SmartCAM Production Milling Trial: Task 5 ‐ Finish Profile the Pocket & Island
Task 5
Finish Profile the
Pocket and Island
You no longer need those Regions to be in the active group.
Remove them from the active group by left-clicking the Remove All icon on the group select toolbar.
We suggest that you suppress the existing toolpaths from the graphics view in order to visually simplify the graphics while you add the finish profiling toolpaths.
Right-click on the Step 10: Rough Milling item in the List View. Or remember that alternatively you can right-click on any part of the toolpath in the graphics view.
Left-click on the Mask/Unmask command on the menu.
The toolpath is suppressed from the graphics view.
You will be using a 10mm cutter to finish profile.
Select the STEP on which to generate the profiling process.
Left-Click on the gray box at the right-side of the Step: field.
Left-Click 20:Fin Mill in the drop-down list.
Open the Profile Process panel by left-clicking on the Wireframe Milling icon on the toolbar and left-clicking the Profile command on the drop-down list.
You are going to profile the pocket and island by applying the command to an active group containing those profiles.
Add the pocket and island to the active group by left-clicking the Profile icon on the group select toolbar and left-clicking on an element in each of the pocket and island profiles.
The profile command can be used to create toolpath for whole or partial profiles using options selected from the Profile Input field drop-down menu.
Ensure that Profile Input is set to Group. If not then left-click within the Profile Input field and select Group from the drop-down list.
The Offset side on which to create the profile toolpath should be set to left. If not then left-click within the Offset Side input field and select Left from the drop-down list.
Let’s machine those profiles in a single depth pass.
Left-click in the Depth of Cut: field and type in a value of 30, being deeper than the depth of the pocket.
Now check some options for the command by left-clicking on the More… button
On the Options tab of the panel that is displayed, note that the Profile command has its own clearance setting: It does
not use the global setting that is displayed in the Insert Properties Bar.
Left-click in the Clear Plane input field and type in the value 2. The cutter will retract to a safe height of Z2 between passes.
Left-click on the Leads tab.
Here you can add a lead-in / lead-out style to the profile and you can control the application of cutter compensation codes.
Left-click within the Lead In Style field and left-click on the Line/Arc option from the drop-down list.
A lead-in line and arc are calculated based upon the current tool diameter. Those values can be over-ridden if necessary.
Leave Lead Out Style as Match: The tool will approach and leave the profiles using line-arc moves.
Left-click Accept to close the parameters panel.
Left-click the Go button on the Profile panel.
Profile toolpaths with lead-in / out will be created for both profiles.
Notice that the outer profile is in a counter-clockwise direction and the island is clockwise.
With that Left offset side setting, those profile directions and with a clockwise spindle rotation you have generated climb-milling toolpath for those profiles.
It follows that in the Profile command you are able to control climb or upcut milling with permutations of profile direction and offset side.
For example, in order to upcut inside that pocket profile, it would be made a clockwise direction and an offset to the right applied.
Profile Start Point. The profile process uses the start point of the profile as a start point for machining.
Profile directions and start points are easily modified using commands in the Order Path task set.
Verify the results and / or generate CNC code if you wish. As a reminder, you can get details about Verification by clicking here
That completes Task 5. Next up: Programming the Hole Making Toolpaths..
