inlay toolpath

Post general information and questions relating to Cut2D in this Forum.
Post Reply
Jon Grey
Posts: 8
Joined: Fri Feb 12, 2021 1:02 am
Model of CNC Machine: sainsmart Genmitsu PROVerXL 4030

inlay toolpath

Post by Jon Grey »

I am new to cnc, I have a Genmitsu PROVer XL 4030 machine paid about a grand for it. My goal is to inlay abalone letters about 1/2 " height into guitar neck headstock, I build guitars as a hobby and have done inlays by hand.
My issue is I cut out some beautiful abalone letters, JG -my initials, but when I cut the pocket for them they don't quite match. I use a
.6 mm dental bit (end mill) and have tried everything I can think of including adding the allowance for the pocket, changing bit sizes, using slightly larger letter size, etc. what am I doing wrong, ? it seems so straight forward.

User avatar
Adrian
Vectric Archimage
Posts: 11914
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: inlay toolpath

Post by Adrian »

In what way are they not matching? Specific places or just too big/small all over?

When you're cutting different materials especially with a bit that small you are going to run into differences of how the two materials cut which is where the allowance comes in. There's always a bit of testing needed to get the right settings.

Jon Grey
Posts: 8
Joined: Fri Feb 12, 2021 1:02 am
Model of CNC Machine: sainsmart Genmitsu PROVerXL 4030

Re: inlay toolpath

Post by Jon Grey »

Thank you for your interest, the pieces mis-match generally all over, jut outs in different places thickness of vectors different, it wants to fit but will take some difficult hand work to make it happen, as for the machining it seems extremely well done I run at a slow speed 5" per min. and the cuttting looks really good.

User avatar
Adrian
Vectric Archimage
Posts: 11914
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: inlay toolpath

Post by Adrian »

I would suspect bit or machine deflection in that case especially with the machine you're using. They aren't the most rigid of machines.

If you could attach the file then it could be checked for any issues.

Jon Grey
Posts: 8
Joined: Fri Feb 12, 2021 1:02 am
Model of CNC Machine: sainsmart Genmitsu PROVerXL 4030

Re: inlay toolpath

Post by Jon Grey »

I will try to attach the file bu
JGPOCKET INLAY225BOLD SCRIPT.crv
(395 KiB) Downloaded 44 times
t I have to figure out how to do it. Oops looks odd ,oh well. Your making me cringe when you say this machine isn't rigid, I was so impressed with it's construction and movement .

User avatar
Adrian
Vectric Archimage
Posts: 11914
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: inlay toolpath

Post by Adrian »

There are some crossovers in that font (left side of the f) but nothing that affects the toolpath.

I notice you only have the female pocket toolpath. What toolpath did you use to cut the male part? If it was a profile toolpath rather than the Male Inlay one then that might be the issue.

Jon Grey
Posts: 8
Joined: Fri Feb 12, 2021 1:02 am
Model of CNC Machine: sainsmart Genmitsu PROVerXL 4030

Re: inlay toolpath

Post by Jon Grey »

No it was the male inlay. Actually I tried every approach I could think of but of course the inlay toolpath was the one I expected to work,
I just tried another one, pocket inlay and it looks better, I am going to my shop to see if I can fit it in without breaking it,

User avatar
sylvan356
Vectric Craftsman
Posts: 163
Joined: Thu Dec 12, 2013 5:28 pm
Model of CNC Machine: CAMaster Stinger 1 w/Rotary, Aspire 10.5
Location: Ormond Beach, Florida
Contact:

Re: inlay toolpath

Post by sylvan356 »

I do a great amount of pearl inlay into a wood substrate (guitars). I have found that 1) you absolutely need to use the inlay tool path because it takes into account the interior corners being automatically radiused to fit the bit that cut the pearl (same bit for pearl and pocket), 2) you need to have an offset on the wooden pocket portion of .005-.008" larger so the pearl will fit snugly, but it will fit, and 3) you need to do the inlay immediately or within about 15 minutes as the wood will swell making the pocket too small.

litzluth
Vectric Craftsman
Posts: 145
Joined: Fri May 09, 2014 1:37 pm
Model of CNC Machine: Laguna IQ

Re: inlay toolpath

Post by litzluth »

I have also found that the sequence you run the toolpaths can be your friend, particularly if you are experimenting with a new material or a new mill. If you cut the male portion first, you can leave a smaller pocket allowance in the female and shoot for a tight fit. Cut the female, but don't unclamp it. Do the test fit, and if it is still too tight, adjust the female toolpath allowance, test fit again. Repeat prn. By the way, any tiny bit is going to flex a bit differently cutting wood versus abalone or MOP. Two other tips: First, as Sylvan says, the inlay toolpath will help the radiused areas fit better given the radius of the bit you are using. I have also found that if you toggle toolpath 2D drawing visibility on, you can make small vector changes that may allow the fit to be even better. Second, make sure you wear a respirator and clean up well when you are cutting abalone or MOP. The dust is quite harmful.

Jon Grey
Posts: 8
Joined: Fri Feb 12, 2021 1:02 am
Model of CNC Machine: sainsmart Genmitsu PROVerXL 4030

Re: inlay toolpath

Post by Jon Grey »

Thankyou both for your assistance! I think with time and practice I will get better results.

Post Reply