How to Create a Multiaxis Parallel Cuts Operation

Introduction

This tutorial explains how to create a Multiaxis feature with the ParallelCuts toolpath.This toolpath creates parallel cuts along a selected surfacegeometry.Only a Drive Surface selection is required for the feature,which can be one or more surfaces.

Example File

If you are connected to the Internet, the part file for this example can be downloaded automatically by clicking the following link: Parallel CutsExample 1.bbcd

Once you download and saved the zip file, extract the files on your system in an easy place to remember.You can then open the file to use with this tutorial.All files for the tutorials in this help system available for download can be found by clicking on the following link: http://www.bobcad.com/helpfiles.

In the example fileprovided, the stock and Machine Setup are already defined for the part.The part is simulated using the BC Table Table machine.

In this example, a finishing toolpath strategy is applied to the curvedface of the part model.You learn how the surface normal direction definesthe tool orientation and how to apply a tilting strategy to change thisorientation and resolve a gouge.You also examine how changing the Linkparameters modifies the toolpath and tool/machine movement.The last partexplains applying a gouge check to the model.

Part 1) Add the Feature

1. In the Data-CAMTree Manager, click the CAM Tree tab.
   
   

2. Right-click MachineSetup and click Mill Multiaxis.
   
   

3. In the MultiaxisWizard, click Surface,and confirm that Parallel Cutsis selected.
   
   

4. Click Next>>to go to the Posting settings.

Part 2) Define the Posting Parameters

1. The Work Offset # is automatically set tothe value defined in the Machine Setup.
   
   You can change the value here to update the Work Offset # for the feature.
   
   

2. Click Next>>to go to the Multiaxis Posting settings.

Part 3) Define the Multiaxis Posting Parameters

1. Notice, at the top of the dialog box, that the Use Machine Settings checkbox is selected.
   
   This means that the Multiaxis Posting parameters for the feature usethe same parameters as the machine that is selected in Current Settings.
   
   You can clear the Use Machine Settingscheck box to define the Multiaxis Posting parameters of the featureseparately from the current machine settings.
   
   An example usage is explained later.
   
   

2. Click Next>>to go to the Tool settings.

Part 4) Define the Tool Parameters

1. In the ToolData group, confirm the Diameter is set to 0.500.
   
   

2. Change theCorner Radius value to0.250so the software searches and loads a matching tool from the Tool Library(System Tool is selected).
   
   

3. Click AssignTool Holder.
   
   

4. On the right side of the Milling Tool HolderLibrary, click to select the 0.5inch I.D. Arbor CAT 40 holder and click OK.
   
   

5. Click Next>>to go to the Parameters.

Part 5) Select Geometry

1. In the Patterngroup of the Surface Pathstab, click Drive Surfaces.
   
   Click to select the front face of the model as shown next.
   
   The Drive Surface selection determines where the toolpath is applied.
   
   
   
   

2. To confirm the selections, click OK.

Part 6) Feature Setup

1. In the Patterngroup, click Constant Z.
   
   Notice that this sets the Machine Angle in Z parameter to 0 and disables the Machine Angle in XY parameter.
   
   This is used to create toolpath cuts that have a constant Z-axis value.
   
   

2. Under Sorting,confirm the Cutting Methodis set to One Way.
   
   

3. At the top of the dialog box, click Link.
   
   Click Retracts.
   
   Confirm that the Directionis set to ZAxisand the Height is set to 4.75
   
   This value is automatically set from the value defined in the MachineSetup (but only when the feature is created).
   
   You can change the value here to update the Clearance Plane after creatingthe feature.
   
   Click OK.
   
   

4. At the bottom of the dialog box, click Compute.

Notice that the toolpath Links are retractingto the Clearance Area between each slice.

You can also see that no lead-in or lead-outis defined.

5. To edit the feature, in the CAMTree, right-click FeatureMultiaxis,and click Edit.

Part 7) Edit the Links

1. On the left side of the dialog box, clickParameters.
   
   Click the Link tab.
   
   

2. In the Entry/Exitgroup, for First Entry, (onthe right side) select Use Lead-In.
   
   To open the Lead-In dialogbox, click .
   
   Confirm that the Use Default Lead-Incheck box is selected, and click OK.
   
   

3. Next toLast Exit, (on the right-side) select UseLead-Out.
   
   

4. To open the DefaultLead-In/Out dialog box, at the bottom of the dialog box, clickDefault Lead-In/Out.
   
   In the Lead-In group, nextto Type, select TangentialLine.
   
   Next to Copy, click .
   
   Click OK.
   
   

5. In the LinkBetween Slice group, set the LargeMoves to Retract to RapidDistance.
   
   (To view the current distance values in the Retracts dialog box, clickRetracts.)
   
   

6. To update the changes, click Compute.

The result shows that the First Entry and Last Exit moves now use aLead-In and a Lead-Out.Also, instead of the tool retracting to the ClearancePlane at the end of each slice, it now retracts to the Rapid Plane.(Theserapid moves are shown in yellow.) You can compare these results to thetoolpath result shown earlier.Notice that the yellow rapid moves arein front of the selected drive surface and not above it as it was earlier.This is the difference between Retract to Clearance Area and Retract toRapid Distance.

Part 8) Simulation

1. In the quick access toolbar, of the CAM Tree Manager, click .
   
   To learn more about using simulation, view GettingStarted with Simulation.
   
   

2. When you simulate the program, you see thatthe tool orientation is always the same as the surface normal directionalong the surface.

During simulation, you can also see thatthe part is gouged because of the short tool length.The gouge happensat the end of the toolpath, because there is not enough clearance betweenthe lower surface and the tool holder.

This issue could be resolved by using a longertool, but maybe you don't have a longer tool to use for the job.

This can be resolved by changing the tiltingstrategy or using a gouge check as explained later.

3. To close simulation, click Exit Simulation.

Adjust the Machine Table Rotation

When you simulate the program, the machine table is sometimes rotatedin a way that doesn't allow you to view the part without rotating theview of the machine.You can change the Angle Pair settings for the featureto modify the table rotation used in simulation and in the posted code.

1. To edit the feature, in the CAMTree, right click FeatureMultiaxis,and click Edit.
   
   

2. Click theMultiaxis Posting icon in the tree.

Clear the UseMachine Settings check box.

In the AnglePair group, next to Use,select Other Solution.

When you simulate the program again, youcan now view the part being cut from the opposite side of the machine.

The table is rotated to use the other solutionto the rotation angles of the primary and secondary rotary axes (anglepair).This changes the posted output of the program as well as the simulation.

Tip: You don'thave to compute the toolpath to update this setting for simulation, butyou must Post the program to update the code if has already been posted.

Part 9) Using Tool Axis Control

In this part of the tutorial, you use the Tool Axis Control tab to tiltthe tool orientation away from the bottom surface.

1. Edit the feature, click Parameters,and click the Tool Axis Controltab.
   
   

2. Next to ToolAxis Will, the Tilting Strategy is set to TiltedRelative to Cutting Direction.
   
   This tilting strategy uses the surface normal direction to define thetool orientation.In addition to this tool orientation, you can definea lead angle (forward and backward) and a side angle (left or right)based on the direction that the tool is moving.
   
   

3. To tilt the tool to the right of the toolpathbased on the cut direction, in the TiltAngle at Side of Cutting Direction, type 45.00.
   
   

4. Click Compute.
   
   The tool tilting is visible in the toolpath display.
   
   This has caused the rapid movements (links) to move up away from thebottom surface.
   
   
   
   

5. To simulate the program, on the Othertoolbar, click .
   
   During simulation, you can observe that the tool orientation is nowtilted 45 degrees to the right of the toolpath (in the cutting direction).
   
   
   
   Because of the new tool orientation, the tool holder no longer gougesthe part.
   
   

6. On the Othertoolbar, click Exit Simulation.

Part 10) About Flip Step Over

When using the Tilt Angle at Side of Cutting Direction parameter, itis important to understand the result created when using Flip Step Over.

1. Edit the feature, and click Parameters.
   
   

2. In the SurfacePaths tab, in the Sortinggroup, select the Flip Step Overcheck box.
   
   

3. Change the CuttingMethod to ZigZag.
   
   

4. Click Compute.
   
   Because of the two previous settings, the toolpath now starts at thebottom-left corner of the surface and ends at the top-right corner.
   
   Also, the toolpath now alternates the cutting direction for each slicewhich eliminates the retract and rapid moves.
   
   
   
   

5. Simulate the part to view the result.

Simulation shows that the tool orientationis still tilted 45 degrees in the same direction as it was previously,even though the toolpath is now cutting in both directions.

Tip: To causethe tool side tilt angle to change orientation with each alternating slice,you must enable Allow Flipping Side Direction.To enable this parameter,in the Tool Axis Control tab,next to Side Tilt Definition,click Advanced.In the Advanceddialog box, select the Allow Flipping Side Directioncheck box.

Part 11) Using Gouge Check

The Gouge Check tab is used next to check the program and correct anyfurther gouges.

1. Edit the feature and navigate to the Gouge Check tab.
   
   

2. To turn on a gouge check: in the Statuscolumn, above 1, select the check box.
   
   In the Check group, selectthe four check boxes for the Flute, Shaft, Arbor, and Holder.
   
   

3. In the Strategyand Parameters group, in the first box, select TiltTool.
   
   In the next box, select Use Side TiltAngle.
   
   

4. To check the values used, click Parameters.

Confirm that the Parametersdialog box shows a Max.Tilt Angleof 90 degrees and a Min.Tilt Angle of -90.

Tip: The MaximumTilt Angle (range of 0 to 180 degrees) determines the amount of tiltingto the left of the cutting direction when using Use Side Tilt Angle.(Whenusing Use Lead/Lag Tilt Angle this determines the amount of tool tiltingforward or towards the cutting direction.) The Minimum Tilt Angle (rangeof -180 to 0 degrees) determines the amount of tilting to the right ofthe cutting direction.(When using Use Lead/Lag Angle, this determinesthe amount of tilting backwards from the cutting direction.)

Set the ClearanceAngle to 3 degrees.

Click OK.

5. In the Geometry group, the Drive Surfaces and CheckSurfaces check boxes are selected.

To select the CheckSurfaces, or the surfaces that are gouge checked, click .

Click and drag a window around the entirepart to select all surfaces.

Click the Drive Surface to remove it fromthe selection.

The resulting selection appears as follows.

Click .

To calculate the gouge check, click Compute.

You can compare the results of using theside-tilt angle or creating a gouge check by using only one or the otherto calculate the toolpath and then simulating each result.

Tip: When gougechecking a feature, you should always try to get the feature as closeas possible to the desired result before you add the gouge check.Thisway you are only using the gouge check to make small changes to the toolpath.The point here is that you should not rely on the gouge check to fix apoorly created toolpath.

This concludes the tutorial.

Related Topics

ParallelCuts