FreeCad Inlay (Part 3)

Part 2 ended with a face created in Draft Workbench.  This face will now be used in the Path Workbench.

1  Open a Job choosing Face in the first dialogue box.

2  Set the stock dimensions to have the diamond face sit on the top face of the stock.  In FreeCad speak the Z top bounding box extension should be zero.

3  For tool controllers select the 60 degree v-bit and create an end mill of 0.134" diameter.  An explanation of for the odd size end mill can be found at the bottom of this post.

4  The first operation will be adaptive clearing using the 0.134" end mill.  For the base geometry choose the 4 inside edges of the diamond.  Set the final depth of cut to -0.110".  The extra 0.010" depth provides a bit of margin of error when joining the pieces.  Some inlay makers will cut this deeper to give excess glue a place to go

5  The second operation is v-carving the face.  Select the face as the base geometry.  Select the v-bit cutter.  The other options are a bit of a mystery.

    This is roughly what the tool paths should look like.  Rotated 90 degrees here to save page space

click to enlarge

This is a view of the tool paths in Camotics.  The little 'pyramids' in the corners are spots the clearing end mill couldn't reach, easy to scrape out.  The gouges seen in the corners are real but not deep,  they are not visible in the assembled piece.

    This is the finished piece.  A bit of chipping on the top and bottom points as a result of over aggressive v-cutting of the inlay.  Overall not horrible.

 

Final thoughts

This was a lot of effort mostly due to the number of calculations and amount of planning involved.  The good news is a lot of this work can be recycled in future inlays. So can FreeCad make inlays ?  Yes and No.  The next post will show how the strategies used in this post can fall apart.

About that weird end mill

  What the image above attempts to show is the form created by the v-bit.  The yellow represents the base.  The black triangle needs to be removed.  The problem is the bottom of the V is not selectable in the FreeCad model.  To work around this I used an end mill 0.058" larger in radius than FreeCad 'believes' is being used.

Using a 0.250" diameter end mill:

0.250 - (2 * 0.058) = 0.134

A 0.134" tool controller is used to create the tool path.  For actual cutting a 0.250" is substituted.

Another approach would be creating an extra model representing the centre of the v-carve path.  There may be a third option but I don't know every trick available in FreeCad.