Autodesk Inventor Fusion Technology Preview ® ® Autodesk Inventor Fusion: Getting Started
Contents Chapter 1 Autodesk Inventor Fusion TP2 . . . . . . . . . . . . . . . . . . . 1 What is new in TP2? . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Working with Inventor Fusion User Interface . . . . . . . . . . . . . . . 4 The Ribbon . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Display and Organize the Ribbon . . . . . . . . . . . . . . . 4 Customize the Ribbon . . . . . . . . . . . . . . . . . . . . . 5 Glyphs and Manipulators . . . . . . . . . . . . . . . . . . . . .
Create a Single Body . . . . . . . . . . . . . . . . . . . . . . . . 75 Create Multiple Bodies . . . . . . . . . . . . . . . . . . . . . . . 84 Modify a Body . . . . . . . . . . . . . . . . . . . . . . . . . . . . 93 Press/Pull Command . . . . . . . . . . . . . . . . . . . . . 94 Move Command . . . . . . . . . . . . . . . . . . . . . . . 105 Draft Command . . . . . . . . . . . . . . . . . . . . . . . 126 Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135 Starting a Sketch . . . . . . .
Slice Graphics . . . . . . . . . . . . . . . . . . Views of models . . . . . . . . . . . . . . . . . Orthographic views . . . . . . . . . . . . Perspective views . . . . . . . . . . . . . . Modeling Paradigms . . . . . . . . . . . . . . . . . . System Requirements . . . . . . . . . . . . . . . . . Operating System . . . . . . . . . . . . . . . . Hardware . . . . . . . . . . . . . . . . . . . . . Graphics Processing Unit (GPU) Requirements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
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Autodesk Inventor Fusion TP2 1 This is the Help for the second technology preview release of Autodesk Inventor Fusion released in October 2009. This content may not apply to prior or future releases.
Press/pull workflow improvements Improved look at behavior when working with sketches and sketch based features Improved sweep path behavior Sweep along spline Sketch: Polygon Ellipse Project existing sketch curves into new sketches Trim/extend spline and ellipse Copy and paste sketch geometry Assemblies: New assemble command Change constraints to move the first selection rather than treat it as grounded Add ground component to browser menu Constrain to work geometry Constraint folder in the browser Cycle c
Global dimension precision control User Interface: Minimize ribbon to panel buttons Simplified ribbon tabs Application menu file thumbnail support New effects and UI display options Option to turn off snap bar UI Improved background gradient Consistent visual style for in graphics UI Marking menu and command cleanup New context menus Selection glyph in canvas Shift middle-mouse-button for rotate Double-click dwg starts Fusion if file was last saved with Fusion User and System Tags: Add user tags Tag search
Support edges on or edges off visual style Working with Inventor Fusion User Interface This section presents general topics related to the Inventor Fusion User Interface. The Ribbon Display and Organize the Ribbon The ribbon is displayed automatically when you create or open a file, providing a compact palette of all commands necessary to create your model. The horizontal ribbon is displayed across the top of the application window. The ribbon minimize button minimizes the ribbon.
An arrow at the bottom of a panel title indicates that you can expand the panel to display additional commands. By default, an expanded panel closes automatically when you click another panel. To keep a panel expanded, click the push pin icon in the bottom-left corner of the expanded panel. Procedure To minimize the ribbon using the minimize button 1 Click the ribbon minimize button to the right of the ribbon tabs.
■ On each tab, you can change the order of ribbon panels. Click the panel to move, drag it to the appropriate position, and release. ■ You can hide panels. Right-click a tab and chose which panels to display. Glyphs and Manipulators As you use Inventor Fusion, you specify modes of operation, range limits, and other options.
Manipulators A Manipulator is a 3D command. It is usually an arrow, sphere, or ring that appears while a command is active. It sets the distance, angle, or direction of an operation, or for setting the location or size of a feature. Drag the manipulator to complete (or preview) the operation. The value that is set by dragging the manipulator can also be set in the ribbon or heads-up-display (HUD). When you release the manipulator, the corresponding value in the ribbon and HUD is updated.
Ring Used in the Hole command to set the hole diameter as well as counterbore and countersink diameters. Sphere Used in the Hole command to set the hole center location, in the Extrude command to set the taper angle, and in the Sweep command to sweep the selected profile along the path. When using manipulators, you do not need to keep your cursor exactly on the 3D arrow. You can drag anywhere over empty graphics space. Many manipulators can also snap to other geometry on your model.
Marking Menu with Context Menu The marking menu consists of eight wedges. Each wedge represents a command/operation. These commands are the seven frequently used commands and the eighth is a context menu which contains additional commands.
The default commands in the marking menu (context menu not shown) are: 1 Press Pull 2 Hole 3 Undo 4 Context Menu 5 Repeat Last Command 6 Delete 7 Select 8 Move You can invoke and hide the marking menu through the following steps, ■ To start the marking menu, right-click or right mouse down ■ To close the marking menu, use the escape key, release the right mouse button when no marking menu item is preselected, or click the left mouse button when no item is selected.
You can select an item from the marking menu through the following steps, 1 Invoke the marking menu (using either the right-click or holding the right mouse down). 2 Drag the cursor to the appropriate item. 3 Once the cursor is over the appropriate item, release the cursor and click the item. The marking menu item for Move is highlighted and the commandtip for the highlighted item is shown.
An alternative technique to execute a command in the marking menu involves gesture behavior. This is useful when you are well conversant with the marking menu layout and need a faster way to execute commands. Hence before using gesture behavior, a little practice with the marking menu to develop some muscle memory (familiarity) around the layout of the marking menu is helpful.
Marking menu wedge appears when cursor is released Context Menu The marking menu displays a context menu in its 4th wedge. After you invoke the marking menu, drag the cursor to the appropriate operation on the context menu. When you release the cursor, the operation is selected.
Context menu in modeling mode 14 | Chapter 1 Autodesk Inventor Fusion TP2
Context menu in sketching mode Context menu for Face selection Marking Menu | 15
Context menu for edge selection The context menu has a default menu item, which varies depending on the context and selection. The default menu item appears in bold text. When you select the 4th wedge of the marking menu in a gesture movement, the default context menu item is invoked. Primary Marking Menu Behavior when a Command is Active When a command is active, certain items in the marking menu display a different behavior depending on the context.
Item no. 3 represents 'Cancel' when in mid-command Item no 3. represents Undo outside a command When a command is executing and you select a different command, the current command is implicitly accepted if the input is valid. After this happens the new command is started. This technique can be utilized for quickly approving a command and ending it. The seventh wedge of the marking menu, which represents a Finish action when a command is active, is an easy way to do this.
Item no 7. represents 'Finish' which can be used to commit an active command Selection commands Mechanical designs often have many objects in the canvas which can make selecting the appropriate object difficult. The Select Other navigation commands in Inventor Fusion help you to select obscured or difficult-to-select geometry. The different options for the Select Other are accessible through a glyph which can be seen when you hover the cursor over a face/edge.
3 Feature 4 Parent Component The Parent Component option directly selects the component which is the parent for the face edge. When you select By Depth, Neighbor, or Feature, a selection strip is displayed. The strip contains several frames each representing a possible selection. When you hover over a frame in the selection strip, the corresponding element is highlighted in the model. When you click a frame in the selection strip, the corresponding element is selected.
In the following example, eligible faces with different depth order are listed in the selection strip. When you highlight the first frame in the Z Depth selection strip, the front most overlapping face element is also highlighted. The next frame selected in the strip causes an eligible element with a different Z Depth to be highlighted.
In the following example, the topological neighbors of a root face are listed in the selection strip. The last item in the strip represents all the edge loops connected with the root face. When you highlight a frame in the selection strip, the corresponding edge element is also highlighted. The last frame causes all edge loops to be highlighted.
In the following example, both the extrusion and the fillet are eligible features. The icons on the selection strip make it easy to identify the features by type. The icon in the selected frame in the selection strip identifies the extrude feature. The icon in the selected frame in the selection strip represents the fillet feature. Parent Component Selection When you choose the Parent Component Selection, the parent component for the root face/edge gets selected.
In the following example, the parent component of the root face gets selected. The parent component option from the fly-out was selected for the root face. Consequently the parent component of the root face is selected. Enhanced tooltip Many of the ribbon commands have enhanced (also referred to as progressive) tooltip which display information for interaction with commands. Initially, the name of the command and a short description of the command is displayed.
Browser and Copy/Paste In Inventor Fusion, the browser presents an organized view of the data in your design. Objects selected in the browser are selected in the graphics and vice-versa. You can create new component instances in the browser. Bodies can be dragged or copied and pasted from one component to another.
The blue node in the browser denotes the active component in your design. By double-clicking the component icon you can change the active component. This is important when creating new sketches, work features and features. All new objects that you create belong to the active component. Information Panel In Inventor Fusion, the model information is readily available. The browser includes an information panel for each node, which you can switch on or off.
right-click any component node and select New Component from the context menu to create a child component under the selected component. Additional Browser Functionality Select Isolate Component to hide all but the selected component (UnIsolate Component redisplays the hidden components). Use the Favorites folder to group frequently referenced components, bodies, features, and patterns. Cut/Copy and Paste bodies from one component to another, or across documents. Delete components, bodies, and features.
2 Marking Menu: right-click open space 3 Ribbon 4 Key strokes This functionality has also been mapped to the key sequences Ctrl+X and Ctrl+C. Note: If the user uses cut, the actual cut operation does not happen until the paste command is invoked. Every time a cut/copy command is used, the previously cut/copied objects are cleared from the clipboard.
The paste command pastes previously cut/copied objects from the clipboard. At the time of pasting a valid paste container is either deduced or needs to be specified. Rules are as follows: 1 Browser Node On a browser node that is a valid paste container. For example, a valid paste container for a set of sketch geometries is a sketch node in the browser.
3 Empty Space When the paste command is invoked in empty space, the active sketch or the active component is used as the paste container if that is valid.
4 Ribbon 5 Key Strokes This functionality has been mapped to the key sequence Ctrl+V. Note: Objects can be pasted in a different document from the one they were copied. Implicit Paste Using Browser Drag and Drop In addition, within a document, the user can drag and drop body objects and component objects. These drag-and drop operations result in an implicit cut and paste.
When a component instance is cut/copied, it can be pasted as a “shallow copy” or as a “deep copy”. In a shallow copy, a copy of the cut/copied component instance is added to the new owner as a new component instance; the structure under it is shared with other component instances. In a deep copy the entire subassembly under the component instance is copied. To distinguish between the two, a command called “Paste New” is available when the cut/copied object is a component.
Implicit Paste Behavior When paste is done implicitly, this is considered a restructure operation and the pasted object changes its place in the hierarchy. Its location and orientation in the world coordinate system remains unchanged. There is no user interaction needed after the drag-drop. Implicit paste clears the clipboard. Make Independent The “Make Independent” command operates on a component instance selection either in the browser or a graphical selection.
The following table contains all the reserved keyboard and mouse shortcuts in Inventor Fusion: Function Key Behavior F2 Pan F3 Zoom Shift+F3 Zoom window F4 Orbit F6 Zoom all F7 Slice graphics (see note) F10 Toggle shortcut keytips in Application menu and Quick Access commandbar Middle mouse button Pan Mouse wheel Zoom Shift+Middle Mouse button Orbit Note: Slice Graphics operation requires the selection of a cutting plane.
■ Red is the X axis ■ Green is the Y axis ■ Blue is the Z axis When you first activate the triad, its origin sphere is coincident with the geometry to transform. Click a triad section or drag to indicate the appropriate type of transform. As you select other parts of the triad, you can drag or enter precise coordinates corresponding to your selection. Triad Part Description Arrowheads Move the triad along the axis. Arcs Rotate the triad around the axis.
■ Populate input boxes with measurement. Access the measure command in the ribbon or in the fly out of any input box. Selection Support You can select objects in the browser or in the graphics window when using measure. You can also use filters to control which geometry types are eligible for selection.
The measure dialog box is displayed when the command is started and persists until the command is terminated. The dialog box displays geometry information dependent on the selected entities. click a row in the measure dialog box to copy that value to the clipboard. Use Ctrl + V to paste the value. Click and drag the dialog box to reposition it. Sample Workflow 1 Select a face to extrude. 2 Start the measure command from the value input fly out and select the objects to measure.
Most commands are available in both the ribbon and the context menu. A subset of frequently used commands appears in the marking menu. For more information see Marking Menu on page 8. Note: Right-click to display the marking menu and context menu. Other commands in the Application Window The application window displays commands such as the application button, the Quick Access commandbar, and the status bars.
Application Menu Click the application button to access commands to create, open, and export a file. Access Common commands Access common commands to start or export a file from the Application Menu. Click the application button to: ■ Create a file. ■ Open an existing file. ■ Save a file. ■ Save a file as another name. ■ Print a file. ■ Close the application.
Quick Reference This section contains descriptions of file access and print dialog boxes. File Open File Open Access: Opens when you perform operations requiring selection of a file. Look in Shows path of the active directory. File list The main window shows a list of the subfolders and files in the selected path. Double-click a subfolder to show the files it contains.
File name Specifies the file to open, enter a file name, or select a file from the listed files. Files of type Filters file list to include only files of a specific type. Click the arrow to show list, and then highlight to select a file type. Open Open the selected file. Cancel Cancels the file open operation and closes the dialog box. New File New File Creates a file. Print Print Prints or plots all or any portion of a model. Access: Click Print.
Number of Copies Sets the number of copies to print. Enter the number of copies, or use the up or down arrow to select the number of copies. You can print or plot all or any portion of a model. To print a model You can print or plot all or any portion of the active model. 1 Set up the view of the model. Only the portion of the model that is displayed in the graphics window prints. Print. 2 Click 3 In the Print dialog box, enter the number of copies.
The contents of the original file are unchanged. Save in Shows path of the active directory and specifies destination of the saved file. Locations File name Specifies the name of the file to save. If the file was saved, the file name is shown. File of type Filters file list to include only files of a specific type. Click the arrow to show list, and then highlight to select a file type. The extension is added to the file name.
Recent Documents View the most recently used files with the Recent Documents list. Files display in the Recent Documents list with the most recently used file at the top by default. Pinned Files You can keep a file listed, regardless of files that you save later, using the push pin button to the right. The file is displayed at the bottom of the list until you turn off the push pin button.
Click Recent Documents to view recent documents. Currently Open Documents View only files that are currently open with the Open Documents list. Files display in the Open Documents list with the most recently opened file at the top. To make a file current, click the file in the list. Procedure Click Open Documents to view open documents. Click Recent Documents to view recent documents. Preview Documents View file information in the Recent Documents and Open Documents lists.
When you pause the cursor over a file in either of the lists, the following information is displayed: ■ Path where the file is stored ■ Date the file was last modified ■ Version of the product used to create the file ■ Name of the person who last saved the file ■ Name of the person who is currently editing the file Quick Access commandbar Display frequently used commands with the Quick Access commandbar.
2 On the Customize menu, click the command name to display on the Quick Access commandbar.A check mark next to a command name indicates it is displayed on the Quick Access commandbar. To add commands to the Customize Quick Access commandbar menu ➤ On the ribbon, right-click the command add, and select Add to the Quick Access commandbar. To move the Quick Access commandbar menu above or below the ribbon 1 On Quick Access commandbar, click the drop-down arrow.
Use keytips to navigate in the Application Menu and in the ribbon using only the keyboard. Use the keyboard arrows to navigate to commands on the ribbon and Application Menu Navigation commands Navigation commands change the orientation and view of your model. The display of a model can be adjusted by increasing or decreasing the magnification at which objects are displayed or rotating the view of the model.
opaque and may obscure the view of the objects in the current view of the model. In addition to controlling the inactive opacity level of the ViewCube command, you can also control the following properties for the ViewCube command: ■ Size ■ Position ■ Default orientation ■ Compass display Using the Compass The compass is displayed below the ViewCube command and indicates which direction North is defined for the model.
ViewCube Menu Use the ViewCube menu to restore and define the Home view of a model, switch between view projection modes, and change the interactive behavior and appearance of the ViewCube. The ViewCube menu has the following options: ■ Go Home restores the Home view saved with the model. ■ Orthographic switches the current view to orthographic projection. ■ Perspective switches the current view to perspective projection.
Procedure To display the ViewCube menu, do the following: ■ Right-click the compass, Home icon, or the main area of the ViewCube. ■ Click the context menu button located near the ViewCube. SteeringWheels SteeringWheels are tracking menus (that follow your cursor) from which you can access different 2D and 3D navigation commands from a single command. Navigation commands Each wheel is divided into different wedges.
The point defined by the Center command provides a focal point for the Zoom command and a pivot point for the Orbit command. Note: To zoom from the Full Navigation wheels from your defined center point, hold down the Ctrl key before zooming. Up/Down command Unlike the Pan command, you use the UP/Down command to adjust the height of the current viewpoint along the Z axis of the model. To adjust the vertical elevation of the current view, you drag up or down.
Procedure 1 Display one of the Full Navigation wheels or the Tour Building wheels. 2 Click and hold down the Up/Down wedge.The Vertical Distance indicator is displayed. 3 Drag up or down to change the elevation of the view. 4 Release the button on your pointing device to return to the wheel. Forward command Use the Forward command to change the magnification of the model by increasing or decreasing the distance between the current point of view and the pivot point.
To adjust the distance between the current point of view and the pivot point you use the Drag Distance indicator. The Drag Distance indicator has two marks on it that show the start and destination distances from the current point of view. The current traveled distance is shown by the orange position indicator. Slide the indicator forward or backwards to decrease or increase the distance towards the pivot point. Procedure 1 Display the big Tour Building wheel.
When using the Look command, adjust the view of the model by dragging the cursor. As you drag, the cursor changes to the Look cursor and the model rotates around the location of the current view. Walking through a Model When using the Look command from the big Full Navigation wheel, you can walk through a model by using the arrow keys on the keyboard. Use the Properties dialog box for the SteeringWheels to adjust the walk command.
Specify the Pivot Point The pivot point is the base point used when rotating the model with the Orbit command. You can specify the pivot point in the following ways: ■ Default pivot point . When you first open a model, the target point of the current view is used as the pivot point for orbiting the model. ■ Select objects . You can select objects before the Orbit command is used to calculate the pivot point. The pivot point is calculated based on the center of the extents of the selected objects.
horizontally, the camera moves parallel to the XY plane. If you drag vertically, the camera moves along the Z axis. If the up direction is not maintained, you can roll the model using the roll ring which is centered around the pivot point. Use the properties dialog box for the SteeringWheels to control whether the up direction is maintained or not for the Orbit command. Pan command When the Pan command is active, the Pan cursor (a four-sided arrow) is displayed.
With the Rewind command, you can retrieve previous views from the navigation history. From the navigation history, you can restore a previous view or scroll through all the saved views. When you hold down the button on the pointing device over the Rewind command on the wheel, the Rewind History panel is displayed. You can scroll through the navigation history. To restore one of the previous views in the navigation history, drag the bracket to the left in the Rewind History panel.
When walking through a model, you can constrain the movement angle to the ground plane. If the Constrain Walk Angle to Ground Plane option is enabled, you can freely walk around while maintaining a constant camera viewpoint elevation. If the walk angle is not constrained, you will fly in the direction you are looking. Use the Properties dialog box for the SteeringWheels to constrain the movement angle to the ground plane for the Walk command.
you start the Zoom command from the Full Navigation wheel, incremental zooming must be enabled in the Properties dialog box for the SteeringWheels to use CTRL+click and SHIFT+click. ■ CTRL+click. If you hold down the CTRL key before you click the Zoom command on a wheel, the current view is zoomed in by a factor of 25 percent. Zooming is performed from the current pivot point, and not the location of the cursor. ■ Click and drag.
Zoom Constraints When changing the magnification of a model with the Zoom command, you cannot zoom in any closer than the focus point, or out any further past the extents of the model. The direction you can zoom in and out is controlled by the center point set by the Center command. Note: Unlike the Zoom command on the big View Object wheel, the Zoom command on the mini View Object wheel and the Full Navigation wheels are not constrained. Navigation Wheels Wheels are available in two sizes: big and mini.
The 2D Navigation wheel wedges have the following options: ■ Pan: Repositions the current view by panning. ■ Zoom: Adjusts the magnification of the current view. Note: Pan and Zoom in a 2D SteeringWheel are used to pan or zoom the page space. In all other wheels, Pan and Zoom moves the camera. ■ Rewind: Restores the most recent view orientation. You can move backward or forward by clicking and dragging left or right.
and out, and hold the SHIFT key while pressing and holding the middle mouse button to orbit the model. Big Full Navigation Wheel The big Full Navigation wheel wedges include the following options: ■ Zoom: Adjusts the magnification of the current view. ■ Rewind: Restores the most recent view. Move backward or forward by clicking and dragging left or right. ■ Pan: Repositions the current view by panning. ■ Orbit: Rotates the current view around a fixed pivot point.
■ Up/Down (Lower right wedge): Slides the current view of a model along the Z axis of the model. ■ Pan (Bottom wedge): Repositions the current view by panning. ■ Look (Lower left wedge): Swivels the current view. ■ Orbit (Left wedge): Rotates the current view around a fixed pivot point. ■ Center (Upper left wedge): Specifies a point on a model to adjust the center of the current view or change the target point used for some of the navigation commands.
Swivels the current view. ■ Rewind: Restores the most recent view. You can move backward or forward by clicking and dragging left or right. ■ Up/Downcommand: Slides the current view of a model along the Z axis of the model. Mini Tour Building Wheel The mini Tour Building wheel wedges have the following options: ■ Walk (Top wedge): Simulates walking through a model. ■ Rewind (Right wedge): Restores the most recent view. You can move backward or forward by clicking and dragging left or right.
Big View Object Wheel The big View Object wheel wedges have the following options: ■ Center: Specifies a point on a model to adjust the center of the current view or change the target point used for some of the navigation commands. ■ Zoom: Adjusts the magnification of the current view. ■ Rewind: Restores the most recent view orientation. You can move backward or forward by clicking and dragging left or right. ■ Orbit: Rotates the current view around a fixed pivot point.
Note: When the mini wheel is displayed, you can press and hold the middle mouse button to pan, scroll the wheel button to zoom in and out, and hold the Shift key while pressing and holding the middle mouse button to orbit the model. Overview of SteeringWheels SteeringWheels, also known as wheels, can save you time by combining many of the common navigation commands into a single interface. Wheels are specific to the context from which a model is being viewed.
Mini Wheels Mini Full Navigation Wheel Mini View Object Wheel Mini Tour Building Wheel Display and Use Wheels Pressing and dragging on a wedge of a wheel is the primary mode of interaction. After a wheel is displayed, click one of the wedges and hold down the button on the pointing device to activate the navigation command. Drag to reorient the current view. Releasing the button returns you to the wheel.
name of the active navigation command near the cursor. Disabling command messages and cursor text only affects the messages that are displayed when using the mini wheels or the big Full Navigation wheel. Wheel Menu Use the Wheel menu to switch between the big and mini wheels that are available, go to the Home view, change the preferences of the current wheel, and control the behavior of the orbit, look, and walk 3D navigation commands.
Increases the walk speed used for the Walk command by two times. ■ Decrease Walk Speed. Decreases the walk speed used for the Walk command by one half. ■ Orient to View. Orients the camera to match the view angle of the selected view (a plan, elevation, section, or 3D view). ■ Orient to a Plane. Adapts the view according to a specific plane. ■ Save View. Saves the current view orientation with a unique name.
Procedure ■ Click the down arrow in the lower-right corner of the wheel or right-click the wheel. Navigation Bar The navigation bar is a user interface element from which you can access both unified and product-specific navigation commands. Unified navigation commands (such as Autodesk ViewCube and SteeringWheels) can be found across many Autodesk products. Product-specific navigation commands are unique to a product.
Collection of wheels that offer rapid switching between specialized navigation commands. The following product-specific navigation commands are available from the navigation bar: ■ Pan. Moves the view parallel to the screen. ■ Zoom commands. Set of navigation commands for increasing or decreasing the magnification of the current view of a model. ■ Orbit commands. Set of navigation commands for rotating the current view of a model. ■ Look At. Views faces of a model from a selected plane.
Customize menu, you click the navigation commands to display on the navigation bar. The position of the navigation commands on the navigation bar is predefined and cannot be changed. Create 3D Models This section describes some common techniques that are used in Inventor Fusion to create designs. It covers a wide range of modeling techniques that can be used to create and edit model geometry and components in an Inventor Fusion design. First, a few notes about the nature of an Inventor Fusion design.
This simple design has some elements that are worth pointing out: 1 The Bodies folder in the browser. This folder contains all of the bodies for a component. This example has a single body Body1. 2 The Body node in the browser. Each body owned by the component has an entry in the Bodies folder. 3 The Sketches folder in the browser. This folder contains all of the sketches for a component.
6 The component body. The graphics area shows the geometry of the component. Most operations are performed by the user on this representation of the component. An Inventor Fusion design may also contain: ■ Multiple bodies ■ Work geometry ■ Annotation planes and annotations ■ Named views ■ Child components An example of a more complex design is shown here: Points of interest: ■ The design contains a second body. ■ The design contains a work axis.
Create a Single Body These steps illustrate how to start with an empty Fusion document, and create a single body in a simple design. This example uses these Inventor Fusion capabilities: ■ Sketching: Sketch on page 135 ■ Feature creation: Features on page 177 Starting point: An empty design This example begins with an empty design. This is the state when Fusion is first invoked, or when the New icon is clicked.
Because no sketch is currently active, the first step is to create a new sketch. Select one of the origin work planes.
This creates and activates a new sketch, changes the view to look at the new sketch, and invokes the Rectangle command: Create a Single Body | 77
Click a first and second point to describe the rectangle: 78 | Chapter 1 Autodesk Inventor Fusion TP2
As soon as the rectangle is finished, Inventor Fusion recognizes the closed region, and shades it in a yellow color: Create a Single Body | 79
Step 2: Extrude the rectangle 80 | Chapter 1 Autodesk Inventor Fusion TP2
Invoke the Extrude command. There are several ways to invoke Extrude. For this simple example, choose the Extrude command in the ribbon: Because there is only a single closed region, Fusion automatically selects it. If more than one closed region were available, you would be required to explicitly select which region to use.
Note that these elements are also present in the ribbon, but are much more convenient to interact with in the graphics area Drag to change the depth of the extrusion. You may drag over empty space, or directly over the distance manipulator.
Finish the command. There are a couple of ways to complete the command - starting another command, or clicking OK in the ribbon. In this case, click OK in the ribbon.
Create Multiple Bodies The steps in this topic illustrate how to create a second body, starting with a Fusion document containing a single body, and create a second body.
To learn how to create a design similar to this see: Create a Single Body on page 75 Step 1: Create a sketch and a sketch circle click the Circle command in the Ribbon Because no sketch is currently active, the first step is to create a new sketch. Select a face of the existing body.
This creates and activates a new sketch, changes the view to look at the new sketch, and invokes the Circle command. Select a circle center and radius point, away from the existing body. Note that because we selected a face of the existing body, Fusion has generated sketch geometry that coincides with the edges of that face. This sketch geometry is fixed, and so can't be edited.
Step 2: Exit the sketch In this example we illustrate how to exit sketch edit mode. click the Stop Sketch icon in the lower left corner of the screen.
Note that Fusion recognizes the two closed regions, and shades them in a yellow color. Step 3: Create a second body using the Revolve feature Invoke the Revolve command. There are several ways to invoke Revolve. For this simple example, we use the context menu. Select the circular closed region, using the left mouse button. Click or hold down the right mouse button to bring up the marking menu and the context menu.
This brings up the Revolve command, with the circular region as the profile to Revolve. Revolve requires a second selection - an axis to revolve about.
This prompts you to select an axis. You can select sketch lines or linear edges. In this case we select a sketch line from the face we sketched on: Once the axis is selected, begin dragging. In this example, we will drag in an area that is away from the manipulator. Click and drag the left mouse button in an area of the screen that is not over any graphics.
the upper right area of the screen. Note that the drag for Revolve,when dragging in open space is a 2-dimensional drag in the plane of the screen. Next, change the Operation Type of the Revolve feature to create a new body. Click and hold down the left mouse button over the Operation Type glyph, and choose New Body.
Finally, click OK in the ribbon to create the Revolve and the new body.
Modify a Body This section discusses how to modify an already-existing geometric body in a Fusion design. This is one of the strengths of Inventor Fusion, and one of the main workflows for new users to understand to be productive when using Fusion.
Inventor Fusion provides a highly interactive environment for geometric editing. You can drag faces of the body into a variety of new positions using the commands described in the following section. Related Topics: ■ Dimensions and Body Constraints on page 184 Press/Pull Command The Press/Pull command is one way that a user can modify body geometry. In general, Press/Pull provides users with an Offset style of modification. That is, the modified geometry is replaced with an offset of itself.
Multiple Faces Press/Pull can be applied to multiple faces at once: Modify a Body | 95
Resulting in: 96 | Chapter 1 Autodesk Inventor Fusion TP2
Cylindrical Faces Press/Pull can be used to change the radius of cylindrical faces: Resulting in: Modify a Body | 97
Fillet Faces Press/Pull can be used to change the radius of Fillet geometry, even if that geometry was not created in Inventor Fusion, and without the user having to select all the faces involved: 98 | Chapter 1 Autodesk Inventor Fusion TP2
Resulting in: Modify a Body | 99
Complex Face Geometry Press/Pull can be used to modify complex geometry as well as simple geometry: 100 | Chapter 1 Autodesk Inventor Fusion TP2
Resulting in: Modify a Body | 101
Used with Split Faces Press/Pull can be used in conjunction with Split Faces to even add geometry to a design: 102 | Chapter 1 Autodesk Inventor Fusion TP2
Resulting in: Modify a Body | 103
Command Interaction Press/Pull is extremely simple to use. invoke the command (using the Ribbon, Marking Menu, or Context Menu), select one or more faces (on one or more bodies), and drag using the left mouse button (either over the arrow drag manipulator, or over an area of the design with no geometry). You can drag, then release the mouse button, drag further, and repeat. When finished, start a new command (using any method), or click OK in the ribbon.
Move Command The Move command can be used to move a variety of objects in Inventor Fusion. These include: ■ Component instances ■ Work Geometry ■ Model body faces Use Move to modify the geometry of the design's body by moving one or more faces. See Position and Constrain Components on page 200 for information on using Move with components. The Move command, when applied to model faces, is a very powerful editing command.
For instance, in this case, a single face is selected and moved along the yellow (yellow indicates selection) direction: 106 | Chapter 1 Autodesk Inventor Fusion TP2
Modify a Body | 107
Move can be applied to geometry of any kind.
Note: Some faces are limited in their ability to move, by the geometry of the model.
disabled: This planar face is not free to move in those directions. In some cases, the move command may not be able to detect these limitations, and manipulators are enabled, even though dragging in that direction does not result in a change to the model.
The planar manipulators in the Move triad can be used to translate the selected faces in two directions at once.
arrow at the same time. Using the origin manipulator in Move to translate faces/features/components The origin manipulator in the Move triad can be used to translate the selected faces/features/components in all three directions at once.
In this case, the highlighted origin manipulator can be used to move the selected component in all the three directions of the green arrow, red arrow and blue arrow at the same time: Modify a Body | 113
Using Move to translate multiple faces at the same time Move can be used to modify more than a single face at a time.
same operation: Modify a Body | 115
Using Move to rotate faces Besides translation the Move triad can be used to rotate faces as well. The rotate manipulators are the arcs on the triad.
manipulator is used to tilt a model face: Modify a Body | 117
Reorienting the triad When a face is selected in the move command, Inventor Fusion will place the Move triad at a default location and orientation. At times, this orientation and position does not match the appropriate transformation.
in this case, a cylindrical face is selected. However, the default orientation is not ideal for moving the face along the rectilinear face that the hole is on. So, to change the default orientation to more fit your intended design modification.
The Reorient glyph can be used to accomplish this: If you click this glyph, the move command enters reorient mode. In this mode, geometry selections are used to reorient the triad, by aligning the active triad manipulator with the selected geometry. If a translate manipulator is active, a linear edge can be selected, and the triad is moved so that the active translate manipulator is aligned with the edge.
highlighted edge is selected while in reorient mode: Modify a Body | 121
The triad is reoriented along the selected edge: Translate manipulators can be reoriented along linear edges, work axes, cylinders, and planar faces. The triad can be reoriented about an active rotate manipulator similarly. Reorienting about a rotate manipulator is identical to reorienting about the corresponding translate manipulator. For instance, the blue rotate manipulator corresponds to the blue translate manipulator.
on the opposite side of the design. Use the Move command to achieve this with its snap to geometry feature. When a face is selected, if an applicable face is clicked that can be snapped to, move transforms the active faces so that they are aligned. Inventor Fusion indicates that snapping is possible with the prompt Select to snap when the cursor is over an available snap face.
face is aligned with the indicated blue face. Move and body constraints The Move command obeys any body constraints or locked dimensions during a move operation. For instance, a dimension has been created and locked between model geometry. Note that as one face moves, the other follows along.
In this case, the user has created a dimension and locked its value: Modify a Body | 125
If the top face of the design is selected in the Move command, the dimension is honored, and so the bottom face moves along with the top face: See Dimensions and Body Constraints on page 184 for more details. Draft Command The Draft command in Inventor Fusion can be used to modify one or more component bodies by creating angled faces, with respect to a neutral plane.
part from the mold easier. In these cases, the draft is usually applied to a selection of several faces, most often all of the side faces of the design. However, this command can also be used as a general modeling command for creating individual angled faces. Using Draft to model a simple molded part In this example, draft can be used to add draft to a part so that it can be easily removed from a mold. The following image is the original part: Invoke the Draft command.
In this example, the user has selected all of the vertical faces as draft faces: Next, you would drag, or enter a precise value into the draft angle entry box. In the following image, the draft angle has been set to an unusually high value, to more clearly show the effect of the draft operation.
Finally, you OK the command to apply the draft to the model: Using Draft to model a part that is to be manufactured with a split mold Sometimes, mold designers use a two-piece mold, which splits in the middle, to remove the part after cooling.
This selection indicates that the mold will be split along this plane. The vertical planes are selected as faces to draft: Next, you specify that this is a symmetric draft. Use the Draft Type glyph to specify this type of draft: Drag or enter a draft angle.
faces: Using multiple draft angles Sometimes you may want to perform a draft operation similar to the previous topic, but apply a different angle to faces above the neutral plane than to those below. You would use the two-way draft type to achieve this. The following example is identical to the previous example.
This time, in the Draft Type glyph menu, select two way.
The final result shows two different angles applied to each set of faces: Using Draft as a general body modification command In addition to using Draft to add an angle to all vertical faces, for the purposes of easier mold extraction, Draft can be used as a general command to edit a design.
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Or, two different angles to the faces: Sketch Introduction If you are creating a new part in Inventor Fusion, the first operation you perform is Sketching. This section explains Sketch creation, Sketch editing and other Sketch features in detail to help you learn the Sketching environment.
Starting a Sketch To start a Sketch, you can pick any Sketch command.
Sketch commands are also available from the context menu if there is no command currently active: Sketch | 137
Once a Sketch command is selected, you are prompted to define a Sketch Plane on page 138. At this point, you can pick any work plane or planar face to sketch on. Once the Sketch Plane is defined, you see the Sketch Grid on page 138 by default. The Sketch Plane The Sketch Plane is a plane on which you can draw Sketch entities. A Sketch Plane is always created as a child of the currently active component.
The Sketch Grid has two icons associated with it. The first is a Look-At icon that you can use to change the camera to look at the Sketch Plane if you perform any camera operations that would change the planes orientation. The second icon is a Stop Sketch icon that deactivates the Sketch and returns you to the select mode. The Grid aids in creating accurate Sketches by precisely snapping to points defined by its spacing. A snap point is indicated by a red rectangle.
Snap points are available throughout the Sketch Plane – they are not restricted to the visible Grid. You can hide the Grid in two ways: 1 Click the Grid icon at the bottom right of your commandbar. 2 Go to the View Tab, and under the “User Interface” drop-down box, uncheck the Sketch grid check box. The Sketch Grids spacing is controlled by the snap bar which appears to the bottom-right of the canvas. If the snap bar is set to 0, the Grid assumes a default spacing value.
Line/Arc Segment Creation Click the Line/Arc command button on the ribbon to activate the Sketch Line/Arc command. If there is no Sketch Plane on page 138 currently active, you are prompted to select one. When you activate the Line/Arc command, you can define points by clicking the mouse, or by typing the values into the Heads-Up Display (HUD) text boxes. When relevant, you get HUD text boxes where you input line lengths and angles from the vertical/horizontal.
If there are existing sketch geometries on your Sketch Plane, you also receive feedback on points that lie on other sketch entities, midpoints, and Grid snap points. See Sketch Inferencing on page 162 to learn more. Although you cannot define explicit constraints while creating Sketch entities, some constrains are implicitly detected when creating/editing Sketch entities. See Sketch Constraints on page 169 to learn more.
perpendicular from the start point to create a perpendicular line. See the Sketch Inferencing on page 162 page to learn more.
Line drawn tangent to a circle When one line segment is created, the creation of the second segment begins where the first ended, in effect producing a polyline. To end the creation of a line or set of lines, double-click the last point you want. Then you can start creating a new line independently of any previously created lines. To exit the Line command, press the Esc key or pick any other command. Any line segment that is currently in a preview state will be discarded.
When you activate the Spline command, you can define fit points by clicking the mouse, or by typing the values into the Heads-Up Display (HUD) text boxes. This helps you to create more precise geometry. You can press the Tab key to navigate from one HUD text box to another. If there are existing sketch geometries on your Sketch Plane, you also receive feedback on points that lie on other sketch entities, midpoints, and Grid snap points. See Sketch Inferencing on page 162 to learn more.
You can create a spline that is tangent to another line or spline by clicking the start or endpoint of the line or spline and dragging away from it. You see a tangent line indicator when the constraint is inferred. You can create open splines as well as closed splines. You can complete the creation of an open Spline entity by double-clicking at the last point. To create a closed Spline, click the start point of the current spline entity – it also is defined at the endpoint.
Note: It is possible to create self-intersecting splines (like a figure-8) using the spline command, but such non-manifold entities are not supported by the Sketch Profile on page 171 recognition system, and may cause undesirable results. To exit the Spline command, press the Esc key or pick any other command. Any Spline that is currently in a preview state is discarded. Circle Creation Click the Circle command button on the ribbon to activate the Circle command in the Center-Radius mode.
■ 3-Tangent Circle: Define a circle by picking three tangent lines. You can also switch between the different Circle creation options from the drop-down menu that is available when you are not in the middle of a creation operation. Press the down arrow key to get this option. If there are existing sketch geometries on your Sketch Plane, you receive feedback on points that lie on other sketch entities, midpoints, and Grid snap points. See Sketch Inferencing on page 162 to learn more.
To exit the Circle command, press the Esc key or pick any other command. Any Circle that is currently in a preview state is discarded. Circular Arc Creation Click the Circular Arc command button on the ribbon to activate the Circular Arc command in the 3-Point Arc mode. If there is no Sketch Plane on page 138 currently active, you are prompted to select one. You can also define a Circular Arc in the Center Point Arc mode by picking the drop-down option on the command button.
■ 3 Point Arc: Define a Circular Arc by picking the start point, endpoint and a third point on the Arc which is not collinear with the other two points. ■ Center Point Arc: Define a Circular Arc by picking the center point, start point and endpoint of the Arc. You can also switch between the two Arc creation options from the drop-down menu that is available when you are not in the middle of a creation operation. Press the down arrow key to get this option.
You can create an arc such that it is tangent to an existing Line or Circle/Circular Arc. To exit the Circle command, press the Esc key or pick any other command. Any Circle that is currently in a preview state is discarded. Rectangle Creation Click the Rectangle command button on the ribbon to activate the Rectangle command in the 2-Point mode. If there is no Sketch Plane on page 138 currently active, you are prompted to select one.
If there are existing sketch geometries on your Sketch Plane, you receive feedback on points that lie on other sketch entities, midpoints, and Grid snap points. See Sketch Inferencing on page 162 to learn more. Although you cannot define explicit constraints while creating Sketch entities, some constrains are implicitly detected when creating/editing Sketch entities. See Sketch Constraints on page 169 to learn more. To exit the Rectangle command, press the Esc key or pick any other command.
If there are existing sketch geometries on your Sketch Plane, you receive feedback on points that lie on other sketch entities, midpoints, and Grid snap points. See Sketch Inferencing on page 162 to learn more. Although you cannot define explicit constraints while creating Sketch entities, some constrains are implicitly detected when creating/editing Sketch entities. See Sketch Constraints on page 169 to learn more. To exit the Ellipse command, press the Esc key or pick any other command.
■ Circumscribed Polygon: Define the center and radius of the Polygons Inscribed circle. Define the number of sides by typing a value into the HUD text box. You see a preview of the inscribed circle in blue.
■ Edge Polygon: Define a Polygon edge, and then place the polygon by clicking on either side of the edge. Define the number of sides by typing a value into the HUD text box. You see a Polygon preview as you move your cursor from one side of the edge to another.
You can also switch between the different Polygon creation options from the drop-down menu that is available when you are not in the middle of a creation operation. Press the down arrow key to get this option. If there are existing sketch geometries on your Sketch Plane, you receive feedback on points that lie on other sketch entities, midpoints, and Grid snap points. See Sketch Inferencing on page 162 to learn more.
To exit the Polygon command, press the Esc key or pick any other command. Any Polygon that is currently in a preview state are discarded. Once a Polygon is created, editing one edge length does not cause all edges to update to that length. The edges and vertices are independent of each other apart from the inferred Constraints. Project Geometry Click the Project Geometry command button on the ribbon to activate the Project Geometry command.
With this command, you can trim Sketch entities against other entities on the Sketch plane, or extend them to other entities. The command is in the Trim mode by default. You can switch to the Extend mode by using the drop-down menu (press the down arrow key). Invoking the drop-down menu again switches back to the Trim option. Trim When you are in the Trim mode, you can hover over any sketch entity.
Extend When you are in the Extend mode, you can hover over any sketch entity. If it is possible to extend that entity against another entity, you see the section to be extended highlighted in dark green. If the entity can be extended at two ends (for example, an arc), the end that extends is the one closest to your mouse position. If an entity cannot be extended against another entity, you do not see a preview and clicking it has no effect.
To exit the Trim/Extend command, press the ESC key or pick any other command. Sketch Fillet Click the Sketch Fillet command button on the ribbon to activate the Sketch Fillet command. If there is no Sketch Plane currently active, you are prompted to select one. With this command, you can create fillets between two intersecting lines, two parallel lines, a line and a circular arc that intersect, and two circular arcs that intersect. Fillets cant be applied to circles, ellipses, elliptical arcs and splines.
Highlighting another valid entity removes the existing preview and show you a new preview. If two entities can be filleted in more than one way (e.g. two lines intersecting to form an X have four possible fillet options) then the selection pick points determines which solution is created. See FilletPreview.avi on page 160 for a demonstration. Once you have selected two valid entities, you see a fillet preview and an updated Context Ribbon.
You can click and drag on the yellow arrow to define the fillet radius. You can also type into the Radius edit box to change the fillet radius. A zero radius is not valid. If you drag the arrow such that the radius is zero, or you type in 0.0 in the box, you see an error message. Change the value to something valid Click OK to commit the preview and exit the command. The Sketch Fillet differs from other Sketch commands in that invoking another command also commits the preview and exit the command.
Note: Some inferences produce temporary constraints that are only available when creating a particular entity. They are not persisted and cannot be added, removed or changed. See Sketch Constraints on page 169 for more information. Some types of inferences are dependent on “touching” other Sketch entities with your mouse when in the middle of creating a new Sketch entity.
The red X symbol on any curve indicates that your cursor is touching a curve. If you click your mouse when you see this inference, then your new point is guaranteed to lie on the curve. ■ Midpoint Inference (5): If your cursor touches the midpoint of a straight line, you see a red triangle symbol indicating the midpoint. If the line has multiple segments, as in the following image, you do not see this inference.
If your cursor touches Sketch Grid snap point (on the visible Grid or the infinite Grid) you see a red square symbol. To learn more about Grid snapping, see the Sketch Grid on page 138 page. Constraint Inferences Constraint inferences are displayed based on your creation action. These inferences produce temporary constraints that affect how your entity is created. Some of these constraints is also inferred when you are editing a Sketch entity.
circle, a Tangent constraint is inferred. You see a red circle symbol with a red line drawn tangent to it. If you actually clicked the point on the circle before moving your mouse, your first point is fixed and you only infer this constraint when you move your mouse in a direction roughly tangential to the circle at your picked point.
A horizontal constraint is inferred if you are drawing a line and drag your mouse such that the line is parallel to the X-axis of the Sketch Plane. It is indicated by a horizontal red line symbol. Another kind of horizontal constraint can be inferred by “touching” a point and moving the mouse in a horizontal direction. You will see a white line stretching from the “touched” (referenced) point to your current mouse position.
A vertical constraint is inferred if you are drawing a line and drag your mouse such that the line is parallel to the Y-axis of the Sketch Plane. It is indicated by a vertical red line symbol. Another kind of vertical constraint can be inferred by “touching” a point and moving the mouse in a vertical direction. You will see a white line stretching from the “touched” (referenced) point to your current mouse position.
A parallel constrained is inferred when you “touch” a line that does not share endpoints with the line you are currently trying to create, and then moving your mouse in a direction roughly parallel to that line. Your line will be adjusted to be parallel to the “touched” (referenced) line and you will see a red horizontal line symbol on both the line being created and the “touched” line.
This inference results in a temporary constraint at edit time. If two entities share a point and that point is moved, it will affect both entities. ■ Point-On-Curve Inference This inference results in a temporary constraint at edit time. If one entity has a point that lies on another entity, moving the second entity will affect the first entity.
An inferred Sketch constraint cannot be removed through any user action. The only way to remove it is to delete one or more of the Sketch entities that participate in the constraint. Stopping a Sketch To exit a sketch command, press the Esc key, or click the specific sketch command button on the ribbon. To exit the sketch environment do one of the following: ■ Click the Stop Sketch glyph in the sketch environment: ■ Select Stop Sketch from the context menu.
In the image above, the Sketch Profiles are shown in Yellow. The blue region shows a highlighted Profile. Editing a Sketch Entity After creating a Sketch entity, you may wish to reposition it or edit its dimensions, or delete it. Selecting a Sketch Entity click a Sketch entity to select it. When an entity is selected you will see its dimensions. Note that selecting one edge of a polygon does not select the entire polygon. It will only select the edge.
Note: When in sketch mode (for example, you have an active Sketch Plane), select area will only select Sketch curves. It will not select Sketch points or Sketch profiles on page 171. Outside of Sketch, select area will select normal topology, but will not select Sketch curves. It will select Sketch profiles. Repositioning a Sketch Entity You can click and drag a selected entity to a new position and release the cursor to “drop” it in its new location.
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Selecting multiple sketch entities will display additional dimensions. As you edit a dimension, other visible dimensions are locked to their current their value as the sketch changes. A red X appears on dimensions that are being edited. The X indicates which endpoint is fixed while the dimension is being edited. To lock or unlock a sketch entity, click the entity, then invoke the marking menu (RMB) and select Lock/Unlock Geometry from the context menu.
Locking Sketch Geometry A Sketch entity can be locked by selecting it, right-clicking and picking the Lock/Unlock Geometry Option. It can be unlocked by selecting the menu item again. When an entity is locked, it is drawn in dark green. User-created edges are unlocked by default. Projected Geometry on page 157 is locked by default. Locking a curve does not automatically lock its endpoints or vertices. When a curve is locked, it cannot be moved.
Locking geometry will not eliminate any inferred Sketch Constraints on page 169. You will not be able to edit entities in a way that would break those constraints. Features This page describes the concept of “Features” in Inventor Fusion. A Feature in Inventor Fusion is essentially a collection of faces that represents a shape corresponding to a mechanical feature. Inventor Fusion uses the Direct Modeling paradigm as opposed to the Parametric Modeling paradigm used by Inventor.
■ Rectangular Pattern ■ Circular Pattern ■ Mirror Of these, Extrusion, Revolution, Sweep and Loft are Sketched Features. They are created from one or more 2D sketches on page 135. Each Feature is created by a command that allows the user to provide the inputs necessary to create the Feature using the direct manipulation user interface. Features can also be created on an imported model by using the Find Features on page 181 command.
pattern on page 181. Each copy of the geometry is called an occurrence. Changes to any one occurrence will effect all other occurrences in the pattern, for example the modification done by operations such as move, fillet, push/pull and draft in one occurrence will be propagated to all occurrences. Inventor Fusion supports two types of patterns: rectangular and circular. Rectangular pattern positions occurrences in rows and columns. Circular pattern positions occurrences in an arc or circular pattern.
Adding a fillet to any occurrence affects all occurrences. Circular pattern Circular patterns allow you to select a center around which to pattern geometry. The center must be a circular face like a cylinder, cone, or torus.
Rectangular Pattern Rectangular patterns allow you to select a direction you can then drag the manipulators to define a pattern that follows the given direction. The direction selection must be an edge. You can also drag away from the direction, in a perpendicular manner to create a rectangular pattern in either direction from one simple selection. Find Features Find Features is also referred to as feature recognition. It is a process to extract design feature information from a solid model.
In the following image, Find Features adds an extrude (the rectangular body) and a counter bore hole (the cylindrical cut) to the browser. Once a feature has been found, it is managed the same as features created with traditional methods. Features can be edited, deleted or dissolved.
If a downstream operation modifies a feature face, the owning feature will be re-evaluated. If the face set does not satisfy the feature definition, the feature will be removed from the browser. In the previous counter bore hole example, if the user moves the highlighted face, the feature will not be a valid counter bore hole and is removed from the browser at the end of move operation.
If a find features recognizes a feature in a way that does not fit your intent you can change it. In the browser you can right-click and change the feature type. For example recognize a hole as a revolve. You can also dissolve the feature which removes the feature from the browser but leaves the geometry on the model.
Body constraints include the following types: ■ Coplanar: Two planar faces are made to lie in the same plane ■ Center: Two cylindrical faces are made to lie along the same axis ■ Parallel: Two planar faces are made to be parallel ■ Perpendicular: Two planar faces are made to be perpendicular All of these body constraint types are accessible from the Constrain command. Note: In addition to body constraints, the Constrain command offers the ability to create inter-component (assembly) constraints.
In addition to explicit body constraints, you can lock a dimension to force the model to maintain that dimension at the current value regardless of other changes. The following video shows the basic operation: Locked dimensions are shown in bold.
the original. It is not possible to predict or specify which edge/face will acquire the constraint. It is possible to create situations where a dimension becomes invalid. In this situation, the dimension changes color during the preview. If you finish the command with dimensions in this state (sick), then the sick dimensions are deleted. It is possible to create a set of constraints that cannot be solved. In such a case, the error glyph will appear.
If you hover over this glyph, a commandtip will be displayed which gives a brief description of the error: If you click the error glyph, more information on the error is given, in a dialog box: 188 | Chapter 1 Autodesk Inventor Fusion TP2
Use the upper-right x icon in this dialog to dismiss it. The error glyph will disappear when the condition that is causing it is removed. For instance, errors in Fillet are often caused when the fillet radius is too large. entering a smaller radius, or dragging the manipulator to a legal value will cause the error glyph to disappear. When the error glyph is displayed, any command in progress cannot be committed. So, the OK check mark will be disabled whenever the command is in an error state.
The three default work planes are the YZ, ZX, and XY planes. The three default work axes are the X, Y, and Z axes. The single default work point is the O point which represents the value 0, 0, 0 in the model. The default work planes and axes are based on the origin point. The following image shows the origin geometries in the graphics window. Note: The origin geometries are not visible by default. When a new sketch on page 135 is started, the geometries are displayed automatically.
Create Work Geometry Work geometry creation commands are grouped as work plane, work axis, and work point creation commands. Each group is arranged in a drop down. Access the different creation methods by clicking the drop down arrow. Create work geometry by selecting a work geometry command then selecting existing geometry. Except for Offset Work Plane and Angle Work Plane, no values are required to create work geometry. The geometry you select defines the position of the work geometry.
Components in Inventor Fusion are organized hierarchically. That is, each component can have zero or more child components, and those child components can have child components, and so on. Every Fusion design has a single root component.
geometry, and is called a component instance. Component instances are indicated by the instance number in the browser: All instances of the same component share the same geometry, so a change to one applies to all instances of that component.
For instance, choosing New Component while the root component (the document) is selected 194 | Chapter 1 Autodesk Inventor Fusion TP2
Will create a new component which is a child of the root component Working with Multiple Components | 195
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A child component of that component is created: Activating a component Inventor Fusion always has an active component. The active component is where newly-created objects go. This includes body geometry (for example, if new features are created), work geometry, and new sketches.
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There are two ways to activate a component: Double-click the component's browser node, and using the Activate Component command. Adding solid geometry to the active component There are two main ways to add geometry to the body of a component. The first is by creating new features, such as Extrude, Revolve, Loft, and so on. The second is by dragging or copy/pasting bodies from other components. The primary method to create geometry is using feature commands.
menu, then select the intended new parent component (which could be the root component), and choose Paste. The result is a new instance of the copied component, which is attached to the cursor, and can be dragged to a new position. A click of the left mouse button will place the new instance. Position and Constrain Components This topic covers how to position component instances in 3D, and how to optionally create constraints to keep instances precisely positioned relative to other geometry in your design.
Selecting a component using the status bar selection breadcrumbs: Working with Multiple Components | 201
Once the component is selected, use the Move command's manipulators to translate or rotate a component. Note that if other components have constraints to the component being moved, they will also move to satisfy the constraints. If you want to position a component relative to other components, you can use the Assemble command. The Assemble command can be used with or without constraints.
In some design workflows, it is desirable to create persistent relationships between components, to assure that components stay together when one is moved. For instance, if your design contains a bolt/nut/washer assembly, you might want to make sure that these individual components stay together. You can create constraints between geometries on components. A constraint is a relationship between geometry on two different component Some examples of constraints are: ■ Align: aligns the two geometries.
This command serves two purposes: ■ Creating constraints between components. This topic will discuss this usage of Constrain ■ Creating body constraints. A body constraint is similar to a component constraint, except that it is used, not to position components, but to change the geometry of a single body in a component.
The two usages of Constrain are controlled by the Type input on the ribbon dialog: In general, when creating component constraints, you select two geometries and specify the Constraint Type. The first geometry selected will be the component that will move as a result of the constraint, while the second will generally remain fixed. Some Constraint Types support the ability to flip the solution (for example, from Mate to Flush when creating an Align between planes).
dimension's value. For more information about driving dimensions, see Dimensions and Body Constraints on page 184.
Two linear edges, not parallel, but in the same plane or parallel planes Angular Use Tab key to swap to Length dimension when edges are on different faces One circular edge Radius or diameter Dimensions as Annotations | 207
Two circular edges, non-concentric Length between centers Two circular edges, concentric and not coplanar Length along axis of cylinder One linear edge and one circular edge Length from line to center of circle Other Details 208 | Chapter 1 Autodesk Inventor Fusion TP2
Dimension precision can be controlled from the context menu. All dimensions use the same precision. (Angular vs. length dimensions have independent precision.) Dimensions are always created on an annotation plane. ■ Annotation planes are created automatically as necessary. Existing annotation planes are shared/reused if possible. ■ When creating a dimension, you can use the Tab key to select the appropriate annotation plane from the available ones.
■ There are no formatting or style mechanisms, other than the precision. Note: The context menu always uses the active selection in preference to the merely highlighted. So if you have a dimension selected, and then hover over a different non-selected dimension, and click right, it will tell you the lock-status of the selected dimension, and not the dimension under the mouse. User Tags Tags can be added to any face or body. These tags can then be used for searching/locating particular entities.
■ Expand the dialog box, select the tag name in the drop-down menu, and enter the tag value in the field. To enter a new tag name, select New. to apply the tag. You can also click Cancel You must click OK terminate the command without applying the tag. to Search User Tags You can search user tags and predefined feature tags. Searches are created and accessed in the Favorites area of the browser. Create a search using the context menu on the My Favorites node in the browser.
■ You can enter any feature type to search for all faces of that feature type. Advanced Tag Search ■ Click the expand button to display advanced search options. ■ You can set search criteria by defining up to two conditions. ■ There is a logical operator ■ The tag name drop-down list contains recently used tag names and a predefined list of feature tags names (Fillet Rad, Hole Dia, Hole Type, Hole Depth, CB Dia, CB Depth, CS Dia, CS Angle, Extrude Dist).
Import Data Import Data Part and assembly files from other CAD systems can be imported for use in Autodesk Inventor Fusion. The import operation does not maintain associativity with the original file. As a result, changes to the original file after the import operation do not affect the imported part or assembly. Likewise, changes to the imported part or assembly do not affect the original file.
3 Browse to and select the file to import. 4 Click Open to import the file. Importing CATIA V5 files Open and change models created in CATIA V5 (versions R6 - R19). Autodesk Inventor Fusion translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor Fusion commands to adjust the base features and add new features to the feature tree.
If an imported STEP file contains one part, it produces an Autodesk Inventor Fusion file with a single body. If it contains an assembly, it produces an Autodesk Inventor Fusion file with multiple components. Importing SAT files You can import a SAT file (versions 4.0 - 7.0). The solid body is saved in an Autodesk Inventor Fusion file, and no links are maintained to the original file. If an imported SAT file contains a single body, it produces an Autodesk Inventor Fusion part file with a single body.
Export Data You can export Autodesk Inventor Fusion parts and assemblies to other CAD system formats. The export operation does not maintain associativity with the Autodesk Inventor Fusion file. As a result, changes to the Autodesk Inventor Fusion file after the export operation do not affect the exported part or assembly. Likewise, changes to the exported part or assembly do not affect the Autodesk Inventor Fusion file.
2 Click the arrow next to the Save as type box, and then select the appropriate file type from the list. 3 Enter the file name in the box. If you do not enter a file name extension, the file is saved with the extension shown for the selected file type. 4 Click Save to export the Autodesk Inventor Fusion data to the file. Materials and Model Appearance Physical Materials When a body or component is created in Inventor Fusion, it will be assigned a default Physical Material (henceforth called Material).
create a body or component that has no Material. For the same reason, any body or component imported into Fusion that does not have a material associated with it is assigned a default material. Faces and other entities like Workplanes, Sketch profiles and so on do not have Materials. Inventor Fusion supports all the same materials as Autodesk Inventor. The default Material in Fusion is “Alloy Steel”. Note: When importing a file from inventor, the part is assigned the Material present in its iProperties.
A body or component typically inherits the Material of its immediate parent. You can set the entire document to have a particular material, and any object created under it will have that Material. You can override the material of child objects by selecting them and using the drop-down menu available in the Quick Access commandbar.
This drop-down menu is only enabled if one of your selected items supports Materials. You can pick any item from the drop-down and it will be applied to all valid selections. Every Material has a default appearance associated with it. When a component or body gets assigned a Material, it also assumes the appearance of the Material.
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Copper You can change the appearance of a component, body or face using Appearance Overrides on page 222. See the Appearance page for more information. Appearance An object in Fusion gets a default appearance based on its Material. This appearance can be overridden at the component, body or face level. Changing the appearance of an object will not affect its physical properties like mass.
Clicking the menu item will open the Appearance Dialog. This is a modeless dialog that shows you all the appearances available in Fusion, categorized in groups. These are the same appearances that would be available to you in Autodesk Inventor.
Moving your mouse over any color square will apply an appearance preview on your selected objects. You can double-click any square or right-click and select the “Apply to Selection” option to apply the appearance to your selection.
To remove an appearance override, open the Appearance dialog box and click the As Material button at the approximate center and bottom of the dialog box. Setting the Material on a component or body will change the appearance of the object. Face appearance overrides are not presently removed when the Material of their parent body or component changes. You can use the “As Material” feature to restore the faces appearance to its parents appearance if you need to.
Appearance Override priorities Appearance overrides applied at a component level have the highest priority and effect the appearance of all their children. The second priority is given to Faces, and the last priority is given to bodies. Hence, if a face has an appearance override, changing the bodys appearance will not remove it, but changing the components appearance will remove it. Edge Visibility You can turn edges on or off in your model by using the drop-down menu in the view ribbon.
The Shaded With Edges option will draw both faces and edges. The Shaded option will only draw faces. Inventor Fusion does not support a Wireframe (Edges-only) style at present.
Shaded Effects Visual effects are available in the View tab of the Ribbon Control. All effects are turned off by default. You can turn any effect on or off by clicking the check box. Effect settings are application-specific and will be saved and restored the next time you start the application. Note that turning any of these visual effects on may slow down performance.
Ambient Occlusion Ambient occlusion is an effect that takes into account attenuation of light due to occlusion. In the simplest terms, any object area that is obscured by another object would receive less light and would appear darker. Note that this effect is computationally expensive and will result in noticeable performance degradation.
Ambient occlusion on Shadow This effect casts a shadow of the object on the ground assuming that a light is directly overhead. The ground is not fixed in world space. It does not rotate with the object. It is the floor plane in view space.
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Shadows on Silhouette This effect draws a silhouette (outline) on the objects in the scene. This effect is only applicable if your Edge Visibility on page 226 is “Shaded With Edges”. If your setting is “Shaded” and edges are not visible, this effect will do nothing. A sphere will also have a circular silhouette, although it has no edges.
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Silhouette on Slice Graphics Use Slice Graphics to cut away part of the scene to better see other objects in the scene. It can slice the scene along any planar surface (a planar face or workplane). Select the surface to slice along before activating this feature.
It can also be activated or deactivated by pressing the F7 function key. When Slice Graphics is active, it will cut any bodies that intersect the plane. It will also create temporary “caps” to close any holes created by the slicing action, as you can see in the following images.
After slicing along the workplane Views of models Orthographic views You can set the view to Orthographic using a drop-down list in the View Tabs Visual Styles panel: In Orthographic Camera mode, a model is displayed so all its points project along parallel lines to their positions on the screen.
closer to you than the other. In Orthographic Camera mode, a 3D model appears flat and unlike objects observed in the real world. Use Orthographic Camera mode to confirm visually or compare the relative dimensions of entities. Note: The term camera mode indicates only the particular view method used for models in the graphics window. It is not meant to indicate that you can record actions that take place in the graphics window by choosing either Orthographic Camera mode or Perspective Camera mode.
In perspective camera mode, the model is displayed as it would be seen with a human eye. Objects further away from the camera appear smaller than objects closer to the camera. Also, if two lines are parallel to each other and are along the line of sight, they will appear to converge as they move further away from the camera. Use Perspective Camera mode to do a realistic “walkthrough” of a scene. Note: The term camera mode indicates only the particular view method used for models in the graphics window.
record actions that take place in the graphics window by choosing either Orthographic Camera mode or Perspective Camera mode. Modeling Paradigms There are many different types of modeling commands. In mechanical design, the need for manufacturing precision has led most commands to use some for of sold or surface BREP (Boundary Representation) modeling technology.
As an example: One common mechanical feature is a hole. It is drilled. Different drills bits come in different standard sizes and with different point angles. Holes can be counter sunk, counter bored and tapped. Rather that make a design create a cylinder and a cone to represent a hole. A hole feature can group the geometry together present the user with the list of available types and sizes making the definition of the geometry fast and easy. Holes are often positioned in specific ways.
You can think of history like a recipe. You can replay a history of features and the same model will result every time. You can change dimensions in a feature and then replay the history to generate new geometry for a new model. As an example: we create a 500mm x 300mm x 100mm Extrusion to create a plate. Next we create a hole with diameter of 20mm and a depth of 80mm. The hole is located 25mm from a corner of the plate. If you change the size of the plate the hole updates.
System Requirements Operating System ■ Microsoft® Windows® Vista (32-bit or 64-bit), SP1 ■ Microsoft®Windows® XP (32-bit), SP2, SP3 ■ Microsoft®Windows® XP (64-bit), SP2 Hardware Minimum requirements: ■ Intel Pentium 4, AMD Athlon 64 or AMD Opteron or later with 2.0GHz or faster processor; or compatible ■ 1.0+ GB RAM ■ 2.
Recommended Specifications: ■ Direct 3D 9-Compatible Graphics Card with Pixel Shader 3.0 support or Direct 3D 10-Compatible graphics card. Supports all Inventor Fusion Effects, including Ambient Occlusion. ■ Technical note: Supports Autodesk Graphics Feature Level 3_0 Testing your Graphics Card Capabilities: In your Inventor Fusion Install directory (“C:\Program Files\Autodesk\ Inventor Fusion Technology Preview 2” or the equivalent on your computer) you will find a Graphics Capabilities Application “Ads
DAC Type: Integrated RAMDAC Graphics HW Memory: 256 MB Display Mode: 1920 x 1200 (32 bit) (60Hz) VendorID: 0x10DE DeviceID: 0x00CC SubSystemID: 0x019B1028 RevisionID: 0x00A2 Graphics driver file: nvd3dum.dll,nvapi.dll Driver file version: 7.15.10.
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