Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

male and female inlay pocket clearing

6 REPLIES 6
Reply
Message 1 of 7
dnoone38
155 Views, 6 Replies

male and female inlay pocket clearing

Hi,

 

I am trying to learn the process for machining inlays using a vcutter.  I am able to cut the shape that i designed using a vcutter using the and an engraving toolpath, but i am unsure best way to clear the remaining material to the end of the chamfer.  

 

For the female piece i am able to get an OK piece because i sitll have some of the chamfer, but i do not know how to pocket the piece to the end of the chamfer.

 

If anything is unclear please let me know and i will gladly clarify.  Any assistance on this is greatly appreciated!

 

Engrave toolpath

dnoone38_0-1699815256678.png

 

Pocket toolpath

 

dnoone38_1-1699815300308.png

 

 

For the male piece there is a wall around the outside of the chamfer that i do not know how to get rid of

 

Engrave toolpath

dnoone38_2-1699815455471.png

 

pocket toolpath

dnoone38_3-1699815488416.png

 

6 REPLIES 6
Message 2 of 7
djlunty
in reply to: dnoone38

@dnoone38  As you have discovered inlays with Fusion is not straight forward but it can be done.

For the pocket part  once you have done the initial engrave with the v-bit you have to use a pocketing tool path with stock to leave to clean out the material left in the middle of the star.

Assuming a Depth of cut of 0.200 inches and a 60 degree V-bit you would want a stock to leave of 0.115. inches.  Could run two tool paths with successivly smaller cutters to to get into the corners - use rest machining.

 

For the inlay part you first want to remove all the material around what will be the final part.  An adaptive tool path works for this with stock to leave so as not to cut into the final inlay.  In your case you used a pocketing tool path and that works - just do it first with stock to leave.  Now run the engrave tool path.  For the geometry select the bottom edge of the inlay and the model at the bottom of the inlay.  This selection will make the V-Bit go on the correct side.  Depth of cut is 0.200 same as for the pocket part.  Now to get the inlay part to fit into the pocket run another engrave tool path but this time Set the heights as follows:

     

djlunty_0-1699848039903.png

In your passes tab the maximum stepdown must be less than Bottom Height Offset from Top Height.  I use 0.05 with is less than 0.067 (ignore the sign for Top Height offset

djlunty_1-1699848232014.png

This should get you going  - if it doesn't work please attach your file and I will have a look at it.  

I have attached some information on this method.  The Recipe for Creating V-Carve Inlays is not mine.  V-Carve Inlay Technique May 11 is a document  that I created for myself with the exception of the first page.   Any questions just ask.

Doug

 

 

Message 3 of 7
djlunty
in reply to: dnoone38

@dnoone38 

Just got to looking at the document that I sent - I did it quite some time ago and it is probably the long way of doing inlays.  The principles apply but can be done with fewer tool paths - the roughing passes are really not needed - can go straight to the pocketing tool paths.  The geometry of the inlay will determine how many different cutters you use for the pocketing tool paths.  The more detail the smaller the cutter will have to be to remove all  the material in corners.   I had the roughing tool paths in there because of the tooling I was using,

Doug

Message 4 of 7
djlunty
in reply to: dnoone38

@dnoone38 

In case my previous instructions were unclear and/confusing here are a couple of files.  One with the star engraving and a second that shows the inlay fitting into the pocket.  

djlunty_1-1699855070683.png

Tools are for my CNC - 60 degree V-bit, 1/4 inch spiral, 1/16 inch spiral.  You may have different tools.

Doug

Message 5 of 7
dnoone38
in reply to: djlunty

Thanks for all the info Doug!  This really helped out.  I did notice in the file you sent for the inlay that there is still a small amount of material left in the corners after the last tool path, which makes sense sense the end mall is larger that the corners.   Any thoughts on how to eliminate that last bit of material?

dnoone38_0-1700067075946.png

 

Message 6 of 7
programming2C78B
in reply to: dnoone38

In wood I just knock it out with a chisel

In CAM you can do radial stock to leave on the V bit until it removes that final triangle of stock. It will take a while since the tool has no flat on it. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 7 of 7
djlunty
in reply to: dnoone38

@dnoone38 

you can do as @programming2C78B suggested - use a chisel.  To do it in CAM just use a bit smaller than the 1/8 inch bit I used.  Just duplicate the path and change the bit.  You could also redefine your V-Bit (give it a different name) to have a small flat (for example 0.010) and use it to do the final clearing - same pocketing tool path as the 1/8 inch bit. programming2C78B suggested this also - using the redefined bit will shorten the machining time as your bit now has a flat instead of a sharp point.

Doug

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report