Inlay Toolpath and pockets
- sylvan356
- Vectric Craftsman
- Posts: 174
- Joined: Thu Dec 12, 2013 5:28 pm
- Model of CNC Machine: CAMaster Stinger 1 w/Rotary, Aspire 12
- Location: Ormond Beach, Florida
- Contact:
Inlay Toolpath and pockets
I think I know how to do this but I would like some confirmation from anyone who is doing this. I want to use the inlay toolpath. The toolpath requires that you use the same bit for the male and female parts. So, I want to cut out the male inlay (pearl) with a .023” bit. Now I need to cut the female (pocket) with a .023” bit. However the inlay is so large that will take hours to cut the pocket. So my question is can I cut the female (pocket) with the pocket toolpath using the .023” bit BUT adding a larger clearance tool to speed up the process. My thinking is that the .023” will cut the portions not cut by a larger bit achieving the same result as if I used a .023” for the entire female pocket. Does this make sense. Comments!
-
- Vectric Craftsman
- Posts: 298
- Joined: Thu Aug 21, 2014 8:13 pm
- Model of CNC Machine: ULS M300, Rockler 60th Ann. Shark
- Location: Dallas, TX USA
- Contact:
Re: Inlay Toolpath and pockets
that need not be the case. I regularly use a larger bit (1/8" or larger) to cut my pockets followed by an internal profile cut with a (1/16) to clean up the sharp corners and missed pieces from the larger bit. It basically boils down to how many sharp corners you have. If necessary hog it out with as big as you can go, and set up a special geometry to clean up with the smaller bit.sylvan356 wrote:The toolpath requires that you use the same bit for the male and female parts.
You need not use the inlay profile tool either - these can be just plain pocket and profile cuts. cheers!
"Out of my mind. Back in 5 Minutes."
- FixitMike
- Vectric Wizard
- Posts: 2177
- Joined: Sun Apr 17, 2011 5:21 am
- Model of CNC Machine: Shark Pro Plus (retired)
- Location: Burien, WA USA
Re: Inlay Toolpath and pockets
You can use an earlier work-around to prepare the vectors for inlaying. Offset outward by the tool radius (plus .001 so program rounding doesn't produce a place that your bit won't fit), then inward twice by the same amount, then back outward. The result will be vectors for your inlay that can be cut with the pocket toolpath that can use 2 tools.
Use the VCarve toolpath, specifying a V bit of .05 degrees included angle, plus the end mills you want to use. Then just use the end mill toolpaths.
If you want to use more than two tools,and you have version 10 use my hack:Use the VCarve toolpath, specifying a V bit of .05 degrees included angle, plus the end mills you want to use. Then just use the end mill toolpaths.
Good judgement comes from experience.
Experience comes from bad judgement.
Experience comes from bad judgement.
-
- Vectric Craftsman
- Posts: 253
- Joined: Fri May 09, 2014 1:37 pm
- Model of CNC Machine: Laguna IQ
- Location: Pensacola FL
Re: Inlay Toolpath and pockets
Maybe I'm missing something in the question, but right there in the female inlay toolpath window there is a box you can check for "use larger area clearance tool." I regularly use this for inlays. Simulate the toolpath to see how much the larger tool cuts, and figure out which size larger mill optimizes things. Then you use the smaller tool for the final cut.
- FixitMike
- Vectric Wizard
- Posts: 2177
- Joined: Sun Apr 17, 2011 5:21 am
- Model of CNC Machine: Shark Pro Plus (retired)
- Location: Burien, WA USA
Re: Inlay Toolpath and pockets
You are absolutely right. It is just not there for cutting the male insert piece. And in most cases it would be unnecessary, except for the case where the the male piece has a large internal hole that one wants to pocket rather than profile. Can I wipe the egg off my face now?litzluth wrote:Maybe I'm missing something in the question, but right there in the female inlay toolpath window there is a box you can check for "use larger area clearance tool." I regularly use this for inlays. Simulate the toolpath to see how much the larger tool cuts, and figure out which size larger mill optimizes things. Then you use the smaller tool for the final cut.
Good judgement comes from experience.
Experience comes from bad judgement.
Experience comes from bad judgement.