Wrong hole size with drilling toolpath
Wrong hole size with drilling toolpath
I drew a circular file with 10 evenly spaced through holes. I originally made each hole 1/4 inch and saved everything. Then I decided they should be 3/8". I changed the size and re saved the file. I deleted my first drilling toolpath and made a new drilling toolpath. I used a 1/4" end mill to cut the holes, but instead of 3/8 it cut them 1/4". I immediately went to the file and verified the holes were 3/8 and made a new toolpath, again 1/4" holes. Any thoughts?
- carbidetooth
- Vectric Apprentice
- Posts: 59
- Joined: Mon Apr 09, 2018 8:01 am
- Model of CNC Machine: ShopSabre Pro 408
Re: Wrong hole size with drilling toolpath
If I'm understanding right, I think I've done, (and was puzzled by) the same.
Drill toolpath goes straight down and assumes correct size cutter in collet. Cut as Pockets if you want 3/8" holes. At least that's what I concluded.
Drill toolpath goes straight down and assumes correct size cutter in collet. Cut as Pockets if you want 3/8" holes. At least that's what I concluded.
Re: Wrong hole size with drilling toolpath
Thanks, I thought that might be the case, but I appreciate your input.
- adze_cnc
- Vectric Wizard
- Posts: 4329
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Wrong hole size with drilling toolpath
Or use a drill path and a 3/8 cutter...carbidetooth wrote:Cut as Pockets if you want 3/8" holes. At least that's what I concluded.
- scottp55
- Vectric Wizard
- Posts: 4713
- Joined: Thu May 09, 2013 11:30 am
- Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP11.5
- Location: Kennebunkport, Maine, US
Re: Wrong hole size with drilling toolpath
A Inside Profile cut using a Spiral Ramp has always been my go-to.
Don't be shy with adding many small pass depths, and sometimes adding a ridiculously no-load small final pass for a cleaner hole if you have enough cutter length....it really doesn't add much time.
Control bit temp by adjusting plunge rate on some test holes to maintain room temp bit....measure holes, and add an offset to get perfect fit.
Bit should be 50-90% of the diameter of the hole.
For clean sidewalls and less tearout, consider a Fishtail cut EM.
Circle Resize gadget is PERFECT for what you just did manually....check it out:)
scott
Don't be shy with adding many small pass depths, and sometimes adding a ridiculously no-load small final pass for a cleaner hole if you have enough cutter length....it really doesn't add much time.
Control bit temp by adjusting plunge rate on some test holes to maintain room temp bit....measure holes, and add an offset to get perfect fit.
Bit should be 50-90% of the diameter of the hole.
For clean sidewalls and less tearout, consider a Fishtail cut EM.
Circle Resize gadget is PERFECT for what you just did manually....check it out:)
scott
Last edited by scottp55 on Thu Apr 04, 2019 1:21 am, edited 1 time in total.
I've learned my lesson well. You can't please everyone,so you have to please yourself
R.N.
R.N.
- TReischl
- Vectric Wizard
- Posts: 4596
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: Wrong hole size with drilling toolpath
Ummm, drilling is not the same as milling. Just thought I would toss that in here.
"If you see a good fight, get in it." Dr. Vernon Johns
Re: Wrong hole size with drilling toolpath
Thanks for everyone's help. I'll check out that hole gadget too, Scott.
This forum is such great resource with so many knowledgeable people.
This forum is such great resource with so many knowledgeable people.
- adze_cnc
- Vectric Wizard
- Posts: 4329
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Wrong hole size with drilling toolpath
For the original poster (OP) via Scott's comment: As the original posting specified both the initial and the replacement paths were drilling paths the OP didn't need to redraw the circles at all as the drilling path doesn't care what size of circle the vector is. I believe it doesn't really even care if it is a circle as long as it can find a centre.scottp55 wrote:Circle Resize gadget is PERFECT for what you just did manually....check it out:)
scott
Steven
- Mark
- Vectric Staff
- Posts: 1054
- Joined: Sat Aug 18, 2007 2:55 pm
- Model of CNC Machine: CNC Shark, ShopBot, Roland PNC3000
- Location: Alcester U.K.
- Contact:
Re: Wrong hole size with drilling toolpath
Hello,
As others have mentioned, the drilling toolpath will just consist of one, or a series of plunge moves,
altering the circle size will only ensure that previews are correct.
The actual hole size will always be whatever the tool diameter would result in.
Any closed vector of any shape can be selected for a drill toolpath, the plunge point will be at the center points of the selected vectors.
This enables 'circles' drawn in other CAD packages, that might quite crudely faceted, to be drilled, without having to modify
the geometry first.
Cheers,
Mark.
As others have mentioned, the drilling toolpath will just consist of one, or a series of plunge moves,
altering the circle size will only ensure that previews are correct.
The actual hole size will always be whatever the tool diameter would result in.
Any closed vector of any shape can be selected for a drill toolpath, the plunge point will be at the center points of the selected vectors.
This enables 'circles' drawn in other CAD packages, that might quite crudely faceted, to be drilled, without having to modify
the geometry first.
Cheers,
Mark.