FreeCad Inlay (Part 1)

This is a continuation of the previous v-bit post.  Please scan that first.

Disclaimer:  I am new to FreeCad.  There may be easier ways to do many of the things shown in this post.  FC v0.19 pre-release is being used in this post.

The SVG file used was downloaded from wikimedia.  I believe it's this https://commons.wikimedia.org/wiki/File:SuitDiamonds.svg 

 

Save 2 copies of the SVG file naming one Inlay and the other Base.  In this post the copy named Inlay will be used. 

Click image for larger size

In the image above the red base piece is cut to a depth of 0.100".  The aqua inlay piece is cut to a depth of 0.150".  The aqua part is being made in this post.

Making the inlay

1  Import the SVG into FreeCad Draft Workbench. (toggle off that annoying grid).  Use Modification -> upgrade to create a face.  This seems to work best if the fill is first removed in Inkscape.  If anyone tries to follow along without a knowledge of Inkscape things will get worse in Inlay (Part 2).  The SVG should be flipped horizontally in Inkscape before importing.  In this case the SVG is most likely symmetrical,  the point is inlays must be a mirror image of the base.

2  Open the Part Workbench and extrude the face to a thickness of 0.150".  In the extrude dialogue box skip Apply and hit OK.  Apply creates a redundant copy.

3  Create a cube the length and width of the stock material being used for the inlay.  Height isn't critical but the actual stock thickness minus 0.150" would be a logical choice.  Place the cube in the appropriate x-y position beneath the extrusion.  Lower the cube's z position by an amount equal to the cube's height.  If this went well there will be no gap between the pieces and the extrusion will protrude 0.150" from the top face of the cube.

4  Click on the extrusion and the cube and create a boolean union.  This should result in a single object named fusion.

5   Open the Path Workbench.  When creating the Job choose Fusion 0 in the first dialogue box.

6  In Job set-up window make the top of the stock level with the top of the model.  If any facing is needed take care of it beforehand.

7 For this operation a 0.250" tool controller was used.

8  Use a pocket tool path to clear the area around the diamond to a final depth of 0.150".  If this is done right the diamond shape should be all that remains of the original top surface.

9  Using a profile op cut around the perimeter of the diamond to a final depth of 0.150".  Adjust the step downs to something sane like 0.050".  In the profile operation deselect "Use Compensation".  The logical operation to profile the diamond is the engrave tool path but it's approximation of the curves was too crude.

10  Post the tool paths. Order of operations should be pocket followed by profile.

11  When cutting the profile tool path use a 60 degree v-bit in place of the 0.250" end mill. 

This was the easy half to explain.

Part 2 gets messier.