Toolpaths are created by applying operations to layers.  If you have several shapes in a layer they will all generate toolpaths when a operation is applied. On the same note, if you have multiple layers, you need to create an operation for each layer you want to create toolpaths for.

In our case we want a toolpath for the shaft hole, and a toolpath for the teeth.  These need to be separate operations since the shaft hole needs a inside cut and the teeth need an outside cut. This is the reason they were separated into two layers in the first place.

To start, select just the "Shaft hole" layer and click the "Create new contour" button shown here.

The Contour dialog will popup. Three fields need to be set before doing anything else.

  • Contour Method = Inside Offset
  • Layer = shaft hole
  • Tool = T1: 1/8 2 flute....


You will also have to set the cut depth.  In our case we want to rout through the .375 material so I have set the cut depth to .385. This will rout through the stock and into my waster board .01. 

Most of the other settings were picked up from our tool.  They are presented here in case you need to make adjustments.

If the settings from you tool dont transfer over, you can force them to by hitting hamburger button shown here.

Hit the update operations buttons and the settings should transfer.

Once you are satisfied with all your settings, click the OK button to create the toolpath.

The actual tool paths will show up in green on the drawing.  In this case there is very little movement so they are very tiny.  

The rapids will show up in blue.

Your operation will be listed in the operations pane.  If you deselect it the toolpaths will be hidden from the drawing. This can be helpful when dealing with complex jobs.


Repeat the process by selecting just the "Teeth" layer and hitting the "Create new contour" button shown here.

The only settings you need to change are the following:

  • Contour Method = Outside Offset
  • Layer = Teeth

All the other settings should have remained the same.  

There is one other thing we must do to the "Teeth" operation.  We need to add some holding tabs to keep it from shifting as we finish the cut.

To do this, go to the Cut path tab and hit the "Holding tabs" button shown here.

Make the settings the same as what I show here.  Don't hit the "Place tabs" button as this will automatically place the tabs and I currently dont know of a way to change them.

Clock the OK button.

Place the project into tab edit mode by hitting the "Edit tabs" button shown here.

Place 4 tabs at the locations shown here.

By clicking some of the buttons in the view tool bar shown with the first arrow, you can change what is shown in the drawing. Here I have turned on actual path width.

Also, if SheetCam notices something that did not go correctly during the path creation it will issue a warning or error as shown by the second arrow.  If it is a warning you can continue as the path was created.  If it is an error the path will not be created and the error must be corrected.

You now have your toolpaths created.  The only thing left is to export them so that Mach3 can run them.