Bit rises after each pass VCPro 10.514
Bit rises after each pass VCPro 10.514
I cut out a part using profile toolpath. The bit retracted above the material after each pass. The path had 8 passes to cut out the part, and the bit retracted each time it made a lap, then plunged to the next pass depth. I can't find anywhere in the toolpath setup that can control this. Any help? This really added a lot of machining time to the process, especially since there were 8 pieces to cut out. Thanks.
- FixitMike
- Vectric Wizard
- Posts: 2176
- Joined: Sun Apr 17, 2011 5:21 am
- Model of CNC Machine: Shark Pro Plus (retired)
- Location: Burien, WA USA
Re: Bit rises after each pass VCPro 10.514
If it is a slow plunge rate that is taking too much time, you can reduce the time spent plunging by setting a not very large value for Z2. in the Material Setup in the toolpaths window.
Good judgement comes from experience.
Experience comes from bad judgement.
Experience comes from bad judgement.
- sharkcutup
- Vectric Wizard
- Posts: 2918
- Joined: Sat Mar 26, 2016 3:48 pm
- Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
- Location: U.S.A.
Re: Bit rises after each pass VCPro 10.514
I use the spiral ramp option when cutting out parts. It is a continuous plunge cut throughout.
You could try that to see if it is to your desired toolpath condition.
Sharkcutup
You could try that to see if it is to your desired toolpath condition.
Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 12.004
YouTube Channel - Sharkcutup CNC
V-Carve Pro 12.004
-
- Vectric Craftsman
- Posts: 182
- Joined: Sat Jun 30, 2012 1:41 am
- Model of CNC Machine: CAMaster Stinger II
- Location: Wisconsin
Re: Bit rises after each pass VCPro 10.514
We’re you using leads options?
Charlie
Aspire, CAMaster Stinger II
Aspire, CAMaster Stinger II
- FixitMike
- Vectric Wizard
- Posts: 2176
- Joined: Sun Apr 17, 2011 5:21 am
- Model of CNC Machine: Shark Pro Plus (retired)
- Location: Burien, WA USA
Re: Bit rises after each pass VCPro 10.514
Any time there is Z movement along with X, Y, movement, the bit will move at whichever is the slowest of the pass or plunge speed. If your plunge rate is quite slow, so will be the pass speed when the bit ramps. You can speed it up by increasing the plunge rate of the tool in the tool description.
If that doesn't help, then post the file here and maybe someone else can figure out what is happening. I tried to duplicate the problem and could not (VCarve Pro 10.514).
If that doesn't help, then post the file here and maybe someone else can figure out what is happening. I tried to duplicate the problem and could not (VCarve Pro 10.514).
Good judgement comes from experience.
Experience comes from bad judgement.
Experience comes from bad judgement.
Re: Bit rises after each pass VCPro 10.514
Did not have leads turned on. Will try ramps. I am trying to eliminate the bit retracting then plunging back. This is wasted motion and time. The X & Y are not moving during this motion. It is like drill pecking, but it is on a profile cut. Is there a setting that commands the bit to retract each pass? Thanks
- adze_cnc
- Vectric Wizard
- Posts: 4367
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Bit rises after each pass VCPro 10.514
Before you start fiddling around with ramps and other complications we should try to figure out why a "plain vanilla" profile cut does this for you.
- what post-processor are you saving the toolpath with
- can you post a CRV file that exhibits this behaviour? You could make a copy of the original file and strip out all but the offending toolpath.
- can you post the file (g-code, tap, mmg, etc.) that you send to your machine that exhibits this behaviour?
- Adrian
- Vectric Archimage
- Posts: 14650
- Joined: Thu Nov 23, 2006 2:19 pm
- Model of CNC Machine: ShopBot PRS Alpha 96x48
- Location: Surrey, UK
Re: Bit rises after each pass VCPro 10.514
Are you machining an open vector? If so the profile toolpath will retract and return to the start point of the vector for each pass to respect the cut direction. With a closed vector it won't retract.
- Adrian
- Vectric Archimage
- Posts: 14650
- Joined: Thu Nov 23, 2006 2:19 pm
- Model of CNC Machine: ShopBot PRS Alpha 96x48
- Location: Surrey, UK
Re: Bit rises after each pass VCPro 10.514
Forgot to mention that if you are machining an open vector the retract will only behave like that if you are using the Left/Right option. If you are cutting On the vector then it won't retract between passes. That is assuming you're using 10.5 as before that all three options would retract on each pass.
Re: Bit rises after each pass VCPro 10.514
Thanks for your ideas. There are no open vectors. I tried ungrouping all and regrouping, recalculaterd toolpaths and saved new g code. I re ran the project, and I was wrong on first description. The profile pass only lifted up before final pass. However, the bit did lift up above material after each pocket pass. Any help or ideas are appreciated.
- Attachments
-
- sander extension discs end.crv
- (1.61 MiB) Downloaded 64 times
- Adrian
- Vectric Archimage
- Posts: 14650
- Joined: Thu Nov 23, 2006 2:19 pm
- Model of CNC Machine: ShopBot PRS Alpha 96x48
- Location: Surrey, UK
Re: Bit rises after each pass VCPro 10.514
You said profile toolpath up until now. Pocket toolpaths always work like that as the software doesn't know if there is material in the way of the move back to the start for the next pass. The only way to remove the retracts if you know it is safe to do so is to edit the g-code or use a profile toolpath with a spiral vector.
- adze_cnc
- Vectric Wizard
- Posts: 4367
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Bit rises after each pass VCPro 10.514
And the profile toolpath would retract for the final pass if you are using the last pass allowance setting.
One thing about the pocket toolpath that would be good is if it compared the current pass's XY end point with the next pass's XY start point. If they are the same then then no retract is necessary.
One thing about the pocket toolpath that would be good is if it compared the current pass's XY end point with the next pass's XY start point. If they are the same then then no retract is necessary.
Re: Bit rises after each pass VCPro 10.514
So how can I "tell" it where the last pass ended for the next path to begin?
I don't understand why the software wouldn't know where the material is, since it just removed the material during the pass.
I don't understand why the software wouldn't know where the material is, since it just removed the material during the pass.
- martin54
- Vectric Archimage
- Posts: 7349
- Joined: Fri Nov 09, 2012 2:12 pm
- Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
- Location: Kirkcaldy, Scotland
Re: Bit rises after each pass VCPro 10.514
Only way to do that would be to edit the gcode, if you can learn how to do that then there isn't much that will hold you back when it comes to running the machine..
As far as I know the software has no way of knowing what it has previously cut, there are software programs with much more advanced toolpath strategies if you want to spend that sort of money
- sharkcutup
- Vectric Wizard
- Posts: 2918
- Joined: Sat Mar 26, 2016 3:48 pm
- Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
- Location: U.S.A.
Re: Bit rises after each pass VCPro 10.514
Have you tried the Spiral Ramp noted above? I use it quite often and I have never seen the bit retract during the toolpath!!!I cut out a part using profile toolpath. The bit retracted above the material after each pass. The path had 8 passes to cut out the part, and the bit retracted each time it made a lap, then plunged to the next pass depth. I can't find anywhere in the toolpath setup that can control this. Any help? This really added a lot of machining time to the process, especially since there were 8 pieces to cut out. Thanks.
Or edit your G-code to remove bit retracts!!!
Sharkcutup
Last edited by sharkcutup on Sat Jun 05, 2021 5:40 pm, edited 1 time in total.
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 12.004
YouTube Channel - Sharkcutup CNC
V-Carve Pro 12.004