark. 4. To set an offset for the cylinder, enable Use custom cylinder offsets and enter the Start Offset and End Offset values. The Part tab is where you adjust the distance of part shove spacing, enter pin and gate swapping settings, and enter trace clearances. Refer to the Shoving Parts section for more information.
Chapter 4 Working with Parts Viewing and Editing Shape/Graphics Properties As with parts and traces, the properties of shapes can be viewed and edited. Complete the following steps to edit the properties of a shape that you have placed on the design: 1. Select the shape. 2. Choose Edit»Properties. Or Right-click, and select Properties from the context menu that appears. The name of the dialog box that appears varies, depending on the selected shape.
Chapter 4 Working with Parts Placing Mounting Holes and Connectors Mounting holes and connectors are placed from the database. Refer to the Placing Parts from the Database section for more information. Placing Holes You can also place holes directly onto the workspace, without using the database, as described below. 1. Select Place»Hole. The Through Hole Pin Properties dialog box appears. 2. Select the desired Shape for the whole. The Hole Preview changes accordingly.
Chapter 4 Working with Parts Button Command Description Place»Shape»Rounded Rectangle Left-click to define the opposite corners of the rectangle, then move the pointer towards the middle of the rectangle to define the roundness of the corners. Place»Shape»Circle Left-click two points that define the circle’s diameter.
Chapter 4 Working with Parts Working with Jumpers Placing Jumpers Default jumper pin settings are defined in the PCB Design tab of the Preferences dialog box. The default pad settings are based on the settings defined in the Pads/Vias tab of the PCB Properties dialog box. They can be manually set to use the annular ring specification or pad diameter settings by setting the properties of the pad when the jumper has been placed on the design. Complete the following steps to place a jumper: 1.
Chapter 4 Working with Parts To control the coordinates for the jumper’s starting and ending points, use the following from the Line tab: • X1—The X coordinate of the jumper’s starting point. • X2—The X coordinate of the jumper’s ending point. • Y1—The Y coordinate of the jumper’s starting point. • Y2—The Y coordinate of the jumper’s ending point. • Units—Units of measurement. To control the jumper’s wire and pin type, use the following in the Jumper tab: • Diameter—Sets the wire’s diameter.
Chapter 4 Working with Parts Viewing and Editing Test Point Properties Complete the following steps to edit a test point’s properties: 1. Select the test point and select Edit»Properties. The Testpoint Properties dialog appears. 2. Select the Test Point tab. 3. In the Wire area, set the following as desired: • Drill Diameter • Board Side—The side of the board on which the test point appears. Select Top or Bottom. • Rotation—The angle of rotation of the test point. 4.
Chapter 4 Working with Parts 5. Click to indicate the end point. Ultiboard stops measuring the length, and draws an arrow between your start and end points. 6. Move the pointer to position the stub line, and click when you’re done. In the example shown below, the vertical dimension of part RPACK1 has been moved to the outside right of the board outline. Viewing and Editing Dimension Properties Dimension properties consist of five tabs: Attributes, General, Position, Line and Dimensions.
Chapter 4 Working with Parts To control the coordinates for the dimension’s starting and ending points, use the following from the Line tab: • X1—The X coordinate of the dimension’s starting point. • X2—The X coordinate of the dimension’s ending point. • Y1—The Y coordinate of the dimension’s starting point. • Y2—The Y coordinate of the dimension’s ending point. • Units—Units of measurement.
Chapter 4 Working with Parts • Zoom In button—Click to zoom in on the part for more detail. You can also press the F8 key. • Zoom Out button—Click to zoom out. Shows less detail and more of the whole part. You can also press the F9 key. • Zoom Window button—Click (or press ) and then drag a rectangle around the portion of the part you want to enlarge. The area inside the rectangle enlarges to fill the Preview panel. • Zoom Full button—Click to view the entire part. You can also press .
Chapter 4 Working with Parts Editing Parts and Shapes Editing a Placed Part (In-Place Edit) In-place part editing lets you add, delete, or change a part and the items that make it up. You can add, delete, or move pads, change or move the lines that define a part, or place new shapes or lines in the part. Complete the following steps to use In-Place Edit on a part: 1. Select the part and choose Edit»In-Place Part Edit. An editing window opens, showing the selected part.
Chapter 4 Working with Parts 4. Indicate the pad type (THT or SMD) and its dimensions and spacing. Changes appear in the Preview panel. When you have made the necessary settings, click OK. The pad is attached to the pointer. Click on the part to place it. 5. When finished, choose Edit»In-Place Part Edit again to end the In-Place Edit function. The part appears with its changes. You can save your edited part in the database for future use.
Chapter 4 Working with Parts Complete the following steps to add a vertex to any line segment of a polygon: 1. Select the line (a selected line segment will have filled selection boxes while the other selection boxes in the polygon will be open). 2. Select Edit»Vertex»Add Vertex. A vertex is added in the middle of the segment. You can now move that vertex to change the shape of the polygon. Complete the following steps to remove a vertex: 1. Click on the point to be removed. 2.
Chapter 4 Working with Parts To edit a through hole pin’s attributes, use the Attributes tab. Refer to the Attributes section for more information. To edit a through hole pin’s display style, use the following in the General tab: • X—The x-axis coordinate. • Y—The y-axis coordinate. • Net—The net this through hole pin is on (read-only) • Angle (degrees)—The angle for the pin. • Board side—Select the Top or Bottom radio button to set the side of the board on which the through hole pin resides.
Chapter 4 Working with Parts Use the Thermal Relief tab to choose what type of thermal relief the pin will use when connecting to a copper area or power plane. 1. Select the desired thermal relief in the Type box. 2. Select the desired width of the spokes in the thermal relief from the Spoke Width drop-down list. Viewing and Editing SMT Pin Properties Complete the following steps to edit SMT (Surface Mount Technology) properties: 1. Select the desired SMT pin and select Edit»Properties. 2.
Chapter 4 Working with Parts Searching For and Replacing Parts Ultiboard allows you to search for parts in two ways: • Searching for parts in open designs. This method tells you if a specific part exists in all of the designs that are currently open. • Locating a part in a design. This method finds a specific part in the design where you are currently working, and zooms in on the part. You can also replace a part with one from the database.
Chapter 4 Working with Parts Replacing Parts Complete the following steps to replace a part on the design with a part from the database: 1. Select the part. 2. Choose Tools»Change Shape. The Get a Part from the Database dialog box opens. 3. In the Database panel, expand the categories until you find the category where the part is. The parts appear in the Available Parts panel. 4. In the Available Parts panel, select the part you need. The part is previewed in the Preview panel when it is selected.
Chapter 4 Working with Parts 3. Select the type of part you want to create: a net bridge, custom pad shape, PCB part or CAD part and click OK. The Edit mode window opens. 4. Design your part using the Place and Draw tools. Refer to the Toolbars section of Chapter 1, User Interface, for more information. 5. To add a pin to a PCB part or net bridge, choose Place»Pins. The Place Pins dialog box opens. Indicate the pad type (THT or SMD), its dimensions and spacing, and click OK.
Chapter 4 Working with Parts If you chose SMT in step 1 of the wizard, the Package Type choices shown below appear: 4.
Chapter 4 Working with Parts • Diameter—The diameter of the circle around pin 1 of the part. Becomes active when Circle Pin 1 Indicator is selected. • Distance from Edge—The distance between the circle around pin 1 and the edge of the part. Becomes active when Circle Pin 1 Indicator is selected. Note Depending on the Package Type selected in step 3 of the wizard, some settings may not be available. 5. Make the desired Package Dimension settings and click Next to display step 4 of the wizard.
Chapter 4 Working with Parts Click Add to create a new pad and then change the settings that are detailed above. You can create as many of these as you like, and choose between them by clicking on the “<<” and “>>” buttons. Remove any undesired pad types by clicking Remove. To change a pad type on the part, use the “<<” and “>>” buttons to select the desired pad in the lower right preview area and click on the pin you wish to change in the upper right part preview.
Chapter 4 Working with Parts 7. Make the desired pad settings and click Next to display step 6 of the wizard. The following Pins information appears: • Units—The unit of measure. • Number of Pins—The number of pins in the part. • Distances - Between pins (A)—The “A” distance between pins as shown on the preview. • Distances - Between rows (B)—The “B” distance between rows as shown on the preview. Distances information changes depending on the Package Type you selected in step 2 of the wizard.
Chapter 4 Working with Parts Managing the Database The Database Manager is where you add, organize, view, create, and manage the parts that Ultiboard stores in its database. To open the Database Manager, choose Tools»Database»Database Manager. There are three panels in the Database Manager: • The Database panel, which lists the databases and their sub-categories. The Database panel contains the following buttons. Refer to the Working with Database Categories section for more information.
Chapter 4 Working with Parts • The Parts panel, which lists the parts in the selected sub-category. The Parts panel contains the following buttons to help you work with the parts: Button Description New button. Creates a new part. Refer to the Using the Database Manager to Create a Part section for more information. Edit button. Edits a part. Refer to the Editing a Placed Part (In-Place Edit) section for more information. Delete button. Deletes a part. Rename button. Renames a part. Copy button.
Chapter 4 Working with Parts – Mouse Wheel—If your mouse has a center wheel, you can use it to zoom in and out on the part. – Scroll bars—When the part has been enlarged beyond the borders of the Preview area, scroll bars appear that you can move in the usual manner to locate the desired section of a part.
Chapter 4 Working with Parts 3. Select the category or sub-category where the category is to be copied. The copied category will go under the item you select. 4. Click OK. The category is copied to the location you specified, and the Select destination in database dialog box disappears. Complete the following steps to delete a database sub-category: 1. In the Database panel, select the sub-category to be deleted. 2. Click the Delete button above the Database panel.
Chapter 4 Working with Parts Adding Parts using the Database Manager Complete the following steps to add parts from the design to the database using the Database Manager: 1. In the Database panel, select the category (within the User or Corporate Database) you want to add the part to. 2. Click the Add button above the Database panel. The Add new parts to database dialog box appears.
Chapter 4 Working with Parts If you selected multiple parts, you can save them to the database as one item. When a part that has been saved to the database in this manner is placed on the workspace, it will become separate items again, including any parts and traces that were in the original selection. Note Merging and Converting Databases You can merge parts from one database into another or convert parts that you created in your old User Database to Ultiboard 10 format. Details follow.
Chapter 4 6. Working with Parts Click Start. A dialog box displays with the following options: • Auto-Rename—Parts will be saved with modified names in the new database. • Overwrite—Parts will overwrite new parts with the same name. • Ignore—Parts with the same name will nobe be merged. 7. Select the desired option and click OK. The parts from the source database are merged into the target database, based on the option selected above. 8. Click Close to close the Database Merge dialog box.
Chapter 4 Working with Parts 7. 8. NI Ultiboard User Manual Select one of the following options: • Auto-Rename...—Imports and automatically renames the duplicate parts. • Overwrite...—Replaces the Ultiboard 10 parts with your old parts. • Ignore...—Does not import parts with duplicate names. Click OK. 4-48 ni.
Working with Traces and Copper 5 The following sections describe how to work with traces and other copper elements in Ultiboard. Some of the described features may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition. Placing Traces You can place the traces on the board by using one of the methods explained here, or by using the methods described in Chapter 7, Autorouting and Autoplacement.
Chapter 5 Working with Traces and Copper operations on traces, be sure to select either the appropriate segment or, if you wish, the whole trace. Clearance is the distance from the edge of the board and around pads and traces that is to be kept free of any other elements. Trying to run a trace through a clearance, or trying to place a part so that a pad is put within a clearance, for example, results in an error. The board outline clearance is defined in the PCB Properties dialog box.
Chapter 5 Working with Traces and Copper 6. Click the next pad in the net. Continue in this way from pad to pad, clicking the points on the board where you must route the trace around obstacles. 7. When you place the final trace in the net, cancel trace placement by either pressing twice or by right-clicking and selecting ESC from the pop-up menu that appears twice.
Chapter 5 Working with Traces and Copper 4. Move the mouse pointer to the next pad in the net. The trace follows the pointer, routing itself around most obstacles. 5. When you place the final trace in the net, cancel trace placement by either pressing or by right-clicking. Use to widen/narrow the trace. You can also change the trace width during routing by typing the desired value in the Draw Settings toolbar. Otherwise, trace size is determined from the net settings.
Chapter 5 Working with Traces and Copper Use to widen/narrow the trace. You can also change the trace width during routing by typing the desired value in the Draw Settings toolbar. Otherwise, trace size is determined from the net settings. If you attempt to change to a net width that is too big (DRC errors appear), the trace width will not change. Tip Placing a Bus Use to connect multiple traces between multi-pinned devices such as ICs. The procedure below uses the following example.
Chapter 5 Working with Traces and Copper 3. Move the cursor toward the bus’s destination pins and double-click to complete copper placement. Working with Density Bars Density bars use color to indicate the density of pins and pads at cross-sections of your board. The higher their density at any given cross-section, the more difficulty you will have routing traces through that section of the board and the more copper is used in that area.
Chapter 5 Working with Traces and Copper Working with Keep-in/Keep-out Areas A Keep-in area is a polygon that you set so that when objects are moved outside of it, a DRC error is generated. Conversely, a Keep-out area generates a DRC error when objects are moved into it. Placing Keep-in/Keep-out Areas The Keep-in/Keep-out properties dialog box lets you place a polygon that will act as either a Keep-in or a Keep-out area. By default, a Keep-out is placed.
Chapter 5 Working with Traces and Copper 4. 5. Optionally, click on one of the following checkboxes in the Advanced options area and then click the Options button when it becomes active: • Net Group—Displays the Select Groups dialog box where you select the net groups to which you wish to apply the Keep-in/out. • Part Height—Displays the Part Height Ranges dialog box where you enter the height of parts to which you wish the Keep-in/out area to apply.
Chapter 5 Working with Traces and Copper Equi-Spacing Traces This option lets you set the spacing between traces to be equal. Complete the following steps to equi-space traces: 1. Select two traces that surround at least one other trace, as shown in the figure below. 2. Select Tools»Equi-space Traces. The spacing between the traces is made equal, as shown in the example in the figure below.
Chapter 5 Working with Traces and Copper To delete a trace that you have just placed, choose Edit»Undo Place Trace Segment. Complete the following steps to delete an existing trace: 1. Select the trace. 2. Choose Edit»Delete. Or 1. Select the trace. 2. Press the DELETE key.
Chapter 5 Working with Traces and Copper Placing Powerplanes Powerplanes are copper areas that cover the entire plane. Complete the following steps to place a powerplane: 1. In the Layers tab, select the layer to be used as a powerplane. 2. Choose Place»Powerplane. The Choose Net and Layer for Powerplane dialog box appears. 3. Specify the Net and Layer for the powerplane. 4. Click OK.
Chapter 5 Working with Traces and Copper Converting a Copper Shape to an Area Use to convert a copper shape to a polygon that supports voiding around unconnected nets. Complete the following steps to shape a copper shape to an area: 1. Select a copper shape in your workspace. The figure below shows a coppers shape (green) that straddles two pins and traces. 2. Select Design»Shape to Area. The copper is cut out to avoid the other elements within its area, as in the example shown below.
Chapter 5 Working with Traces and Copper Adding and Removing Teardrops A teardrop is a flair that you can add to a trace where the trace connects to a pad. This is typically used with very small sized traces, to prevent possible breakage in the copper between the trace and the pad. Complete the following steps to add teardrops: 1. Select Design»Add Teardrops. The Teardrops dialog box displays. 2. Select the Units for the teardrop length. 3.
Chapter 5 Working with Traces and Copper 3. Optionally, change the Units (of measurement). 4. In the Clearances box, enter the desired clearance of the selected object to traces in the To Trace field. The Attributes tab is where you edit the attributes of the selected copper element. Refer to the Attributes section of Chapter 4, Working with Parts, for more information. The Position tab is where you change the layer the selected copper element is on, from the Layer drop-down list.
Chapter 5 2. Working with Traces and Copper In the Remove Islands box, set the parameters to remove islands using the following (an island is a section of copper within the copper area that is not connected to any other copper): • Smaller than checkbox—Enable the checkbox and enter the desired setting. Any copper islands with length and width smaller than this value are automatically deleted. • Not connected to outer edge checkbox—Any unconnected copper within the coppe area will be removed.
Chapter 5 Working with Traces and Copper Depending on your setting in the PCB Design tab of the Preferences dialog box, vias associated with a trace may be deleted when the trace is deleted. Note Viewing and Editing Via Properties Via properties consist of five tabs: Attributes, General, Via, Layer Settings and Thermal Relief. The Attributes tab allows you to edit the properties of the selected via. Refer to the Attributes section of Chapter 4, Working with Parts, for more information.
Chapter 5 Working with Traces and Copper 3. In the Autorouter Settings box, select either Via is Fixed or Via can be Moved (during autorouting). 4. In the Solder Mask box, select the following as desired: • Top checkbox—Enable to place a solder mask on the top of the PCB. • Bottom checkbox—Enable to place a solder mask on the bottom of the PCB. If the via that you have selected is a micro via, the Micro Via tab displays instead of the Via tab.
Chapter 5 Working with Traces and Copper Placing SMD Fanouts The Fanout SMD command attaches vias to each pin of either a selected surface mount device (SMD) or all SMDs on the board. Complete the following steps to place SMD fanouts: 1. Optionally, select the part(s) to which you wish to apply fanouts, as in the example shown in the figure below. 2. Select Design»Fanout SMD. The Fanout Options dialog box appears. 3. In the Fanout Type box, select one of: 4.
Chapter 5 5. Working with Traces and Copper Click Start Fanout. The Fanout Options dialog box disappears and the fanout vias are placed on the design, as circled in the figure below.
Chapter 5 Working with Traces and Copper Complete the following steps to find a net in the design: 1. Click the net in the list to select it. 2. Click the Find the selected net button. The view zooms in on the net and selects it. Complete the following steps to highlight a selected net: 1. Click the net in the list to select it. 2. Click the Highlight selected nets button. The selected net is highlighted on the design.
Chapter 5 Working with Traces and Copper Complete the following steps to add new pins to a locked net: 1. Select the desired net in the Net drop-down list. 2. Click the Lock Net button to unlock the net. 3. Add the necessary pins and connections. Refer to the Adding a Net section for more information. 4. Route the new net. 5. Click the Lock Net button. To show or hide a ratsnest, click the Show/Hide Ratsnest button.
Chapter 5 Working with Traces and Copper The remainder of this section uses the example shown in the figure below. The parts shown are not connected any net. 3. NI Ultiboard User Manual Click the Add pins button and click the desired pin in the workspace. Continue until all pins for the net are listed in the Pins area. 5-22 ni.
Chapter 5 Working with Traces and Copper Or Click Add. The Add Pins to the Net dialog box displays. Highlight the pins to be added and click Add. The dialog box closes and the Net edit dialog box shows the added pins in the list of pads for the displayed net. 4. © National Instruments Corporation Click OK in the Net edit dialog box. The dialog box closes and the net information is added in the workspace, including its ratsnest and force vectors.
Chapter 5 Working with Traces and Copper Complete the following steps to change a net’s topology. NI Ultiboard User Manual 1. Select Tools»Netlist Editor and select the net from the Net drop-down list in the Net edit dialog box. 2. Click either Shortest, Daisy chain or Star in the Topology area and click OK. The ratsnest placement on the workspace changes to reflect the new topology. • Shortest—When connections are made, the shortest distance possible will be maintained.
Chapter 5 Working with Traces and Copper net, then the pin below the reference point will become the source. Refer to the figure below for an example. Renaming a Net Complete the following steps to rename a net: 1. Select Tools»Netlist Editor and select the desired net from the Net drop-down list in the Net edit dialog box. 2. Click Rename in the Net edit dialog box. You are prompted for the new net name. 3. Type a name for the net. 4. Click OK to save the new name.
Chapter 5 Working with Traces and Copper Deleting a Pin from a Net Complete the following steps to delete a pin from a net: 1. Select Tools»Netlist Editor, click the Pins tab and select the desired net from the Net drop-down list in the Net edit dialog box. 2. Highlight the pin you wish to delete in the list in the Pins tab and click Remove. The pin disappears from the list of pins for the net displayed. Note There is no deletion confirmation. 3. Click OK to close the Net edit dialog box.
Chapter 5 Working with Traces and Copper Setting Miscellaneous Net Parameters Complete the following steps to set miscellaneous parameters for a net: 1. Select Tools»Netlist Editor and select the desired net from the Net drop-down list in the Net edit dialog box. 2. Click on the Misc tab. 3. In the Routing Layers area: • Select layers to use for routing copper for the selected net. If the selected net is part of a net group, the Use Group Settings checkbox will be checked.
Chapter 5 Working with Traces and Copper Setting Via Parameters Complete the following steps to edit via information for a net: 1. Select Tools»Netlist Editor and select the desired net from the Net drop-down list in the Net edit dialog box. 2. Click on the Via tab. 3. Set desired Via Drill Diameter and Via Pad Diameter and click OK. Highlighting a Net Complete the following steps to highlight a net: 1. Click on a segment of the net that you wish to highlight. 2.
Chapter 5 5. Working with Traces and Copper Select the net to use for the shield in the Shield net area: • Use Net Settings—Select to use the shield set in the Spreadsheet View (also set in the Net edit dialog box). • GND—Select to activate the drop-down list, where you can pick the net to use for the shield. 6. In the On DRC Error area, select the action to take when a DRC error occurs. 7. In the On Other Failures area, select the action to take when other errors occur. 8.
Chapter 5 Working with Traces and Copper Net Bridges The net bridge functionality permits connections between different nets (for example, digital and analog grounds) without losing the properties of either net. Creating a Net Bridge Complete the following steps to create a net bridge: NI Ultiboard User Manual 1. Select Tools»Database»Database Manager. 2. Click the Create New Part button in the Parts area, select Net bridge and click OK. The Net Bridge Edit Layer displays on your workspace. 3.
Chapter 5 Working with Traces and Copper 7. Close the Net Bridge Edit Layer, and when prompted, Click Save. 8. The following dialog box appears. Enter the name for the new netbridge (Netbridge2 in the following example): 9. Click OK.
Chapter 5 Working with Traces and Copper Placing a Net Bridge This example connects two traces - one is on net “DGND” and the other is on net “GND”. Complete the following steps to place a net bridge: NI Ultiboard User Manual 1. Select Place»Net Bridge. The Place Net Bridge dialog box appears. 2. Click Select Net Bridge From Database. The Get a part from the database dialog box appears. 3. Select the desired net bridge in the Available Parts area and click OK.
Chapter 5 Working with Traces and Copper Copying a Copper Route You can copy the routing of traces between two identical parts groups that have been set up using the Group Replica command. Complete the following steps to copy copper routing between groups: 1. Create two identical part groups. Refer to the Replicating a Group section of Chapter 4, Working with Parts, for more information. 2. Route the traces for one of the groups. In the example below, Part Group A consists of U7 and U8.
Chapter 5 Working with Traces and Copper 3. Select Design»Copy Route. The Copy route dialog box appears. 4. Select the group you have already routed in the Source group field, and the group you wish to have the same routing in the Destination group field and click OK. The routing is duplicated for the destination group. Swapping Pins and Gates Pin and gate swapping are done between like pins and gates to reduce the amount of copper needed to route a given net.
Chapter 5 3. Working with Traces and Copper Click on the second pin to complete the action. Error messages will display if the selected pins cannot be swapped, or if there is no PINGROUP information for a pin. Note Swapping Gates This feature allows you to swap similar gates, and works for the following, which are set in the Pin & Gate Swapping Settings area of the Design Rules tab of the PCB Properties dialog box: • Internal Gates Only—Allows gate swapping in the same IC only.
Chapter 5 Working with Traces and Copper The following design is used in this example: Complete the following steps to swap gates between parts: NI Ultiboard User Manual 1. Select Design»Swap Gates. The workspace changes to reflect the gates. 2. Select the first gate that you wish to swap by clicking on the corresponding letter. 5-36 ni.
Chapter 5 3. © National Instruments Corporation Working with Traces and Copper Click on the letter corresponding to the gate with which you want to exchange the gate you selected above. The ratsnest changes to reflect the swap.
Chapter 5 Working with Traces and Copper Automatic Pin/Gate Swapping This feature lets you swap pins and/or gates after moving part(s) on the workspace. For this feature to function, you must allow pin/gate swapping in the Spreadsheet View, and in the Design Rules tab of the PCB properties dialog box. Note Complete the following steps to swap pins and gates automatically after a part move: 1. Move desired parts on the workspace. 2. Select Design»Automatic Pin Gate Swap.
Chapter 5 Working with Traces and Copper Real-Time Pin/Gate Swapping This feature allows you to swap pins and/or gates automatically in real-time as you move parts on the workspace. Note For this feature to function, you must allow pin/gate swapping in the Spreadsheet View, and allow real-time swapping in the Design Rules tab of the PCB properties dialog box.
6 PCB Calculators The following sections explain how to use Ultiboard’s PCB Calculators. Some of the described features may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition. PCB Transmission Line Calculator To control reflections on high-speed PCBs, it is necessary to make the traces appear as if they are transmission lines.
Chapter 6 PCB Calculators The PCB Transmission Line Calculator supports: • Microstrip Trace Calculations. • Embedded Microstrip Trace Calculations. • Centered Stripline Trace Calculations. • Asymmetric Stripline Trace Calculations. • Dual Stripline Trace Calculations. Microstrip Trace Calculations Complete the following steps to perform microstrip trace calculations: NI Ultiboard User Manual 1. Select Tools»PCB Transmission Line Calculator. 2. Select Microstrip in the Type drop-down list.
Chapter 6 PCB Calculators Microstrip Equations The equations used to perform the microstrip calculations are: Z0 = 87/(sqrt(Er + 1.41)) * ln(5.98*H/(0.8*W+T)) Tpd = 58.35247*sqrt(Er+1.41) C0 = Tpd/Z0 L0 = C0*Z0*Z0 Embedded Microstrip Trace Calculations Complete the following steps to perform embedded microstrip trace calculations: 1. Select Tools»PCB Transmission Line Calculator. 2. Select Embedded Microstrip in the Type drop-down list. 3.
Chapter 6 PCB Calculators Embedded Microstrip Equations The equations used to perform the embedded microstrip calculations are: Z0 = 56*ln(5.98*H/(0.8*W+T))/sqrt(Er*(1-exp(-1.55*H1/H))) Tpd = 84.66667*sqrt(Er*(1-exp(-1.55*H1/H))) C0 = Tpd/Z0 L0 = C0*Z0*Z0 Centered Stripline Trace Calculations Complete the following steps to perform centered stripline trace calculations: NI Ultiboard User Manual 1. Select Tools»PCB Transmission Line Calculator. 2. Select Centered Stripline in the Type drop-down list.
Chapter 6 PCB Calculators Centered Stripline Equations The equations used to perform the centered stripline calculations are: Z0 = 60*ln(4*(2*H+T)/(0.67*3.1415926*(0.8*W+T)))/sqrt(Er) Tpd = 84.66667*sqrt(Er) C0 = Tpd/Z0 L0 = C0*Z0*Z0 Asymmetric Stripline Trace Calculations Complete the following steps to perform asymmetric stripline trace calculations: 1. Select Tools»PCB Transmission Line Calculator. 2. Select Asymmetric Stripline in the Type drop-down list. 3.
Chapter 6 PCB Calculators Assymetric Stripline Equations The equations used to perform the asymmetric stripline calculations are: Z0 = (1-H/(4*H1))*80*ln(4*(2*H+T)/(0.67*3.1415926*(0.8*W+T)))/sqrt(Er) Tpd = 84.66667*sqrt(Er) C0 = Tpd/Z0 L0 = C0*Z0*Z0 Dual Stripline Trace Calculations Complete the following steps to perform centered stripline trace calculations: NI Ultiboard User Manual 1. Select Tools»PCB Transmission Line Calculator. 2. Select Dual Stripline in the Type drop-down list. 3.
Chapter 6 PCB Calculators Dual Stripline Equations The equations used to perform the dual stripline calculations are: Z0 = 30*( ln(8*H/(0.67*3.1415926*(0.8*W+T)))+ ln(8*(H+C)/(0.67*3.1415926*(0.8*W+T))))/sqrt(Er) Tpd = 84.66667*sqrt(Er) C0 = Tpd/Z0 L0 = C0*Z0*Z0 PCB Differential Impedance Calculator To control reflections on high-speed PCBs, it is necessary to make the traces appear as if they are transmission lines.
Chapter 6 PCB Calculators You can use the PCB Differential Impedance Calculator to calculate the following parameters for differential pairs: • Characteristic Impedance (Zo). • Per unit length Capacitance (Co). • Per unit length Inductance (Lo). • Propogation Delay (tpd). • Differential Impedance (Zdiff). The PCB Differential Impedance Calculator supports: • Microstrip Calculations. • Embedded Microstrip Calculations. • Centered Stripline Calculations. • Asymmetric Stripline Calculations.
Chapter 6 4. PCB Calculators Click Calculate. Results of the calculation appear in the Calculation Results area. They also appear in the Results tab of the Spreadsheet View. Note If you chose User Defined Zo in the previous step, the Per Length Unit and the Differential Impedance are the only values that appear in the Calculation Results area of the PCB Differential Impedance Calculator dialog and the Results tab when you click Calculate. 5.
Chapter 6 PCB Calculators • Dielectric Thickness (H)—Refer to the figure below. • Trace Thickness (T)—Refer to the figure below. • Trace Width (W)—Refer to the figure below. • Trace Spacing (S)—Refer to the figure below. • Relative Permittivity (epsilon r)—Refer to the figure below. Or If you wish to define the Characteristic Impedance (Zo) yourself, click User Defined Zo and edit the following fields as desired: 4.
Chapter 6 PCB Calculators Embedded Microstrip Differential Impedance Equations The equations used to perform the embedded microstrip differential impedance calculations are: Z0 = 56*ln(5.98*H/(0.8*W+T))/sqrt(Er*(1-exp(-1.55*H1/H))) Tpd = 84.66667*sqrt(Er*(1-exp(-1.55*H1/H))) C0 = Tpd/Z0 L0 = C0*Z0*Z0 Zdiff = 2*Z0*(1-0.48*exp(-0.96*S/H1)) Centered Stripline Calculations Complete the following steps to perform centered stripline differential impedance calculations: 1.
Chapter 6 PCB Calculators 4. Click Calculate. Results of the calculation appear in the Calculation Results area. They also appear in the Results tab of the Spreadsheet View. Note If you chose User Defined Zo in the previous step, the Per Length Unit and the Differential Impedance are the only values that appear in the Calculation Results area of the PCB Differential Impedance Calculator dialog and the Results tab when you click Calculate. 5.
Chapter 6 3. PCB Calculators In the Input Data area, edit the following fields as desired: • Input Length Unit—Select mils or millimeters. • Dielectric Height (H1)—Refer to the figure below. • Dielectric Height (H)—Refer to the figure below. • Trace Thickness (T)—Refer to the figure below. • Trace Width (W)—Refer to the figure below. • Trace Spacing (S)—Refer to the figure below. • Relative Permittivity (epsilon r)—Refer to the figure below.
Chapter 6 PCB Calculators Asymmetric Stripline Differential Impedance Equations The equations used to perform the asymmetric stripline differential impedance calculations are: Z0 = (1-H/(4*H1))*80*ln(4*(2*H+T)/(0.67*3.1415926*(0.8*W+T)))/sqrt(Er) Tpd = 84.66667*sqrt(Er) C0 = Tpd/Z0 L0 = C0*Z0*Z0 Zdiff = 2*Z0*(1-0.347*exp(-2.9*S/(H+H1+T))) NI Ultiboard User Manual 6-14 ni.
7 Autorouting and Autoplacement There are a number of autorouting and autoplacement tools that vary depending on your edition of Ultiboard. These tools offer advanced autoplacement with state-of-the-art autorouting for optimal layout of your printed circuit boards, and are fully integrated with Ultiboard. For details on the autorouting and autoplacement features found in your edition of Ultiboard, refer to the release notes.
Chapter 7 Autorouting and Autoplacement Note This is only active when an unconnected pad corresponding to that net is selected. Autoroute»Autoroute Selected Buses Use to autoroute selected buses. Refer to the Autorouting buses section for more information. Autoroute»Start Optimization Use to optimize the placement of traces. Refer to the Optimization section for more information. Autoroute»Autoroute/place Options Use to set up router and placer functions.
Chapter 7 Autorouting and Autoplacement The autoplacer places parts as clusters. These clusters are generated by grouping a multi-pin part with a series of connected parts, each of which has fewer than four pins. Each cluster is then assigned a placement priority. By arranging parts into clusters, the autoplacer can place together those parts that have multiple connections. Block capacitors, which are connected to power signals, are always excluded from clusters.
Chapter 7 Autorouting and Autoplacement connections. 10 prioritizes parts with the highest ratio of connections to total pins. A high part pin factor value usually results in a better distribution of nets than a low value. However, high values may cause excessive placement area fragmentation on high-density layouts by placing small parts prematurely and preventing you from placing larger ones later on. • 5.
Chapter 7 6. Caution Autorouting and Autoplacement • SMD Rotation Mode—Used to set amount by which surface-mount parts can be rotated during autoplacement. Select one of None, for no rotation; 90 Deg, for 90 clockwise rotation of all autoplaced SMD parts; 0 or 90 Deg, to have parts either not rotate, or rotate 90 clockwise; 90 Deg Steps, to have parts rotate either 90, 180, or 270 degrees clockwise. • Global Part Spacing—Enter the minimum allowed space between parts.
Chapter 7 Autorouting and Autoplacement • Use smaller Keep-out or Keep-in areas. Often, a PCB with Keep-in areas can be designed with an equivalent set of Keep-out areas, or vice-versa. Whenever possible, choose a design strategy that minimizes the total area of the board covered by these Keep-in or Keep-out areas since each area radically decreases the autoplacement algorithms’ effectiveness. • With very dense boards, the last few parts may need to be hand-placed.
Chapter 7 Autorouting and Autoplacement Understanding the Four Fundamental Routing Functions The following sections describe the four fundamental routing functions used by Ultiboard. Router Preprocessing Before routing begins, Ultiboard analyzes the entire board, considering trace widths, clearances, Keep-in, and Keep-out areas.
Chapter 7 Autorouting and Autoplacement unless you achieve poorer routing results than you expect. When changing cost factors, even slight adjustments can have large effects on routing success, either improving or worsening the results. Optimization The optimizer is usually applied after the autorouter achieves 100% completion. It eliminates unnecessary vias and smooths wire bends to reduce manufacturing costs. It also routes any remaining open connections.
Chapter 7 Autorouting and Autoplacement To perform a full autoroute, choose Autoroute»Start/Resume Autorouter. Ultiboard begins routing your board and displays its progress in the status line. When the process is complete the results are displayed in the Results tab of the Spreadsheet View. Interactivity Ultiboard provides complete interactivity, letting you stop the routing process as desired to manually place items and then continue autorouting when ready.
Chapter 7 Autorouting and Autoplacement Complete the following steps to autoroute selected bus(es): 1. Select Autoroute»Autoroute Selected Buses. The Bus autorouting dialog box displays. 2. Select the desired buses to route in the Defined bus groups area and click OK. The buses are routed as in the following example. Placing Automatic Test Points You can automatically place a test point on each net on your design. Note Testpoints may be placed either before or after autorouting the entire board.
Chapter 7 Autorouting and Autoplacement 4. The Automatic Testpoint Placement Setup dialog box disappears and one test point is placed on or near each net on your board. If placed near an existing net, the test point will be automatically connected. 5. Results of testpoint placements, including a list of any nets which the router could not connect, will appear in the Results tab of the Spreadsheet View. You can click on an error to go to the unrouted testpoint.
Chapter 7 Autorouting and Autoplacement Caution • Pin Contact Mode—Select Allow Pin Corners to allow traces to connect to pins diagonally. • Place Vias Under SMD Pads—Select Yes or No as desired. • Auto Adjust Trace Width checkbox—Enable to allow the router to narrow the trace to its minimum width as set in the Nets tab of the Spreadsheet View or the Width tab of the Net edit dialog box. • Fanout BGA Parts checkbox—Attaches vias to each pin of all BGA (Ball Grid Array) parts.
Chapter 7 Autorouting and Autoplacement Complete the following steps to set up cost factor parameters: 1. Select the Cost Factors tab in the Routing Options dialog box. 2. Edit one or more of the following fields in the Routing and Optimization area: • Via Cost Factor—A high via cost factor results in fewer vias than a low via cost factor, but also results in relatively complex circuit traces.
Chapter 7 Autorouting and Autoplacement 4. 5. Caution Edit one or both of the following fields in the Optimization area: • Change Direction Cost Factor—A high direction cost factor limits the number of trace corners the optimizer creates. A low factor allows frequent changes in routing direction. • Equi-Space Trace Cost Factor—A high value here indicates that traces will be spread out more during optimization, with a resultingly higher cost.
Chapter 7 • Caution Autorouting and Autoplacement Distance-2 (2 Grid) Cost Factor—Controls the use of channels left by ripped-up traces in the far distance (2 or more grid points, trace-to-trace). A high value results in infrequent use of these channels, forcing relatively more global changes during rip-up and retry routing. 3. Optionally, enable the Memory Cleanup During Routing checkbox in the Router Housekeeping area to purge the memory of unneeded information. 4.
Chapter 7 Autorouting and Autoplacement Routing Options: Bus Autorouting Tab To autoroute buses, the topology for the nets, as set in the Net edit dialog box, or the Spreadsheet View, must be set to either Daisy chain or Star and the nets must be part of a Bus Group as set in the Edit Groups dialog box. You can also add new Bus Groups from the Bus Autorouting tab in the Routing Options dialog box. Complete the following steps to set Ultiboard bus routing options: Caution 1.
Chapter 7 Autorouting and Autoplacement Strategies to Achieve Better Routing Results Speed and completion may be trade-offs. Many of the suggestions for routing completion will greatly increase the time needed to complete routing. While it may be tempting to try to guarantee completion by using all possible completion tricks for all layouts, many non-dense boards can be completely routed without them, and they will be routed much faster. Set alternating layer biases.
8 Preparing for Manufacturing/Assembly The following sections explain the basic functions you need to perform to prepare your board for manufacturing. Some of the described features may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition. Placing and Editing Text Text can be placed anywhere on the design and on any layer, regardless of what element is selected.
Chapter 8 Preparing for Manufacturing/Assembly 4. Optionally, in the Next Label area: • Increment—Enable to increase a number that you placed at the end of the text with each successive placement of that text. You must also enter a value in Step Size. For example, if you enable this checkbox and enter “1” in Step Size, and the Value you entered was “Resistor1”, the first placement of the text will say “Resistor1”, the second will say “Resistor2”, the third will say “Resistor3”, and so on.
Chapter 8 3. Preparing for Manufacturing/Assembly Optionally, to re-size the selection frame: • Move the cursor to one of the sizing handles. • Drag the cursor to re-size the selection frame. 4. Click on the copy button at the top left corner of the selection frame. The image inside the selection frame is copied to the system clipboard. 5. Click on the x at the top right corner of the selection frame to close it. 6.
Chapter 8 Preparing for Manufacturing/Assembly Complete the following steps to pin a comment to a part or the workspace: 1. Double-click on the Comment layer in the Design Toolbox to make it the active layer. 2. Select Place»Comment. The Comment dialog box appears. 3. If desired, enable the Show Comment checkbox to show the contents of the comment on the design. 4. Type the comment in the area below the Show Comment checkbox. 5.
Chapter 8 6. Preparing for Manufacturing/Assembly In the Size area: • Auto-Resize checkbox—Enable to have the size of the displayed comment automatically resized to fit the text. Disable if you wish to set the size of the displayed comment by typing values into the Width and Height fields. 7. In the Font area, set the font Name, Style and Size as desired. 8. Click OK to close the dialog and double-click at the desired location on the design to place the comment.
Chapter 8 Preparing for Manufacturing/Assembly 4. If you only want to renumber parts you selected prior to opening this dialog box, select the Change selected parts only option. 5. To apply your changes and keep the dialog box open, click Apply. To apply your changes and close the dialog box, click OK. Backannotation to Multisim Backannotation is a highly automated process which ensures that modifications made to an Ultiboard design are transferred to the board’s schematic in Multisim.
Chapter 8 Preparing for Manufacturing/Assembly Complete the following steps to miter the corners of traces prior to manufacturing: 1. Optionally, select the traces to which you want mitering to apply. 2. Choose Design»Corner Mitering. The Corner Mitering dialog box appears. 3. To apply the changes to just the selected traces, enable the Current Selection option. To apply the changes to the whole design, enable the Whole Design option. 4.
Chapter 8 Preparing for Manufacturing/Assembly Manually Re-Running the Design Rules and Netlist Check The design rules and netlist check normally runs automatically, but you may want to force a final check of the board's integrity prior to saving or exporting the design. To do this, select Design»Netlist and DRC Check. The results of the check appear in the Results tab of the Spreadsheet View.
Chapter 8 Preparing for Manufacturing/Assembly It is important to talk to your production house and identify all the files and formatting information they need to support their manufacturing process.
Chapter 8 Preparing for Manufacturing/Assembly The new setting uses the same properties as the Default setting, or the setting that was last loaded. Refer to the Viewing and Editing Export Properties section for information about changing the properties stored in the new setting. Complete the following steps to delete an export setting: 1. Choose File»Export. The Export dialog box appears. 2. Select the setting to be deleted from the Export settings drop-down list. 3. Click Delete.
Chapter 8 Preparing for Manufacturing/Assembly • Oversize box—Define the parameters for solder mask and solder paste. • Options box—Select the desired options. Setting DXF Properties The DXF export settings dialog box allows you to select the layers to be exported and the units of measurement to be used: • Available layers list—Select the layers to export in this list and click the -> button to move them to the Layers to process list. • File Units box—Choose the units of measurement.
Chapter 8 Preparing for Manufacturing/Assembly Complete the following steps to change the SVG export properties: 1. Select Scalable Vector Graphics in the Export dialog box and click Properties. 2. In the SVG File Format box, select one of: • Compressed svg—The SVG file will be compressed when it is exported. • Uncompressed svg—The SVG file will not be compressed when it is exported. 3. Enter the Minimum stroke width in the SVG Options box.
Chapter 8 Preparing for Manufacturing/Assembly Working with Parts Centroids Properties The Parts Centroids dialog box provides a list of all parts on the boards and their coordinates, and includes facilities for sorting the information displayed: • Columns—Click column headers in the list to sort the columns. • File type box—Select any of TXT, CSV, and HTML. • Units box—Select the unit of measurement.
Chapter 8 Preparing for Manufacturing/Assembly Working with Layer Stackup Properties A Layer Stackup Report shows you a board’s layers, the layer type (ground, power, signal or unassigned) and the types of vias that are between layers. The Layer Stackup Report dialog lets you set which file types to export when you run a Layer Stackup Report. Exporting the Desired File Complete the following steps to export a file: Note 1. Select File»Export to display the Export dialog box. 2.
Chapter 8 Preparing for Manufacturing/Assembly Once you have more than one layer selected, you can choose to print layers on separate sheets. You can also choose to print a header at the top of each page, containing the design name, date, and layer name. Finally, you can use the arrows to change the order in which layers will be printed. 8. When you have finished setting the print parameters, click Print. Complete the following steps to print a 3D image of your design: 1. Select Tools»View 3D.
Chapter 8 Preparing for Manufacturing/Assembly If you elect to enlarge the size of your printout in the Zoom Options area, each layer will be tiled onto as many pages as required to print the whole layer. NI Ultiboard User Manual 8-16 ni.
Viewing Designs in 3D 9 Ultiboard allows you to see what the board looks like in three dimensions (3D) at any time during the design. The following sections explain how to set up the options for 3D viewing, how to view the board in 3D, and how to manipulate the view. Some of the described features may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition.
Chapter 9 Viewing Designs in 3D To close the 3D view, right-click on the 3D view in the Projects tab and choose Close Window from the context menu. If you loaded a file from Ultiboard 2001, before you can use the 3D view you must use Tools»Update Shapes. The 3D appearance of individual parts is controlled by the 3D properties of those parts. Refer to the Viewing and Editing Part Properties section of Chapter 4, Working with Parts, for more information.
Chapter 9 3. Viewing Designs in 3D Continue holding the button and move the pointer as follows: • to the bottom of the screen to view more of the top of the board. • to the top of the screen to view the edge and then the underside of the board. • to the left or right to view the board from either end. Complete the following steps to pan the 3D view: 1. Hold down your mouse wheel. The pointer becomes a four-headed arrow. 2. Move the pointer in any direction.
Chapter 9 Viewing Designs in 3D Showing an Object’s Height While in the 3D view, you can show an object’s height, as shown in the figure below. Complete the following steps to show an object’s height: 1. Select Tools»Show or Hide Height. 2. Click the cursor on a 3D part. A callout with the part’s height appears. 3. Repeat on as many parts as desired. To hide a part’s height, click on the part. The callout with the height disappears. To rotate or magnify the board, select Tools»View 3D Position.
Chapter 9 Viewing Designs in 3D The figure below shows the normal 3D view of a sample PCB. The figure below shows the internal 3D view of the same PCB. Note Internal View options are set in the 3D Options tab of the Preferences dialog box. Refer to the 3D Options Tab section of Chapter 1, User Interface, for more information. Exporting to 3D DXF Ultiboard can export a 3D DXF file for your design. Complete the following steps to export a design’s 3D properties: 1.
Chapter 9 Viewing Designs in 3D Exporting to 3D IGES 3D IGES (Initial Graphics Exchange Specification) is a file format for the exchange of CAD information (both 2D and 3D). A 3D IGES file contains surface information and details of a part. Complete the following steps to export a design’s 3D IGES properties: NI Ultiboard User Manual 1. Select File»Export to display the Export dialog box. 2. Highlight 3D IGES and click Properties. The IGES export settings dialog box appears. 3.
Using Mechanical CAD 10 Ultiboard’s mechanical CAD function can be used to design enclosure boxes, front panels, or any other mechanical part associated with your PCB design. Mechanical CAD functionality in Ultiboard takes two forms: • You can create multi-layer mechanical CAD design files. • You can have mechanical CAD layers as part of your PCB design files. Design files can include up to 10 mechanical CAD layers.
Chapter 10 Using Mechanical CAD Creating Mechanical CAD Design Files To create a new mechanical CAD design, you can either use the new design that appears when you create a mechanical CAD file, or you can create a new design and assign it to an existing file. To create a new design and assign it to an existing file: 1. Open the file that the new design is to be added to. 2. Choose File»New Design. The New Design dialog box appears. 3. Type the design name in the Design name field. 4.
Chapter 10 Using Mechanical CAD Importing a DXF File Complete the following steps to import a DXF file into a mechanical CAD design: 1. Choose File»Import»DXF. A standard file selector appears. 2. Navigate to the correct location for the .dxf file, select it and click OK. Setting Mechanical CAD Properties and Options Setting Mechanical CAD Properties To set mechanical CAD properties: Choose Edit»Properties. Or Right-click on an empty area of the design and choose Properties from the context menu.
Chapter 10 Using Mechanical CAD Controlling Workspace Elements for Mechanical CAD The General tab allows you to control whether or not invisible attributes or cross hairs are shown in normal view, and options for full screen view. This tab also allows you to have Ultiboard load your last project automatically, and to have Ultiboard automatically save your project at specified intervals. Complete the following steps to view or change workspace options: 1. Choose Options»Global Preferences.
Chapter 10 9. Using Mechanical CAD In the Auto save settings box: • Enable auto save—Activates the autosave function. When activated, you can also change the time between autosaves in the Time interval (minutes) field. 10. Edit the following as desired: • Minimum control point size—The size of control points on vertices and other objects. • Line width cache size—The number of recently used line widths Ultiboard keeps in memory. Minimum cache size is 5.
Menus and Commands A The following sections contain brief descriptions for the commands in the Ultiboard menus. Some of the described menu items may not be available in your edition of Ultiboard. Refer to the NI Circuit Design Suite Release Notes for a list of the features in your edition. File Menu The subjects in this section describe the commands found in the File menu. File»New Design Creates a new design (if a project is open) or project (if no project is open).
Appendix A Menus and Commands File»Save As Saves the current design file with a name and location that you specify in the Save As dialog box. File»Save All Saves all open design files and projects. File»Close Closes the current design file. File»Close Project Closes the current project. File»Close All Closes all open design files and projects. File»Import Use to import an Ultiboard Netlist or DXF file.
Appendix A Menus and Commands File»Print Setup Sets up the printing paramaters required to print the Ultiboard design file. Refer to the Printing your Design section of Chapter 8, Preparing for Manufacturing/Assembly, for more information. This is found in the 3D view only. File»Print Preview Lets you preview the design file before printing. Refer to the Printing your Design section of Chapter 8, Preparing for Manufacturing/Assembly, for more information. This is found in the 3D view only.
Appendix A Menus and Commands Edit»Cut Removes the selected element(s) from the board. The element is placed on the Windows Clipboard and can be pasted again. Edit»Copy Copies the selected elements and stores them on the Windows Clipboard so they can be pasted again. Edit»Paste Pastes the item on the Windows Clipboard to its original layer (regardless of what layer is currently active). Creates new duplicate object(s) without the netlist information.
Appendix A Menus and Commands • Open Trace Ends—Use to delete all open trace ends in the design. Use to clean up the design after design completion. Refer to the Deleting Open Trace Ends section of Chapter 8, Preparing for Manufacturing/Assembly, for more information. • Copper Island—Use to remove copper islands. Refer to the Placing Copper Areas section of Chapter 5, Working with Traces and Copper, for more information. Edit»Find Use to find an element in the design.
Appendix A Menus and Commands Edit»Selection Filter Use these commands to prevent accidentally selecting a particular type of element, for example, selecting a part when you meant to select a trace: • Enable Selecting Parts—When enabled, allows parts to be selected. • Enable Selecting Traces—When enabled, allows traces to be selected. • Enable Selecting Polygons—When enabled, allows polygons to be selected. • Enable Selecting Vias—When enabled, allows vias to be selected.
Appendix A Menus and Commands • Align Top—Aligns the top edges of the selected elements. • Align Bottom—Aligns the bottom edges of the selected elements. • Align Center Horizontal—Shifts the selected elements horizontally so their centers are aligned. • Align Center Vertical—Shifts the selected elements vertically so their centers are aligned. • Align to Coordinate—Displays the Enter coordinate dialog box where you enter new coordinates for the selected element.
Appendix A Menus and Commands View Menu The subjects in this section describe the commands found in the View menu. View»Full Screen Use to fill the screen with the design only (hide menus, toolbars, other windows). Click the Close Full Screen button to return to normal view. View»Redraw Screen Use to refresh the screen. View»Zoom In Use to zoom in to see more details. View»Zoom Out Use to zoom out to see more of the design. View»Zoom Window Use to magnify a selected part of the board.
Appendix A Menus and Commands View»Ruler Bars Use to toggle the ruler bars on and off. Refer to the Using Ruler Bars and Guides section of Chapter 4, Working with Parts, for more information. View»Status Bar Use to toggle the status bar on and off. View»Density Bars Use to toggle the density bars on and off. Refer to the Working with Density Bars section of Chapter 5, Working with Traces and Copper, for more information. View»Birds Eye Use to toggle the Birds Eye View on and off.
Appendix A Menus and Commands • Draw Settings—Use to toggle the Draw Settings toolbar on and off. Refer to the Draw Settings Toolbar section of Chapter 1, User Interface, for more information. • Edit—Use to toggle the Edit toolbar on and off. Refer to the Edit Toolbar section of Chapter 1, User Interface, for more information. • Align—Use to toggle the Align toolbar on and off. Refer to the Align Toolbar section of Chapter 1, User Interface, for more information.
Appendix A Menus and Commands Place»Follow-me Use to place a trace between two selected points. Refer to the Placing a Trace: Follow-me Method section of Chapter 5, Working with Traces and Copper, for more information. Place»Connection Machine Use to place a trace between two pads. Refer to the Placing a Trace: Connection Machine Method section of Chapter 5, Working with Traces and Copper, for more information. Place»Shape Use to place shapes of different types: • Ellipse—Use to place an ellipse.
Appendix A Menus and Commands Place»Graphic»Arc Use to place an arc or a trace, depending on the active layer. Refer to the Placing Shapes and Graphics section of Chapter 4, Working with Parts, and the Placing a Trace: Manual Method section of Chapter 5, Working with Traces and Copper, for more information. Place»Graphic»Bezier Use to place a bezier or a trace, depending on the active layer.
Appendix A Menus and Commands Place»Keep-in/Keep-out Area Use to define a polygon to restrict elements from either exiting or entering the area. Refer to the Working with Keep-in/Keep-out Areas section of Chapter 5, Working with Traces and Copper, for more information. Place»Group Array Box Use to place parts in a grid array. Refer to the Placing a Group Array Box section of Chapter 4, Working with Parts, for more information. Place»Pins Used during In-Place Editing of a part to place a footprint.
Appendix A Menus and Commands Place»Automatic Test Points Use to automatically place a test point on each net on your design. Refer to the Placing Automatic Test Points section of Chapter 7, Autorouting and Autoplacement, for more information. Place»Unplace Parts Use to unplace all non-locked parts. Refer to the Unplacing Parts section of Chapter 4, Working with Parts, for more information. Place»Comment Places a comment on the design.
Appendix A Menus and Commands Design»Polygon Splitter Use to split a copper area or powerplane. Refer to the Splitting Copper section of Chapter 5, Working with Traces and Copper, for more information. Design»Shape to Area Use to cut out areas in a copper shape to avoid other elements within its area. Refer to the Converting a Copper Shape to an Area section of Chapter 5, Working with Traces and Copper, for more information.
Appendix A Menus and Commands Design»Fanout SMD Use to place a via fanout for a SMD part. Refer to the Placing SMD Fanouts section of Chapter 5, Working with Traces and Copper, for more information. Design»Add Teardrops Use to add teardrops to pads. Refer to the Adding and Removing Teardrops section of Chapter 5, Working with Traces and Copper, for more information. Design»Corner Mitering Use to apply corner mitering before production.
Appendix A Menus and Commands Tools Menu The subjects in this section describe the commands found in the Tools menu. Tools»Board Wizard Assists you in creating a board outline. Refer to the Working with the Board Outline section of Chapter 3, Setting Up a Design, for more information. Tools»Part Wizard Assists you in creating a part and adds it directly to the user database. Refer to the Using the Part Wizard to Create a Part section of Chapter 4, Working with Parts, for more information.
Appendix A Menus and Commands Tools»Database»Convert Database Use to update your old User and Corporate databases to Ultiboard 10 format. Refer to the Converting Databases section of Chapter 4, Working with Parts, for more information. Tools»PCB Transmission Line Calculator Use to calculate parameters for typical printed circuit board trace geometries. Refer to the PCB Transmission Line Calculator section of Chapter 6, PCB Calculators, for more information.
Appendix A Menus and Commands Tools»Equi-space Traces Use to equally space selected traces. Refer to the Equi-Spacing Traces section of Chapter 5, Working with Traces and Copper, for more information. Tools»Change Shape Use to substitute a part from the database for the current selected part. Refer to the Replacing Parts section of Chapter 4, Working with Parts, for more information. Tools»Update Shapes Use if you loaded Ultiboard V. 5 files into Multisim and plan to use 3D.
Appendix A Menus and Commands Options Menu The subjects in this section describe the commands found in the Options menu. Options»Global Preferences Displays the Preferences dialog box. Refer to the Setting Preferences section of Chapter 1, User Interface, for more information. Options»PCB Properties Use to define the general parameters of your PCB design. Refer to the Setting PCB Properties section of Chapter 1, User Interface, for more information.
Appendix A Menus and Commands Window»Close All Use to close all open windows. Window»Cascade Use to cascade the open windows, so they are arranged one on top of the next while remaining separately selectable. Window»Tile Horizontal Use to adjust two or more windows so that they sit one on top of the other. Window»Tile Vertical Use to adjust two or more windows so that they sit beside each other.
Appendix A Menus and Commands Help»About Ultiboard Use to display the version numbers of your copy of Ultiboard. Context Menus Depending on the action, the following context sensitive menus display when the right mouse button is clicked: • Select Menu • Right-drag Menu • Place Trace Menu Select Menu When you select an object or objects in a design and then right-click your mouse, a context menu with the following options displays. Cut Removes the selected element(s) from the board.
Appendix A Menus and Commands Quick Layer Toggle Use to toggle between the last copper layer or to the opposite copper layer if the last layer was not copper. Lock Locks the selected elements in place so they cannot be moved. Unlock Unlocks the selected elements. Place Displays a number of elements that you can place on the design. Shape Displays a number of shapes that you can place on the design. Orientation Use these commands to adjust the orientation of parts as they are placed on a design.
Appendix A Menus and Commands Right-drag Menu When you select an area by dragging and releasing the right mouse button, a context menu appears with the following selections. Select all in rectangle Selects all objects in the rectangle that you “drew” by dragging and releasing the right mouse button.
B Archiving Data National Instruments recommends that you regularly back up the files created within the Multisim and Ultiboard components of NI Circuit Design Suite. Additionally, you should back up internal files that store user-created data, such as database components. This section provides information on where to find these files in order to properly back them up. NI Circuit Design Suite stores program and user data in two possible locations.
Appendix B Archiving Data The ProgramData folder is a system folder and thus may be hidden. Complete the following steps to view this folder: 1. Open a standard Windows explorer window. 2. Select Organize»Folder & Search Options. 3. Select the View tab, Show hidden files and folders, OK. Note The default location for the Corporate database can change if the database has been configured to be shared across a network drive. Check the Preferences dialog box to find the location of this database.
Appendix B Archiving Data The user’s configuration file is stored at: C:\Users\\AppData\Roaming\National Instruments\10.1\config\. The AppData folder is a system folder and thus may be hidden. Complete the following steps to view this folder: 1. Open a standard Windows explorer window. 2. Select Organize»Folder & Search Options. 3. Select the View tab, Show hidden files and folders, OK.
Technical Support and Professional Services C Visit the following sections of the award-winning National Instruments Web site at ni.com for technical support and professional services: • Support—Technical support resources at ni.com/support include the following: – Self-Help Technical Resources—For answers and solutions, visit ni.
Appendix C Technical Support and Professional Services If you searched ni.com and could not find the answers you need, contact your local office or NI corporate headquarters. Phone numbers for our worldwide offices are listed at the front of this manual. You also can visit the Worldwide Offices section of ni.com/niglobal to access the branch office Web sites, which provide up-to-date contact information, support phone numbers, email addresses, and current events. NI Ultiboard User Manual C-2 ni.
Glossary Symbol Prefix Value p pico 10 –12 n nano 10 –9 μ micro 10 – 6 m milli 10 –3 k kilo 10 3 M mega 10 6 G giga 10 9 T tera 10 12 A Active Layer The layer on which any actions you choose will be performed. All Angle Routing Routing that allows both 90° and 45° angles. Aperture Code Identifies the type of aperture to be used by the Gerber output. B Birds Eye View The small window that appears, by default, at the top left of the screen.
Glossary C Chamfer Corners Corners at an increment of 45º on the trace routes. Copper Area A copper polygon. Copper Island A copper area that is not connected to any other copper. D Design Toolbox By default, appears on left side of screen. Consists of multiple tabs used to manage a design. DRC Design Rule Check. F Feedthrough Via A normal via that connects all layers, top, bottom and inner.
Glossary O Output Window Gives you useful information on the status of your design. By default, is turned off. P Pad Stack The connections between layers of the board. Part Grid Determines the increments by which elements (parts and shapes) can be placed on the board. Prepreg Prepreg is fiber glass that is pre-impregnated with resin to make it semi-rigid. Prepreg sheets can then be placed between the copper foil and heated under pressure to activate and set the resin.
Glossary T Thermal Relief Area around a pin where no copper appears, but which is crossed by copper lines to make connections. A thermal relief is used to dissipate heat during the soldering process. Through-Hole Via Normal via. Trace Code The system provides 32 trace codes, each with a width and clearance. “Clearance” describes the space required between pads and pads, between traces and pads, and between traces and traces. This free space is continuously checked by the real-time design rule check.
Index Numerics B 3D view controlling elements in, 9-3 manipulating, 9-2 using, 9-1 Viewer options, 1-19 backannotation, 8-6 Bill of Materials exporting, 8-12 birds eye view, 1-28 block capacitor placement, 7-2 board adding layers, 1-24 cleaning up before manufacturing, 8-8 number of layers, 1-24 removing layers, 1-24 statistics export properties, 8-12 board outline creating, 3-5 drawing, 3-5 from database, 3-6 importing, 3-6 using wizard, 3-7 board properties about, 1-20 displaying, 1-20 grids and units,
Index adding parts to using Database Manager, 4-45 categories, about, 4-43 categories, copying, 4-43 categories, creating, 4-43 managing, 4-41 placing parts from, 4-27 sub-categories, deleting, 4-44 database categories about, 4-43 copying, 4-43 creating, 4-43 Database Manager about, 4-41 panels of, 4-41 using to create parts, 4-35 Database merge, 4-46 database sub-categories deleting, 4-44 Delete command, A-4 density bars, 5-6 design adding parts to database, 4-45 adding to project, 2-2 closing, 2-5 creati
Index settings, 8-9 Export command, A-2 dimensions default, 1-18 placing, 4-25 properties, 4-26 type, 4-25 documentation conventions used in the manual, vi NI resources, C-1 DRC running, A-14 DRC tab, 1-30 drivers (NI resources), C-1 Duplicate Component Name dialog, 4-46 DXF export properties, 8-11 importing, 3-6 importing into mechanical CAD design, 10-3 F Fanout Options dialog, 5-18 fiducial marks, 1-15 file export properties, 8-10 export settings, 8-9 exporting, 8-14 exporting - about, 8-8 locations,
Index multi--layered boards, 3-1 number on the board, 1-24 PCB layers, 3-3 removing from board, 1-24 swapping parts on, 4-11 tab, using, 3-3 Layers tab using, 3-3 leave drill holes open, 8-14 lines placing, 4-21 Lock command, A-5, A-23 guides moving, 4-10 placing, 4-10 removing, 4-10 using, 4-10 H help, technical support, C-1 highlighting in Multisim, 4-35 I initial routing, 7-7 in-place edit using, 4-29 In-Place Part Edit command, A-7 instrument drivers (NI resources), C-1 interface elements, 1-1 M ma
Index adding to database from design, 4-45 adding to database using command, 4-45 adding to database using Database Manager, 4-45 aligning, 1-8, 4-11 angle of, 4-11 centroids properties, 8-13 creating using Database Manager, 4-35 creating using the Part Wizard, 4-36 dragging, 4-7 editing (once placed), 4-29 finding, 4-4 flipping, 4-11 locating in open design, 4-34 locking, 4-4 orienting, 4-11 placing from the database, 4-27 placing multiple, 4-3 placing single, 4-3 placing using Design Toolbox, 4-2 positio
Index R PCB Differential Impedance Calculator, 6-7 PCB Properties Board Default tab, 1-25 PCB Transmission Line Calculator, 6-1 pin type test point, 4-25 Place toolbar, 1-9 placement strategies, 7-5 placing a comment, 8-3 placing powerplanes, 5-11 Placing SMD Fanouts, 5-18 placing traces, 5-1 placing vias, 5-15 polygon editing, 4-30 placing, 4-21 placing copper, 5-10 splitting, 5-11 position of parts, 4-17 powerplanes placing, 5-11 preferences Preferences dialog, 1-13 pre-placed traces, 7-8 pre-placing pa
Index trace ends, deleting open, 8-8 trace hugging, 7-7 trace spacing equi-space, 5-9 traces deleting, 5-9 training and certification (NI resources), C-1 troubleshooting (NI resources), C-1 Select toolbar, 1-5 Selection Filter command, A-6 selection filtering, 2-7 Setting database password, A-17 shape properties, 4-20 shapes placing, 4-21 shoving toggling on and off, 4-7 SMT pin properties, 4-33 software (NI resources), C-1 spacing of parts, 4-12 Spreadsheet View, 1-29 strategies for 100% part placement,
