Inlay Toolpath and pockets

This forum is for general discussion about Aspire
Post Reply
User avatar
sylvan356
Vectric Craftsman
Posts: 148
Joined: Thu Dec 12, 2013 5:28 pm
Model of CNC Machine: CAMaster Stinger 1 w/Rotary, Aspire 10
Location: Ormond Beach, Florida

Inlay Toolpath and pockets

Post by sylvan356 »

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!

nicksilva
Vectric Craftsman
Posts: 295
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

Post by nicksilva »

sylvan356 wrote:The toolpath requires that you use the same bit for the male and female parts.
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.
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."

User avatar
FixitMike
Vectric Wizard
Posts: 1709
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

Post by FixitMike »

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.
Inlay.JPG
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.

litzluth
Vectric Craftsman
Posts: 124
Joined: Fri May 09, 2014 1:37 pm
Model of CNC Machine: Laguna IQ

Re: Inlay Toolpath and pockets

Post by litzluth »

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.

User avatar
FixitMike
Vectric Wizard
Posts: 1709
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

Post by FixitMike »

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.
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?
Good judgement comes from experience.
Experience comes from bad judgement.

Post Reply