SolidCAM Simultaneous 5-axis Machining User’s Guide ©1995-2005 SolidCAM LTD. All Rights Reserved.
SolidCAM2005 Milling Manual 5-axis Machining Contents 1. Introduction ............................................................................................................................... 5 2. User Interface ........................................................................................................................... 6 2.1 Adding a 5-axis Operation....................................................................................................6 2.
5-axis Machining SolidCAM2005 Milling Manual 6.6 Direction for One Way machining ...................................................................................... 62 Exercise 16:.................................................................................................................. 64 6.7 Cutting Area ....................................................................................................................... 65 Exercise 17:.........................................................
SolidCAM2005 Milling Manual 5-axis Machining 9.3.4 Tool axis will be tilted with fixed angle to axis ............................................................ 114 9.3.5 Tool axis will tilted around axis ................................................................................... 115 9.3.6 Tool axis will be tilted through point ........................................................................... 116 9.3.7 Tool axis will be tilted through curve ..............................................
-axis Machining SolidCAM2005 Milling Manual 1. Introduction Simultaneous 5-Axis machining is becoming more and more popular due to the need for reduced machining time, better surface finish and improved life span of tools. SolidCAM utilizes all the advantages of Simultaneous 5-Axis machining and together with collision control and machine simulation, provides a solid base for your 5-Axis solution.
SolidCAM2005 Milling Manual 5-axis Machining 2. User Interface 2.1 Adding a 5-axis Operation 5-axis (3) This operation performs 3-axis operations using special tools such as Lollipop and T-cutter, mostly for undercut areas. It is also possible to use the standard tools in this operation in order to create a 3D finish tool path; in this case the operation generates 3 axis G-Code and it is not possible to tilt the tool. This operation is available for 3 axis, 4 axis and 5 axis CNC-machines.
5-axis Machining SolidCAM2005 Milling Manual 5-axis (4) This operation is used for 4-axis finish operations such as turbine blade profiles on the outside diameter and spiral parts. The tool will be normal to the center line but will not necessarily cross the center line. The only tilt strategies that are available are those that support this type of tilting (4-axis). This operation generates 4-axis G-code and is available for 4-axis and 5-axis CNC-machines.
SolidCAM2005 Milling Manual 5-axis Machining 2.2 5-axis Operation user interface The following 5-axis Operation dialog is displayed on the screen: The parameters of the 5-axis Milling Operation are divided into a number of sub-groups. The sub-groups are displayed in a tree format on the left side of the 5-axis Operation dialog box. When you click on an item in the tree, the parameters of the selected sub-group appear on the right side of the Operation dialog box.
5-axis Machining • SolidCAM2005 Milling Manual Finish Parameters This page enables you to define the machining parameters such as Cut tolerances, Stock to leave, Run tool etc. • Gaps Page Surfaces defining the work piece can have gaps and holes. In such cases you can choose between several options. For example you can choose to have small gaps ignored and milled without the tool retracting and big gaps detected with the tool retracting back to the rapid plane and skipping the gap.
SolidCAM2005 Milling Manual 5-axis Machining 2.3 Stages of the Simultaneous 5-axis Operations parameters definition The process of the Operation parameters definition for the tool path creation is divided into 3 stages: 1. Geometry, Finish Parameters and Gaps – the type of finish tool paths generated along the selected faces is defined. Tool tilting and gouging are not taken into account at this stage. 2.
5-axis Machining SolidCAM2005 Milling Manual 3. CoordSys Page Choose the appropriate CoordSys position for the operation. The CoordSys Position can be chosen either direcly on the model or from the list. After the CoordSys selection, the model will be rotated to the selected CoordSys orientation. The CoordSys selection operation must be the first step in the Operation definition process.
SolidCAM2005 Milling Manual 5-axis Machining 4. Tool Page The Data button enables you to choose a tool from the Part Tool Table.
5-axis Machining SolidCAM2005 Milling Manual Feed Finish This field gets the default from the Feed Finish parameter in the Tool Data dialog. If the user changes this value it will not change the related field in the Tool Data dialog. Feed Z The feed that SolidCAM will use to move from the safety position to the depth point. Retract Rate The feed that SolidCAM will use to move the tool from the material to the retract level. Spin Finish The spindle speed for the cutting operation.
SolidCAM2005 Milling Manual 5-axis Machining 5. Levels Page Clearance Plane The clearance plane is a Z coordinate value and presents an absolute plane at this height which is parallel to the XY plane. The tool moves from and to this clearance plane to make major repositionings. In some cases like turbine blade machining around the X axis, it might be better to have the clearance plane defined in the X axis.
5-axis Machining SolidCAM2005 Milling Manual Clearance plane Safety distance Retract distance Retract distance Retract Distance and Safety Distance The tool changes its orientation at the clearance plane (machine tables or spindles are turned) and then it moves down to the part to the retract distance. The tool then moves in a rapid motion with some orientation to the safety distance. The tool then approaches the surface with the cutting feed rate.
SolidCAM2005 Milling Manual 5-axis Machining When the Rapid Retract option is active, the retract movement will be performed with the Rapid Feed. Rapid feed Retract distance Safety distance Depth The Depth defines a further offset of the tool in the axial direction (especially for swarf operations). This command shifts each point of the tool path in the vector direction of the tool. The start position of the cutting will also be shifted.
5-axis Machining SolidCAM2005 Milling Manual 6. Geometry Page This page enables you to select the faces to be machined and the machining strategy. The different strategies available are: • Parallel cuts • Cut along curve • Morph between 2 curves • Parallel to curve • Project curve • Morph between 2 surfaces • Parallel to surface For all the above strategies, select the drive surface and the related geometries.
SolidCAM2005 Milling Manual 5-axis Machining 6.1 Drive surface selection Click on the Define button. The Choose faces dialog will be displayed. This dialog enables you to select one or several faces of the SolidWorks model. The selected Face tags will be displayed in the dialog. If you chose wrong entities, use the Unselect option to undo your selection. You can also right click on the entity name (the object will be highlighted) and choose the Unselect option from the menu.
5-axis Machining SolidCAM2005 Milling Manual SolidCAM enables you to machine surfaces from the positive direction of the surface normals. Sometimes surfaces are not oriented correctly and you have to reverse their normals. The Reverse/Reverse All command enables you to reverse the direction of the surface normals. SolidCAM does not enable you to see the surface direction. You have to select the faces for the 5 axis operation and calculate the operation.
SolidCAM2005 Milling Manual 5-axis Machining 6.2 Cut Controls: The Exercises of the Cut control option are located in the Exercises\Cut_Control folder. 6.2.1 Parallel cuts The Parallel cuts option will create tool paths that are parallel to each other. The direction of the cuts is defined by two angles. The angles in X, Y and Z determine the direction of the parallel cuts of the tool path.
5-axis Machining SolidCAM2005 Milling Manual With constant Y Y X Changing the Machining angle in Z and the Machining angle in X, Y to 90 degrees creates tool paths parallel to the X axis. The Y-distance is constant. With constant Z Z X Changing the Machining angle in Z and the Machining angle in X, Y to 0 degrees creates circular tool paths. The Z-distance is constant.
SolidCAM2005 Milling Manual 5-axis Machining Fast orientation buttons Th following buttons enable you to expedite the definition of the orientation of the parallel cuts. The Constant Z button. The Parallel button. In this setup you can enter any angle to get the required tool path.
5-axis Machining SolidCAM2005 Milling Manual Exercise 1: 1. Load the CAM-Part: Exercises\Cut_control\parallel_cuts.prt 2. Simulate the operations and check the parameters used to control the Machining angles for the Parallel Cuts strategy. 3. Add operations for the machining of other cylinders. Use the Parallel Cuts strategy and define the necessary parameters in order to cut the cylinder normal to the direction of the center line. 4.
SolidCAM2005 Milling Manual 5-axis Machining Change Parallel cuts to spiral This option enables you to substitute the parallel cuts with the spiral cuts with the pitch equal to the defined Step over.
5-axis Machining SolidCAM2005 Milling Manual Exercise 2: 1. Load the CAM-Part: Exercises\Cut_control\parallel_cuts.prt 2. Simulate the operations and check the parameters used to control the Machining angles for the Parallel Cuts strategy. 3. Edit the operation rotate around z 45 deg. 4. In the Geometry page, choose the Change parallel cuts to spiral option. 5. Calculate and simulate the operation. Note that the parallel cuts of the operation were changed to spiral movements.
SolidCAM2005 Milling Manual 5-axis Machining 6.2.2 Cuts along curve The Cuts along curve option enables the user to select a leading curve. The generated tool path is orthogonal to this leading curve, so the cuts do not have to be parallel to each other. If a wrong leading curve is selected, the cuts can cross over each other and the result will be unacceptable. The curve geometry does not have to be located on the surface or on the edges of the surface.
5-axis Machining SolidCAM2005 Milling Manual Exercise 3: 1. Load the SolidWorks document: Exercises\Cut_control\cone.sldprt 2. Define a new CAM-Part. Use the Fanuc_4x_x postprocessor. 3. Define the Machine CoordSys with the X-axis directed along the cone centerline and the Z-axis directed upwards. For the CoordSys definition, use the home_ definition sketch. 4. Start a new 5-axis Operation and choose the Cuts Along Curve strategy. 5. Define the conical face as the drive surface.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 4: 1. Load the SolidWorks document: Exercises\Cut_control\cone.sldprt 2. Create a new CAM-Part. Use the Fanuc_5x CNC controller. 3. Define the CoordSys on the top face of the model. 4. Start a new 5-axis Operation and choose the Cuts Along Curve strategy. 5. Define the internal face of the manifold as the Drive Surface and the sketch segment containd in the Center_line sketch as a Lead curve.
5-axis Machining SolidCAM2005 Milling Manual 6. Calculate and Simulate the Operation. The simulation can be performed using either 3D or HostCAD simulation modes.
SolidCAM2005 Milling Manual 5-axis Machining 6.2.3 Morph between two curves The Morph between two curves option will create swarf cuts morphing between two leading curves. This option is very suitable for machining steep areas for mould making. The more accurate the guiding curves are to the real surface edges, the better this function works. To select the first (upper) and second (lower) curve, click on the Upper and Lower button.
5-axis Machining SolidCAM2005 Milling Manual It is very important to define the geometry for the Upper and Lower Edge curves correctly. SolidCAM generates the tool path from the Upper Edge curve till the Lower Edge curve. Upper Edge curve It is recommended to select the edges of the surface as the geometry of the Upper and Lower Edge curves. SolidCAM will check the distance from the curve to the surface and if Lower Edge curve the distance is bigger than 0.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 5: 1. Load the CAM-Part: Exercises\Cut_control\air_console.prt 2. Create a new 5-Axis Operation using the Morph between two curves strategy. 3. Define the Drive Surface as shown. 4. Select the model edge for the Upper Edge curve geometry as shown.
5-axis Machining SolidCAM2005 Milling Manual 5. Select the model edge for the Lower Edge curve geometry as shown. Make a note to select the short edge as shown. 6. Save, Calculate and Simulate the operation.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 6: 1. Load the CAM-Part: Exercises\Cut_control\impeller.prt 2. Create a new 5-Axis Operation using the Morph between two curves strategy. This option is used due to the inequality of the distance between the upper and lower curves of the blade. 3. Define the Drive Surface as shown. 4. Select the model edge for the Upper Edge curve geometry as shown. Make a note to select the geometry accurately without gaps.
5-axis Machining SolidCAM2005 Milling Manual 5. Select the model edge for the Lower Edge curve geometry as shown. Select the short edge as shown - the absence of this edge in the geometry causes an inaccurate tool path. 6. Save, Calculate and Simulate the operation.
SolidCAM2005 Milling Manual 5-axis Machining 6.2.4 Parallel to curve The Parallel to curve option will align the cut direction along a leading curve. Click Single Edge and select the curve.
5-axis Machining SolidCAM2005 Milling Manual Exercise 7: 1. Load the CAM-Part: Exercises\Cut_control\air_console.prt. 2. Create a new 5-Axis Operation using the Parallel to curve strategy. 3. Define the Drive Surface as shown. 4. Select the model edge as shown as the Curve geometry. 5. Save, calculate and simulate the operation.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 8: 1. Load the CAM-Part: Exercises\Cut_control\impeller.prt 2. Create a new 5-Axis Operation using the Parallel to curve strategy. 3. Define the Drive Surface as shown. 4. Select the model edge for the Lower Edge curve geometry as shown.
5-axis Machining SolidCAM2005 Milling Manual Select the short edge as shown - the absence of this edge in the geometry causes an inaccurate tool path. 5. Save, calculate and simulate the operation.
SolidCAM2005 Milling Manual 5-axis Machining 6.2.5 Project curves Project curves generates a single tool path along a curve. Click on the Projection curve button to define a curve. Curve & Tool path The projected curve is a result of the projection of the specified curve onto the selected surface. SolidCAM will not check the curve against the surface to check if it is a good curve.
5-axis Machining SolidCAM2005 Milling Manual Exercise 9: 1. Load the CAM-Part: Exercises\Cut_control\Solidcam.prt. 2. Create a new 5-Axis Operation using the Project curves strategy. 3. Define the Drive Surface as shown.
SolidCAM2005 Milling Manual 5-axis Machining 4. Select the model edges of the text for the Projection curves geometry as shown. 5. Save, calculate and simulate the operation.
5-axis Machining SolidCAM2005 Milling Manual Exercise 10: 1. Load the CAM-Part: Exercises\Cut_control\3D_engraving.prt. 2. Create a new 5-Axis Operation using the Project curves strategy. 3. Define the Drive Surface as shown.
SolidCAM2005 Milling Manual 5-axis Machining 4. Select the curve in the middle of the surface as the Projected curve geometry. This curve has to be created in the middle of the selected face and projected on the surface or created exactly on the surface. 5. Save, calculate and simulate the operation.
5-axis Machining SolidCAM2005 Milling Manual 6.2.6 Morph between two surfaces Upper edge surface Drive surface This option is similar to the Morph between two curves option. SolidCAM will create tool path morphing between two leading curves. In contrast to the Morph between two curves option where the leading curves are directly selected on the model, the Morph between two surface option enables you to choose two surfaces adjacent to the drive surface.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 11: 1. Load the CAM-Part: Exercises\Cut_control\insert.prt. 2. Create a new 5-Axis Operation using the Morph between two surfaces strategy. 3. Define the Drive Surface as shown.
5-axis Machining SolidCAM2005 Milling Manual 4. Select the upper fillet as shown to define the Upper Edge surface geometry. 5. Select the lower fillet as shown to define the Lower Edge surface geometry. 6. Save, calculate and simulate the operation.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 12: 1. Load the CAM-Part: Exercises\Cut_control\air_console.prt. 2. Create a new 5-Axis Operation using the Morph between two surfaces strategy. 3. Define the Drive Surface as shown. Select all the tangential side faces of the pocket. 4. Select all the adjacent top faces as shown to define the Upper Edge surface geometry.
5-axis Machining SolidCAM2005 Milling Manual 5. Select all the faces of the lower fillet as shown to define the Lower Edge surface geometry. 6. Save, calculate and simulate the operation.
SolidCAM2005 Milling Manual 5-axis Machining 6.2.7 Parallel to surface Drive surface Edge surface This option is similar to the Parallel to curve option. SolidCAM will align the cut direction along a leading curve. In contrast to the Parallel to curve option where the leading curve was directly selected on the model, the Parallel to surface option enables you to choose the surface adjacent to the drive surface. The common boundary of this surface and the drive surface will be used as the leading curve.
5-axis Machining SolidCAM2005 Milling Manual You can work with margins. The tool has to be a sphere mill and the Calc based on tool center option has to be activated in the Misc. Parameters page.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 13: 1. Load the CAM-Part: Exercises\Cut_control\insert.prt. 2. Create a new 5-Axis Operation using the Parallel to surface strategy. 3. Define the Drive Surface as shown.
5-axis Machining SolidCAM2005 Milling Manual 4. Select the lower fillet as shown to define the Single Edge surface geometry. 5. Switch to the Finish parameters page and set the Step Over to 5. 6. Save, calculate and simulate the operation. SolidCAM finds the common edges between the drive and edge surfaces and defines the leading curve for the tool path. The tool path is a result of the offset of the leading curve along the drive surface.
SolidCAM2005 Milling Manual 5-axis Machining 6.3 Flip Stepover changes the start cutting direction. This can change the machining direction from the outside to the inside or from the left to the right. Flip step over The machining begins at the top of the With the Flip Step over option the machining workpiece. begins at the edge.
5-axis Machining SolidCAM2005 Milling Manual Exercise 14: 1. Load the CAM-Part: Exercises\Cut_control\insert.prt prepared in Exercise 11. 2. In the Geometry page make sure that the Flip step over checkbox is not activated. 3. Simulate the Operation. During the simulation, note that the cutting is performed from the upper boundary of the drive surface downwards. 4. Activate the Flip step over checkbox. 5. Save, calculate and simulate the Operation.
SolidCAM2005 Milling Manual 5-axis Machining 6.4 Cutting Method SolidCAM enables you to choose the following Cutting methods: • One way • Zig Zag If you have a closed geometry and you select one way machining, the tool will always move around the part in the same direction.
5-axis Machining SolidCAM2005 Milling Manual If the geometry is not completely closed, then it is recommended to set the option Enforce closed contours.
SolidCAM2005 Milling Manual 5-axis Machining 6.5 Cut Order In the cut order menu you can choose between three options: • Standard - Sets a default cut order. • From Center Away - The machining begins in the center of the surface.
5-axis Machining SolidCAM2005 Milling Manual • From outside to center - The machining begins from outside the surface.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 15: 1. Use the CAM-Part prepared in Exercise 14. 2. Edit the 5-axis operation. 3. Make sure that the Flip step over checkbox is not active in the Geometry page. 4. Set the Cut order to the From center away option. 5. Calculate and simulate the operation. You will see that the tool path starts from the center and moves sequentially one step up and one step down.
5-axis Machining SolidCAM2005 Milling Manual 6. Set the Cut order to the From outside to center option. 7. Calculate and simulate the operation. As you can see the tool path starts from the top, moves to the bottom and then moves to the second top and so on. 8. Do not close the CAM-Part.
SolidCAM2005 Milling Manual 5-axis Machining 6.6 Direction for One Way machining This option is available only for the One way Cutting method. The Clockwise and Counter clockwise options are not for the spindle rotation. They are used to determine whether the tool should move around a closed surface model in clockwise or counter clockwise direction. • Ccwise This option enables you to perform the machining in counter clockwise direction.
5-axis Machining SolidCAM2005 Milling Manual • Cwise This option enables you to perform the machining in clockwise direction. • Climb The tool movement and the tool rotation have the same direction. Climb milling is preferred when milling heat treated alloys. Otherwise chipping can result when milling hot rolled materials due to the hardened layer on the surface. Tool rotation Tool movement direction • Conventional The tool movement is opposite to the tool rotation.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 16: 1. Use the CAM-Part prepared in Exercise 15. 2. Edit the 5-axis operation. 3. Switch to the Geometry page and choose the Cwise for the Direction for one way machining option. 4. Calculate and simulate the operation. As you can see the tool path works in the opposite direction. When the tool path is normal to the surface, it is not so clear what is the conventional or climb milling direction.
5-axis Machining SolidCAM2005 Milling Manual 6.7 Cutting Area SolidCAM enables you to choose the following options for the Cutting area: • Full, start and end at exact surface edge If this option is chosen, the tool path will be generated on the whole surface and exactly to the surface edge or to the nearest possible position. Edge Simulate the appropriate operation of Exercise18. The CAM-Part is located in the Exercises/Cutting_area folder.
SolidCAM2005 Milling Manual 5-axis Machining • Full, avoid cuts at exact edges Edge With this option the tool path will be generated on the whole surface but avoids the surface edges. Simulate the appropriate operation of Exercise18. The CAM-Part located in the Exercises/Cutting_ area folder. Edge • Limit cuts by one or two points This option enables you to limit the machining between one or two points. The Data button displays the Limit cuts between two points dialog.
5-axis Machining SolidCAM2005 Milling Manual Exercise 17: 1. Use the CAM-Part prepared in Exercise 16. 2. Edit the 5-axis operation. 3. Simulate the operation. Note that the tool path does not reach the edges of the drive surface because of the Cutting area option. This option is set to Full, avoid cuts at exact edges. 4. Switch to the Geometry page and set the Cutting area option to the Full, start and end at exact surface edges.
SolidCAM2005 Milling Manual 5-axis Machining 5. Calculate and simulate the operation. Note that the first and last cuts are performed exactly on the drive surface edges.
5-axis Machining SolidCAM2005 Milling Manual 6.8 Start Point Examples of the Start Point option are located in the Exercises\Start_Point folder. The Start point option enables you to choose a new start point where the machining begins. Depending on the geometry, 5axmsurf tries to find the nearest possible position next to your point. With the Rotate by option you can relocate the start position for the following cut. The coordinates will be calculated with the stepover and the angle you set.
SolidCAM2005 Milling Manual Original start point Default tool path start position 5-axis Machining New start point Tool path start position with new start point 20° 20° 20° Start points This is a tool path start position with a new start point and a 20 degrees rotation angle. Simlate operations of Exercise4 . The CAM-Part is located in the Exercises\Start_Point folder.
5-axis Machining 7.
SolidCAM2005 Milling Manual 5-axis Machining 7.1 Tool Contact point Examples of the Tool Contact point option are located in the Exercises\Tool_Contact_point folder. This parameter defines the contact point of the tool and drive surfaces. At a surface point with a given surface normal direction, the tool can always be placed tangentially. Move direction Radius Center Front You can see the touching points in the above picture. Center is exactly in the middle of the tool.
5-axis Machining SolidCAM2005 Milling Manual AT CENTER If this parameter is set to AT CENTER, then the tip of the tool touches the surface’s contact point. If the tool axis orientation is changed due to tilting options, then the tool will be tilted around this tip point. In such a case, the tool and surface are not tangential anymore and the tool will gouge the surface. This situation must be avoided by setting the first gouge check strategy to retract the tool from the drive surfaces.
SolidCAM2005 Milling Manual 5-axis Machining AT FRONT The option AT FRONT is similar to AT CENTER and forces the tool touching point to be always a fixed point on the tool. In this case, this fixed point is the beginning of the radius of a bull nose tool in the direction of the tool motion. All changes to the tool orientation are done around this pivot point which can cause gouging of the drive surfaces. Setting the gouge control is critical when working with this option.
5-axis Machining SolidCAM2005 Milling Manual Exercise 18: 1. Load the CAM-Part: Exercises\Tool_Contact_point\blade.prt. 2. Simulate the CAM-Part. This part is machined using the 4 axis CNC machine. The blade is twisted and if the tool is positioned tangentially to the surface, the tool path will not be parallel. It is possible to define a parallel tool path by using the Run tool option. 3. Edit the 5-axis operation and switch to the Finish parameters page. 4.
SolidCAM2005 Milling Manual 5-axis Machining 5. Calculate and simulate the operation. It is recommended to use 3D simulation mode to perform the simulation of the tool path with the tool displayed. The tool center is coincident to the drive surface along the whole length of the tool path. This causes gouges, so this option has to be used together with the gouge control options.
5-axis Machining SolidCAM2005 Milling Manual 6. If a flat tool is used for rough face milling, the At Front option enables you to mill the front part of the tool. Change the Tool Contact point option to At Front. 7. Calculate and simulate the operation. It is recommended to use the 3D simulation mode to perform the simulation of the tool path with the tool displayed. The front of the tool is placed on the point and the angle results from the vector of this point.
SolidCAM2005 Milling Manual 5-axis Machining 9. Set the Tool Contact point option to At radius. 10.Calculate and simulate the operation. It is recommended to use the 3D simulation mode to perform the simulation of the tool path with the tool displayed. Note that the tool corner radius is tangent to the drive surface along the whole length of the tool path. Make a note that the corner radius of the tool is tangent to the surface.
5-axis Machining SolidCAM2005 Milling Manual 7.2 Lead in / Lead out This switch turns on and off the tangential entry and exit moves. The Lead in / Lead out dialog enables you to define the parameters of Lead in / Lead out.
SolidCAM2005 Milling Manual 5-axis Machining Lead in/Lead out– These checkboxes enable you to define the lead in/out. The approach/retreat movements are performed by an arc with the following parameters: Arc sweep – The sweep angle of the lead in/out arc from the entry point on the tool path. Lead in point Tool path Arc sweep Lead in arc Arc diameter / Tool diameter % - This parameter specifies the ratio of the tool diameter.
5-axis Machining SolidCAM2005 Milling Manual When this option is not chosen, the approach arc plane will be normal to the previous plane.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 19: 1. Load the CAM-Part Exercises\Lead_in_Lead_out\insert.prt Now we will see how to use the entry and exit arc moves. 2. Set the following parameters in the Finish page. Choose the Morph between 2 surfaces option in the Cut Control field. Choose the Drive, Upper edge and Lower edge surface as shown.
5-axis Machining SolidCAM2005 Milling Manual Choose the Zigzag option in the Cutting method field. Choose the Standard option in the Cut Order field. 3. Switch to the Finish parameters page and set the following parameters: Set the Step Over value to 3. 4. Activate the Lead in/Lead out checkbox and click on the Lead in/Lead out button in order to define the Lead in/Lead out parameters.
SolidCAM2005 Milling Manual 5-axis Machining 5. In the Lead in/Lead out dialog activate both the Lead in and Lead out sections. Set the Arc Sweep to 90 and Arc diameter/Tool diameter to 200 in both sections. 6.
5-axis Machining SolidCAM2005 Milling Manual 7. Calculate and simulate the operation. As you can see, the entry and exit movements are performed by arcs. The arc size is double the tool radius. The arcs are parallel to the tool path direction in the entry point. 8. Display the Lead in/Lead out dialog and activate the Plunge with Z-Axis option. 9. Calculate and simulate the operation.
SolidCAM2005 Milling Manual 5-axis Machining Exercise 20: 1. Load the CAM-Part Exercises\Lead_in_Lead_out\Undercut.prt We will now see how the gouge checking affects the entry and exit arcs. 2. Start a new 5-axis Operation and choose Tool #1 from the Part Tool table. 3. Set the following parameters in the Geometry page: Choose the Parallel Cuts option for the Cut Control. Click on the Constant Z button to define the Machining Angle. Choose the One Way option in the Cutting Method field.
5-axis Machining SolidCAM2005 Milling Manual 4. Define the Drive surface as shown below. 5. Switch to the Finish parameters page and set the following parameters: Set Step Over to 6. Check the Lead in/Lead out checkbox.
SolidCAM2005 Milling Manual 5-axis Machining 6. Switch to the Gouge check page and define the following parameters: Activate the Enable/Disable checkbox. Inactivate the Check surfaces option. In the Strategy field, choose the Tilting tool away with max. angle option. The Gouge check options will be explained later. 7. Switch to the Gouge 2 page and define the following parameters: Activate the Enable/Disable checkbox. Inactivate the Drive surfaces option.
5-axis Machining SolidCAM2005 Milling Manual 8. Define the Check surfaces as shown below. Check surfaces The chosen strategy enables the user to avoid gouging by retracting the tool along the tool axis. 9. Switch to the Tool Axis Control page.
SolidCAM2005 Milling Manual 5-axis Machining 10. Set the following options: Choose the Tilted relative to cutting direction option in the Tool axis direction combo-box. Set the Tilt angle at side of cutting direction value to 90. Choose the Follow surface iso direction option in the Side tilt direction combobox. 11.Calculate and simulate the operation.
5-axis Machining SolidCAM2005 Milling Manual We can see arcs in every tool path depth in the right side approach and only one in the left side. This is because the gouge check sees that the tool will gouge to the left wall and moves the tool along the vector of the tool center till this gouge is finished. In this part all the paths move to a safe point (in the same point in this part) and then adds the exit arc. The gouge algorithm and the Entry/Exit algorithms protect the part from gouging. 12.
SolidCAM2005 Milling Manual 5-axis Machining 7.3 Round surface by tool radius This switch can be set to find small radius areas and inner sharp edges in the surface model. Such areas will be left out from the tool path generation. Inside corners can cause “fish tails” in tool paths. Such fish tails are removed by turning on this switch. This flag can also be considered as a fillet generator.
5-axis Machining The Round surface by tool radius option is active.
SolidCAM2005 Milling Manual 5-axis Machining 7.4 Stock to leave The Stock to leave parameter describes the stock to be left on the finishing surfaces. This parameter can also be negative, e.g. for cutting electrodes. Stock to leave For example, if this value is set to 0.2 units, then the tool will not come closer than 0.2 units to the surface. Therefore, after the machining, there will be remaining stock on the surface of about 0.2 units. Simulate the operations of Exercise14.
5-axis Machining SolidCAM2005 Milling Manual 7.5 Multi Passes This switch can be turned on to calculate multiple tool path passes on the same geometry. The Multi passes dialog enables you to define the following parameters: The Roughing passes section enables you to define a number of rough passes (specified by the Number parameter) with the specified spacing (the Spacing parameter) between them. The Finishing passes section enables you to define a number of finishing passes.
SolidCAM2005 Milling Manual Constant step over at each pass roughing and finish passes. pass 1 pass 2 pass 3 pass 4 5-axis Machining – this option enables you to define the order of execution of the pass 1 pass 2 pass 3 4 pass With Constant Stepover Without Constant Stepover When this option is turned off, all the rough and finish passes will be done at the current height level before moving to the next height level.
5-axis Machining SolidCAM2005 Milling Manual 7.6 Surface Quality 7.6.1 Chaining Tolerance The chaining tolerance is an internal value for the tool path generation and should be 1 to 10 times the cut tolerance. If you have untrimmed simple surfaces, then this value can be set to 100 times of the cut tolerance and will increase the calculation speed drastically. Using higher values in the chaining tolerance can cause inaccuracies. The tool path will not be as good, but the calculation time will be faster.
SolidCAM2005 Milling Manual 5-axis Machining 7.6.2 Cut tolerance The Cut tolerance is the tolerance for the accuracy of the tool path. A tight Cut tolerance gives you more tool path points on the drive surface. Therefore the generated tool path is more accurate. The result of the machining is a very good surface quality but the calculation time is increased. A loose Cut tolerance generates less points on the tool path. After the machining, the surface is rougher but the calculation time is much faster.
5-axis Machining SolidCAM2005 Milling Manual 7.6.3 Distance Whether you have more or less points depends on the Cut tolerance. You have more points on round surfaces because the tool path always changes direction. Use the Distance option to get more points on flat surfaces. Although the Cut tolerance is the same you get more points on straight or flat surfaces. Setting a small value gives more points whereas a high value gives fewer points.
SolidCAM2005 Milling Manual 5-axis Machining 7.6.4 Stepover The Stepover is the distance between two neighboring parallel cuts.
5-axis Machining SolidCAM2005 Milling Manual 8. Gaps Page The tangential entry and exit switch add 90° arc moves to the beginning and end of each tool path section. The diameter of this arc is determined in relation to the currently used tool diameter. The plane of the arc is automatically determined perpendicular to the surface. 8.
SolidCAM2005 Milling Manual 5-axis Machining 8.1.1 Gap Size as % of tool diameter The value in the field Gap Size as % of tool diameter sets the threshold for small and large gaps along a tool path segment. The value is defined as the percentage of the tool diameter. All gaps along the tool path segment, which are smaller than this threshold value, are considered as small gaps and the action defined for small gaps is executed.
5-axis Machining SolidCAM2005 Milling Manual Here you can see the Direct tool path between the two drive surfaces. Simulate the appropriate operation of in the Exercise19 The CAM-Part is located Exercises\Gap_Along_Cut folder. 8.1.3 Broken If you choose Broken and a gap is detected, the tool retracts a litt le bit. The retracting direction is the tool axis. With rapid speed, the tool leaves the drive surface and moves over to the next tool path point with machining speed.
SolidCAM2005 Milling Manual 5-axis Machining Here you can see the tool retracting to the rapid plane. It leaves and enters the drive surfaces along its axis. Simulate the appropriate Operation of Exercise19 The CAM-Part is located in the Exercises\Gap_Along_Cut folder. 8.1.5 Follow Surface SolidCAM performs the machining of the gap area tangentially to the surfaces close to the gap. Simulate the appropriate Operation of in the Exercise19 The CAM-Part is located Exercises\Gap_Along_Cut folder.
5-axis Machining SolidCAM2005 Milling Manual 8.2 Gaps between cut (Gap Size as % Of Stepover) If gaps between a tool path are detected, you can ignore the gap and move the tool connecting the two sides of the gap or retract the tool to the rapid plane, skip the gap and then come back from the rapid plane to the other side of the gap and pursue the machining. The limit for ignoring the gap can be entered as the gap size as a % of the maximum stepover. 8.2.
SolidCAM2005 Milling Manual 5-axis Machining 8.2.2 Direct If you choose Direct, the tool uses the shortest way to the other side of the gap without any retracting movements. The tool path in the gap is a straight line and the tool moves in machining speed. Here you can see the Direct toolpath between the two drive surfaces. 8.2.3 Broken If you choose Broken and a gap is detected, the tool retracts a little bit. The retracting direction is the tool axis.
5-axis Machining SolidCAM2005 Milling Manual 8.2.4 Retract With Retract the tool moves back to the rapid plane. The tool movement has rapid speed. Only the return to the drive surface has machining speed. Here you can see the tool retracting to the rapid plane. It leaves and enters the drive surfaces along its axis. 8.2.
SolidCAM2005 Milling Manual 5-axis Machining 9.
5-axis Machining SolidCAM2005 Milling Manual 9.1 Output format The output format can be set to 3, 4 or 5 axis. In case of 3 axis, the tool axis direction must be defined by the user, e.g. top view is 0,0,1. In case of 4 axis output, the rotary axis must be selected, e.g. around X, Y or Z. The output format is the property of this operation. As explained previously, SolidCAM has three types of 5-axis Operations: 3-axis, 4-axis and 5-axis.
SolidCAM2005 Milling Manual 5-axis Machining 9.2 Maximum angle change The maximum angle step is the maximum angle value between two tool path points on the surface. The number of points generated depends on the surface blending and the maximum angle step. Increasing the maximum angle step generates more points, decreasing the value generates less points.
5-axis Machining SolidCAM2005 Milling Manual 9.3 Tilting strategies (Tool axis direction) Exercises of the Tilting strategies are located in the Exercises\Tilting_strategies folder. 9.3.1 Tool axis is not tilted and stays normal to the surface Simulate the appropriate Operation of Exercise9 The CAM-Part is located in the Exercises\Tilting_ strategies folder.
SolidCAM2005 Milling Manual 5-axis Machining 9.3.2 Tool axis will be tilted relative to cutting direction This option enables you to change the lag angle of the cutting direction as well as the lag angle at the side of the cutting direction. Both are shown below. 45° Surface Normal Tool Axis tti Cu ng tion c e r di Simulate the appropriate Operation of Exercise9 The CAM-Part is located in the Exercises\Tilting_strategies folder.
5-axis Machining SolidCAM2005 Milling Manual Tool Axis Cutting direction 45° 45° Surface Normal Z-Axis 45° Tool Axis Simulate the appropriate Operation of Exercise9. The CAM-Part is located in the Exercises\Tilting_ strategies folder. The tool axis is tilted with a lag angle of 45° to the cutting direction and 45° at the side of the cutting direction.
SolidCAM2005 Milling Manual 5-axis Machining 9.3.3 Tool axis will be tilted with the angle Tool Axis Simulate the appropriate Operation of Exercise9. The CAM-Part is located in the Exercises\Tilting_ strategies folder. Tilt Axis 45° In the above case, the tool axis is tilted 45 degrees from the surface normal direction towards the Y axis. Surface Normal 9.3.4 Tool axis will be tilted with fixed angle to axis Simulate the appropriate Operation of Exercise9.
5-axis Machining SolidCAM2005 Milling Manual 9.3.5 Tool axis will be tilted around axis Simulate the appropriate Operation of Exercise9. The CAM-Part is located in the Exercises\Tilting_ strategies folder. The tool axis direction is the same like the surface normal but tilted with a 45 degrees angle around the main Z axis.
SolidCAM2005 Milling Manual 5-axis Machining 9.3.6 Tool axis will be tilted through point Simulate the appropriate Operation of Exercise9. The CAM-Part is located in the Exercises\Tilting_ strategies folder. Tool Axis direction Point The tool axis is always aligned to the point above the work piece.
5-axis Machining SolidCAM2005 Milling Manual 9.3.7 Tool axis will be tilted through curve Simulate the appropriate Operation of Exercise9. The CAM-Part is located in the Exercises\Tilting_ strategies folder. The tool axis is always aligned to the curve above the workpiece.
SolidCAM2005 Milling Manual 5-axis Machining Closest point The direction of your tool axis here is the same like the shortest distance between your present tool path point and the tilt curve. So the 3D-length is used. The following example shows a wavy surface with a tilt curve above. You can see that the tool axis has the same direction like the shortest 3D distance between the surface and the present tool path point.
5-axis Machining SolidCAM2005 Milling Manual Fixed tilt angle You can set an additive tilt angle to your present tool axis direction. The Positive angle lets the axis tilt against the main axis. With negative angles the tool axis tilts from the main axis. The main axis is usually the Z-axis. Maximum tilt is reached when the tool axis is parallel to the main axis.
SolidCAM2005 Milling Manual 5-axis Machining Angle from curve The direction of your tool axis here is the projected length between your present tool path point and the tilt curve. So the 2D distance is used. The following example shows a wavy surface with an tilt curve above. You can see that the tool axis has the same direction like the projected distance between the surface and present tool path point.
5-axis Machining SolidCAM2005 Milling Manual The view from the top shows the shortest 2D distance between the tilt curve and the tool path point. The tool axis always has the same direction.
SolidCAM2005 Milling Manual 5-axis Machining From Start to end This tilt type is used for generating tool paths for tube milling. The tube milling is usually machined in z-constant cuts and the result is cut slices. The amount of the z constant cuts depends on the maximum stepover. Now the tilt curve will be divided by the number of slices of the tool path. Every slice is now aligned to its point on the curve. Make sure that the beginning of the curve is on the right side.
5-axis Machining SolidCAM2005 Milling Manual 9.3.8 Tool axis will be tilted through lines Simulate the appropriate Operations of Exercise9 and Exercise8 The CAM-Part is located in the Exercises\Tilting_strategies folder. Line Tool Axis Tool Axis Line Line Tool Axis Line 9.3.9 Tilted from point away Simulate the appropriate Operation of Exercise9 The CAM-Part is located in the Exercises\Tilting_strategies folder. The tool axis is always aligned from the point.
SolidCAM2005 Milling Manual 5-axis Machining 9.4 Side tilt definition This parameter defines the side tilting direction when the tilt strategy is set to relative to cutting dir. Side tilting definition is an important setting to define a proper side milling with the tool. Side milling is aimed to get a line contact between the tool and the surface.
5-axis Machining SolidCAM2005 Milling Manual the surface normal rotated 90 degrees towards the spindle main direction. In practical terms, such a rotation can be handled by a machine tool without utilizing the C axis. The next option Use user defined dir is the same like the previously described spindle main direction option. The only difference is that the user can set any user defined direction instead of the spindle main dir.
SolidCAM2005 Milling Manual 5-axis Machining 9.5.1 XZ Limit This switch is set to true to limit the tool on the XY plane between angle b1 and b2. In this example you can see that the minimum tool limit angle b1 = 30 degrees and the maximum angle b2 = 120 degrees. Tool axis B2=120° B1=30° Z X 9.5.2 YZ Limit This switch is set to true to limit the tool on the YZ plane between angle a1 and a2.
5-axis Machining SolidCAM2005 Milling Manual 9.5.3 XY Limit: This switch is set to true to limit the tool on the XY plane between angle c1 and c2. In this example you can see that the minimum tool limit angle c1 is 40 degrees and the maximum angle c2 is 95 degrees. You can use any angle between 0 and 360 degrees. C1=40° C1=40° Y X 9.5.4 Conical angles from leading curve This switch is set to true to limit the tool between two angles which are orthogonal to the leading curve.
SolidCAM2005 Milling Manual 5-axis Machining 10. Gouge Check page The gouge checking option looks at the generated tool path and the end surfaces to decide whether the tool tip or shaft is gouging the surfaces. Further check surfaces can be selected to avoid gouges with surfaces that are not going to be machined. The gouge checking is supported for all tool types (flat, ball, conical and bull nose). The check is done at each calculated tool position.
5-axis Machining SolidCAM2005 Milling Manual 10.2 Check gouge between positions Exercises of Check gouge between positions option are located in the Exercises\Gouge_Check folder. This switch is set to true to activate the collision check between tool path positions. The 5 axis sweep moves from one position to the next position and is then used to check for collisions with drive and check surfaces.
SolidCAM2005 Milling Manual 5-axis Machining Position 2 Position 1 Position 1 Position 2 No gouge check between positions With gouge check between positions SolidCAM sets this field as the default to avoid problems of gouging check surfaces along movements. If the option is checked, the gouge check will be done in steps of the Cut tolerance defined in the Finish Parameters page. If the tolerance is 0.01, the check will be performed every 0.01 of mm (or inch) along the tool path.
5-axis Machining SolidCAM2005 Milling Manual 10.3 Gouge pages SolidCAM enables you to set a number of parameter sets for the gouge check. When the page is enabled, the collision checking will be performed with the defined parameters. 10.4 Tool Here you can activate the gouge check for the Tool Tip, Tool Shaft, Arbor and Holder. It is also possible to give a clearance to the arbor and the holder.
SolidCAM2005 Milling Manual 5-axis Machining 10.4.2 Check Arbor and Check Holder Both switches should be set to true if the collision checking is performed with the arbor and holder. Both switches are set to false to turn off collision checking with the arbor and holder. 10.5 Strategy Examples of the Check gouge between positions option are located in the Exercises\Gouge_Check folder. This function sets the collision elimination strategy for the first collision checking block.
5-axis Machining SolidCAM2005 Milling Manual 10.5.1 Retracting tool along tool axis If control by retracting tool along tool axis is selected, then the gouge is avoided by retracting the tool. The resulting tool path is then gouge free. The retract distance is shown to the user. Also a red line is drawn which shows the retraction move. Another line connects the calculated tool position before retraction and the surface point used for calculating the tool position.
SolidCAM2005 Milling Manual 5-axis Machining 10.5.2 Moving the tool away This option assigns the direction in which the tool has to move away. When retracting, the tool always uses the shortest distance to go around the check surface. From the point a gouge is detected, the tool moves away only in the selected retracting direction. New tool path points X-direction Check surface Old tool path points Drive surface Here a gouge is detected.
5-axis Machining SolidCAM2005 Milling Manual Retract tool in XY: Simulate the appropriate Operation of Exercise11 The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts in X or Y. Retract tool in XZ: Simulate the appropriate Operation of Exercise11 The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts in X or Z.
SolidCAM2005 Milling Manual 5-axis Machining Retract tool in YZ: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts in Y or Z. Retract tool in +Z: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts only in +Z.
5-axis Machining SolidCAM2005 Milling Manual Retract tool in –Z: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts only in -Z. Retract tool in –X: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts only in -X.
SolidCAM2005 Milling Manual 5-axis Machining Retract tool in +X: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts only in +X (Operation 7). Retract tool in –Y: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts only in -Y.
5-axis Machining SolidCAM2005 Milling Manual Retract tool in +Y: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Here the tool retracts only in +Y. Retract tool along surface normal: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder.
SolidCAM2005 Milling Manual 5-axis Machining Retract tool away from orign: Simulate the appropriate operation of Exercise11. The CAM-Part is located in the Exercises\Gouge_ check folder. Tool axis Surface normal Origin Retract tool cut to center: Cut center You need this gouge check option for Tool path tube milling. To avoid the gouge the cutter will be tilted to the cut center. The cut center is the center point of your enclosed geometry. This drawing shows a simple cutout through a tube.
5-axis Machining SolidCAM2005 Milling Manual 10.5.3 Tilting tool away with max angle If control by tilting tool away with max. angle is selected, then the gouge is avoided by tilting the tool. Below you can see the options that are given with the option with tilting tool away with max. angle to prevent gouging: The gouge checking requires a lot of computing time. So the best approach is to use limit angles, tilt angles etc.
SolidCAM2005 Milling Manual 5-axis Machining Use lead/lag angle: The tool tilts horizontally with a 90 degrees angle orthogonal to the surface normal. -90° Surface normal +90° Tool Axis Use lead/lag angle and side tilt angle -90° +90° Surface normal Tool Axis +90° -90° The tool tilts horizontally and vertically with a 90 degrees angle orthogonal to the surface normal.
5-axis Machining SolidCAM2005 Milling Manual 10.5.4 Leaving out gouging points Activating this option will cause the tool path to be trimmed when a collision is detected. Check surface 10.5.5 Stop tool path calculation If you select the option Avoid by leaving out the tool, the tool path will be created only until the first gouge is detected. First gouge Here you can see that the next cut would cause contact with the check Check surface surface. The tool path was created until the stop position.
SolidCAM2005 Milling Manual 5-axis Machining 10.6 Drive Surfaces This switch should be set to true if collision control is performed with the drive surfaces passed by the user. 10.7 Check Surfaces This switch should be set to true if collision control is performed with the check surfaces passed by the user. E.g. if collision control operation Nr. 3 is used, then the user needs to pass Check Surfaces 3 as geometry to the interface. 10.
5-axis Machining SolidCAM2005 Milling Manual 11. Stock Page If this switch is set to true, then the surfaces or triangle meshes must be provided to the library to define the stock or remaining stock from the last operation. This information is then used to allow only tool path segments that are removing chip (material) from this given stock. E.g. if multiple cuts are used, the stock definition will allow the library to eliminate air cuts.
SolidCAM2005 Milling Manual 5-axis Machining 12. Additional parameter Page The following parameters in this page are implemented to handle very exceptional cases. Please ignore this page unless you are advised otherwise. Read last operation flag reads the last operation in the operation manager and creates a 5 axis tool path based on that. This “base operation” can be any 3 axis or 5 axis operation. In such a case 5axmsurf is used to modify the tool angles or to do a gouge checking.
5-axis Machining SolidCAM2005 Milling Manual 13. Appendix 13.1 Single Surface versus Multi Surface Machining in 5 Axis Due to increased availability and lower pricing of 5 Axis Milling machines and recent developments from the controller side (Fanuc etc.), the need for information about 5 Axis machining has recently increased dramatically. This publication tries to as easily and clearly as possible address one common question about 5 Axis machining of multiple surfaces.
SolidCAM2005 Milling Manual 5-axis Machining Each surface point is associated with a surface normal that is always perpendicular to the surface at that point. Surface Normal In 3 axis machining this surface normal for a ball end mill points to the cutter center. The cutter axis always comes from one direction, usually it is aligned with Z. In some rare cases the cutter is aligned with the Y axis.
5-axis Machining SolidCAM2005 Milling Manual In 5 Axis machining the surface normal may not only determine the cutter center but the cutter orientation as well (there are other ways to control the tool axis to achieve a 5 axis machining tool path, but this will be discussed later): A Flowline 5 Axis tool path follows only the u-direction and v-direction of the surface. In the subsequent figure, a 5 axis flow line tool path is shown which is mainly calculated in the u-direction.
SolidCAM2005 Milling Manual 5-axis Machining On a real machine the machine has to move its axis to rotate the tool to the required direction as shown below.
5-axis Machining 151 SolidCAM2005 Milling Manual
