Any option for “clearing bit” for profile cutting?
Any option for “clearing bit” for profile cutting?
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?
- adze_cnc
- Vectric Wizard
- Posts: 4380
- 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?
Short answer: no
Slightly longer answer: FixitMike posted a solution to this sort of question here: viewtopic.php?p=195135#p195135
Slightly longer answer: FixitMike posted a solution to this sort of question here: viewtopic.php?p=195135#p195135
- FixitMike
- Vectric Wizard
- Posts: 2177
- 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?
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.
.
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.
.
Good judgement comes from experience.
Experience comes from bad judgement.
Experience comes from bad judgement.
- FixitMike
- Vectric Wizard
- Posts: 2177
- 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?
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.
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.
Experience comes from bad judgement.
Re: Any option for “clearing bit” for profile cutting?
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
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
- Adrian
- Vectric Archimage
- Posts: 14684
- 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?
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.