Roughing Vs Finishing toolpath

This forum is for general discussion regarding VCarve Pro
monlover
Vectric Craftsman
Posts: 113
Joined: Wed Sep 17, 2014 6:53 am
Model of CNC Machine: Omnitech 4X8 with 8 tool

Roughing Vs Finishing toolpath

Post by monlover »

Hi, is it normal the roughing toolpath takes a way longer than the finishing path?
at his example the roughing toolpath takes 8 hrs and if i ran the finishing path from scratch it takes 3 hrs and 51 min

roughing using 1/4 ball nose at 12000 and 100 Ipm
and finishing using 1/4 ball nose at 12000 and 100 ipm also.
plunge at 35ipm
thank you for your help in advance.
Attachments
roighing
roighing
finishing
finishing

User avatar
Xxray
Vectric Wizard
Posts: 2107
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Roughing Vs Finishing toolpath

Post by Xxray »

No, its not normal - Check your stepover on roughing, jack it up to 40% or so, also would be better off using an endmill for roughing
Doug

User avatar
Adrian
Vectric Archimage
Posts: 10228
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Roughing Vs Finishing toolpath

Post by Adrian »

Other thing to check is the pass depth. The roughing toolpath is done in multiple passes if the needed cut depth is more than the pass depth of the tool. The finishing pass is always done in one pass. If you've got a very small pass depth on the roughing tool it could be taking lots of passes. I expect, as Xxray suspects, that the stepover is the biggest issue.

User avatar
dealguy11
Vectric Wizard
Posts: 1513
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA
Contact:

Re: Roughing Vs Finishing toolpath

Post by dealguy11 »

Another thing to think about. Are you cutting this on your Omnitech or on your other machine? What material are you cutting?

If this is on the Omnitech you might consider increasing the feed rate on your tools. A 1/4" ballnose can go pretty fast on carving. Try setting it to at least 200 ipm. It probably won't go any faster than that because of the amount of z movement but it's worth a try. For roughing, it should be able to go much faster than 100 ipm, and as others have suggested you might want to use an end mill rather than the ball nose.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com

Mikehell
Vectric Craftsman
Posts: 155
Joined: Wed Mar 22, 2017 9:34 pm
Model of CNC Machine: eBay special China 3040

Re: Roughing Vs Finishing toolpath

Post by Mikehell »

I use a normal flat 1/4" bit for roughing and not a ballnose and it works fine. I set it to take shallower passes and less stepover and it seems to work ok. It leaves just enough meat on the bone for a small ballnose to take off. I sometimes run the finish pass pretty fast. Set the plunge rate these same as the feed rate.

monlover
Vectric Craftsman
Posts: 113
Joined: Wed Sep 17, 2014 6:53 am
Model of CNC Machine: Omnitech 4X8 with 8 tool

Re: Roughing Vs Finishing toolpath

Post by monlover »

Flower_Box_3_TP.png
Hello every one,
thank you for your great help,
after some toolpath modification, and did not have a chance to run the actual file here is some results:
as you can see the time decreased a lot, the finish toolpath now is 3:39

below is my tool setup:
using Zenbot CNC 4X4 with Hitachi Metabo router 11 Amp
roughing using 1/4 end mill down cut at 100 FR and 100 Plunge rate
Finish toolpath using 1/8 Ball Nose at 100 FR and 100 Plunge rate
Profile toolpath using 1/8 End mill down cut at 50 FR and 20 Plunge rate

is 5 hours and 13 minutes is reasonable time for 12X12 inch poplar material.
this is my fires carving project and do not know time needed for such projects.
Thank you for your help.
Attachments
Final.png

User avatar
Xxray
Vectric Wizard
Posts: 2107
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Roughing Vs Finishing toolpath

Post by Xxray »

mon, we would get more useful into seeing the box that pops up when you click tool edit rather than the summary. Others can elaborate on this more than me, but the time estimation is just a wild guess until its calibrated to your particular machine so it may or may not reflect what would actually happen time wise if you ran the file.
I can say that 5 hours for a detailed 12x12 3d carving is not excessive, if there are no concerns with the preview you should try it.
Doug

monlover
Vectric Craftsman
Posts: 113
Joined: Wed Sep 17, 2014 6:53 am
Model of CNC Machine: Omnitech 4X8 with 8 tool

Re: Roughing Vs Finishing toolpath

Post by monlover »

xxry, at the Right section, at the toolpath can not find any tool edit button, I am guessing you are asking for the details for the attached tool path details?
Attachments
edit_tp.png

User avatar
scottp55
Vectric Wizard
Posts: 3574
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10
Location: Kennebunkport, Maine, US

Re: Roughing Vs Finishing toolpath

Post by scottp55 »

AT the very top of that pic Mon...in Tool category...that will show feeds and stepover.
scott
"One accurate measurement is worth a thousand expert opinions"

GMH


scott

User avatar
Rcnewcomb
Vectric Wizard
Posts: 3802
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: GCnC/WinCNC
Location: San Jose, California, USA
Contact:

Re: Roughing Vs Finishing toolpath

Post by Rcnewcomb »

is 5 hours and 13 minutes is reasonable time for 12X12 inch poplar material.
Compare that time with how long it would take you to carve it by hand with a set of chisels.
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

User avatar
rscrawford
Vectric Wizard
Posts: 976
Joined: Mon Jan 17, 2011 6:49 pm
Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408
Location: Wetaskiwin, Alberta
Contact:

Re: Roughing Vs Finishing toolpath

Post by rscrawford »

'Reasonable time' for 3D work totally depends on your machine.

I would never consider doing a roughing pass on something like that. I'd use a raster cut at 18000rpm and feed speed of 800XYZ. Probably 45 minutes on my machine (its the acceleration/decelleration settings that makes the biggest difference in cut times on something like this, not just your feed speeds)
Russell Crawford
http://www.cherryleaf-rustle.com

User avatar
Rcnewcomb
Vectric Wizard
Posts: 3802
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: GCnC/WinCNC
Location: San Jose, California, USA
Contact:

Re: Roughing Vs Finishing toolpath

Post by Rcnewcomb »

(its the acceleration/decelleration settings that makes the biggest difference in cut times on something like this, not just your feed speeds)
Russ,
I'd be interested in looking at you WINCNC.INI file for your setting.
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

User avatar
Xxray
Vectric Wizard
Posts: 2107
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Roughing Vs Finishing toolpath

Post by Xxray »

I thought about the no roughing angle, personally I think those with less experience should rough to get familiar with the entire process, then once they gain experience they can omit the step if they wish. I rarely use roughing myself except thick plexiglas and the hardest of woods with deep cuts. Now he knows thats an option, would advise .125 passes max and a good, sharp endmill when roughing.
Doug

User avatar
TReischl
Vectric Wizard
Posts: 3339
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Roughing Vs Finishing toolpath

Post by TReischl »

Maybe I think about finishing passes a little differently than some others?

Since very little material is being removed I push my machine as fast as it will go, or at least set the feedrates so it has the opportunity to do so. Acceleration is fast. A lot of folks look at a part like that and say, oh, well, it will never get over X IPM so there is no point in setting it any higher. That is a mistake. It doesn't take 3 inches of flat to get up to 250 IPM. A while back I did a spreadsheet to calc what accelerations do. The 25in/sec/sec used is actually very conservative.
Capture.JPG
The point here is that if the machine can go faster let it. Programming a low feed rate because you feel the machine will never reach that feed rate is a mistake that costs lots of time.
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
Xxray
Vectric Wizard
Posts: 2107
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Roughing Vs Finishing toolpath

Post by Xxray »

I missed it, did someone suggest programming a low feed rate ?
Doug

Post Reply