Any option for “clearing bit” for profile cutting?

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro
Post Reply
Marty3450
Posts: 2
Joined: Tue May 04, 2021 10:14 pm
Model of CNC Machine: Onefinity

Any option for “clearing bit” for profile cutting?

Post by Marty3450 »

I’m relatively new to Vectric. I’m using Vcarve Pro. I’ve done a few carves on my woodworking CNC but curious to know if there is any option for profile cutting similar to pocket carving where you can start with a larger bit and use a smaller bit just for inside corners? Is there anyway to configure this?

User avatar
adze_cnc
Vectric Wizard
Posts: 4303
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Any option for “clearing bit” for profile cutting?

Post by adze_cnc »

Short answer: no

Slightly longer answer: FixitMike posted a solution to this sort of question here: viewtopic.php?p=195135#p195135

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Any option for “clearing bit” for profile cutting?

Post by FixitMike »

It can be done, but is somewhat complex. This description is for using a 3/8" profiling bit and a 1/16" finishing bit. The numbers used are to show the method only.
1. Add a dummy V-bit with a 0.1 degree included angle in the tool data base. (That's right: 0.1 degrees.)
2. Offset the profile outwards .400". (A bit more than the profiling bit diameter.)
3. Select both the original profile and the offset. Set up a VCarve toolpath:
- A. Flat depth equal to material thickness (Or possibly a tad more.)
- B. Use the dummy V-bit, and a 1/16, and 3/8" clearance bits.
- C. Calculate the toolpath. Use only the VCarve toolpath for the 1/16" bit.
4. Calculate the Profile toolpath for the 3/8" bit. Include tabs if desired.
5. Cut the piece out using the profile toolpath and the 1/16" toolpath from the VCarve calculation.
Rest machine star.jpg


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

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Any option for “clearing bit” for profile cutting?

Post by FixitMike »

And, a similar method using a Pocket toolpath. This also uses 1/16" and 3/8" bits.

1. Add a dummy end mill with a .001" diameter to the tool data base. (That's right: 0.001" diameter.)
2. Offset the profile outwards .400". (A bit more than the profiling bit diameter.)
3. Select both the original profile and the offset. Calculate a Pocket toolpath:
- A. Flat depth equal to material thickness (Or possibly a tad more.)
- B. Use the dummy .001" dia. end mill, and 1/16, and 3/8" clearance bits.
- C. Calculate the toolpath. You will use only the Pocket toolpath for the 1/16" bit. ( Probably "Pocket 1 [Clear 2]".)
4. Calculate the Profile toolpath. Use a 3/8" bit. Include tabs if desired.
5. Cut the piece out using the Profile toolpath and the 1/16" toolpath from the Pocket toolpath calculation.
Good judgement comes from experience.
Experience comes from bad judgement.

Marty3450
Posts: 2
Joined: Tue May 04, 2021 10:14 pm
Model of CNC Machine: Onefinity

Re: Any option for “clearing bit” for profile cutting?

Post by Marty3450 »

Thanks for the feedback guys. A few things for me to try.

I wonder if that is something they would ever consider adding in the future. I'm surprised it has never been recommended before.

Thanks again

User avatar
Adrian
Vectric Archimage
Posts: 14504
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Any option for “clearing bit” for profile cutting?

Post by Adrian »

Depends how many (if any) people have asked for it directly to Vectric. I can only remember it coming up once or twice in all the years I've been on the forum. I can think of many other things that come up on a monthly basis that aren't in the software (yet) so it's all a question of priorities with a small company I would guess.

Post Reply