Wrong hole size with drilling toolpath

This forum is for general discussion about Aspire
Post Reply
tagguy
Posts: 35
Joined: Fri Aug 11, 2017 5:37 pm
Model of CNC Machine: ShopBot Desktop

Wrong hole size with drilling toolpath

Post by tagguy »

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 I originally made each hole 1/4 inch and saved everything.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?

User avatar
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

Post by carbidetooth »

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.

tagguy
Posts: 35
Joined: Fri Aug 11, 2017 5:37 pm
Model of CNC Machine: ShopBot Desktop

Re: Wrong hole size with drilling toolpath

Post by tagguy »

Thanks, I thought that might be the case, but I appreciate your input.

User avatar
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

Post by adze_cnc »

carbidetooth wrote:Cut as Pockets if you want 3/8" holes. At least that's what I concluded.
Or use a drill path and a 3/8 cutter...

User avatar
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

Post by scottp55 »

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
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.

User avatar
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

Post by TReischl »

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

tagguy
Posts: 35
Joined: Fri Aug 11, 2017 5:37 pm
Model of CNC Machine: ShopBot Desktop

Re: Wrong hole size with drilling toolpath

Post by tagguy »

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.

User avatar
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

Post by adze_cnc »

scottp55 wrote:Circle Resize gadget is PERFECT for what you just did manually....check it out:)
scott
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.

Steven

User avatar
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

Post by Mark »

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.

Post Reply