Need help with 3d toolpath

This forum is for general discussion about Aspire

Need help with 3d toolpath

Postby jmlewis74 » Sun Aug 06, 2017 6:24 pm

I have been having a lot of problems with 3d toolpaths lately and have been struggling to determine where the problem lies. I have been getting a lot of too marks on 3d paths but mostly on the end of the models. I do understand that there will be toolmarks but I am trying to figure out why I am getting gouges. Is it the tool setup, 3d setup or is the machine not responding fast enough to direction changes. Any help would be appreciated. I have included pics of the issue. Machine setup is a 3 axis, using mach3 and g540 with parallel cable connection.

Thanks

JML
Attachments
image1.JPG
image2.JPG
image3.JPG
bit settings.PNG
3d setting.PNG
jmlewis74
 
Posts: 7
Joined: Mon Jul 02, 2012 11:56 pm
Model of CNC Machine: Geometric Robotics 2x4 commercial kit

Re: Need help with 3d toolpath

Postby joeporter » Sun Aug 06, 2017 6:56 pm

What kind of router/spindle are you using? It looks to me like the cutter is being dragged across the material and is scratching more than cutting. Also, what kind of material is this? It looks like it is being compressed and then rebounding like something that is spongy. Very good photos by the way, so is hard to figure why a good router with a good cutter would leave these kinds of marks if all is working like you show for rpm and stepover, etc.....joe
joeporter
Vectric Wizard
 
Posts: 395
Joined: Tue Jul 21, 2009 8:22 pm
Location: Marietta, GA.
Model of CNC Machine: ShopBot Buddy Standard

Re: Need help with 3d toolpath

Postby jmlewis74 » Sun Aug 06, 2017 7:17 pm

Thanks for your reply. I'm using a Bosch 1617 router body. I don't remember it cutting like this previously, but it seems to be on every part now.
jmlewis74
 
Posts: 7
Joined: Mon Jul 02, 2012 11:56 pm
Model of CNC Machine: Geometric Robotics 2x4 commercial kit

Re: Need help with 3d toolpath

Postby ger21 » Sun Aug 06, 2017 8:15 pm

Probably a combination of your lookahead, acceleration, and CV settings.
Gerry
ger21
Vectric Wizard
 
Posts: 854
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: Need help with 3d toolpath

Postby jmlewis74 » Sun Aug 06, 2017 8:39 pm

ger21

My lookahead was still set at the default of 20 lines. What would be a reasonable value to change to to try out. Should I start there vs the acceleration and velocity settings?
jmlewis74
 
Posts: 7
Joined: Mon Jul 02, 2012 11:56 pm
Model of CNC Machine: Geometric Robotics 2x4 commercial kit

Re: Need help with 3d toolpath

Postby martin54 » Sun Aug 06, 2017 9:36 pm

You say you have been getting a lot of problems lately so is this something that you haven't seen in the past ? Are these parts that you have cut in the past without problem or are these parts you have never cut before ?
Have you tried cutting a file that previously cut well to see if you are getting this same problem now ?
Have you changed anything about your set up lately ?
User avatar
martin54
Vectric Wizard
 
Posts: 3277
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Need help with 3d toolpath

Postby jmlewis74 » Sun Aug 06, 2017 10:39 pm

I don't do a lot of 3d toolpaths. These are all new models. I can try one of the old projects and do a section. The only thing that I have changed lately was the max rate and velocity of my Z axis, but this was to help prevent toolmarks on future projects. The look ahead setting can not be the only issue since i changed and reran and am still having same results.
jmlewis74
 
Posts: 7
Joined: Mon Jul 02, 2012 11:56 pm
Model of CNC Machine: Geometric Robotics 2x4 commercial kit

Re: Need help with 3d toolpath

Postby Seachaser » Sun Aug 06, 2017 10:44 pm

Is this material HDU, or some type of foam? And what is the holdown method?
Seachaser
 
Posts: 8
Joined: Thu Nov 26, 2015 5:27 pm
Model of CNC Machine: Camaster

Re: Need help with 3d toolpath

Postby ger21 » Sun Aug 06, 2017 11:05 pm

jmlewis74 wrote:ger21

My lookahead was still set at the default of 20 lines. What would be a reasonable value to change to to try out. Should I start there vs the acceleration and velocity settings?


I would make sure the accel is as high as possible first.
Then, make sure CV feedrate and CV distance are turned off.
Then play with the lookahead last. I would set it to 100, and see if it's better, or worse.
Gerry
ger21
Vectric Wizard
 
Posts: 854
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: Need help with 3d toolpath

Postby jmlewis74 » Sun Aug 06, 2017 11:13 pm

Seachaser wrote:Is this material HDU, or some type of foam? And what is the holdown method?


The material was pine and the item was both glued down (tape crazy glue), but was also clamped down on all four corners. Over kill yes.
jmlewis74
 
Posts: 7
Joined: Mon Jul 02, 2012 11:56 pm
Model of CNC Machine: Geometric Robotics 2x4 commercial kit

Re: Need help with 3d toolpath

Postby jmlewis74 » Sun Aug 06, 2017 11:16 pm

ger21 wrote:
jmlewis74 wrote:ger21

My lookahead was still set at the default of 20 lines. What would be a reasonable value to change to to try out. Should I start there vs the acceleration and velocity settings?


I would make sure the accel is as high as possible first.
Then, make sure CV feedrate and CV distance are turned off.
Then play with the lookahead last. I would set it to 100, and see if it's better, or worse.


ger21,

I changed the look ahead to 200 lines and the results were worse. I will adjust the acceleration and other suggestion when I get a chance this week.

Thank you all for your suggestions. I will reply with results when I try different settings.

JML
jmlewis74
 
Posts: 7
Joined: Mon Jul 02, 2012 11:56 pm
Model of CNC Machine: Geometric Robotics 2x4 commercial kit

Re: Need help with 3d toolpath

Postby martin54 » Mon Aug 07, 2017 12:47 am

Have you checked the machine physically for signs of backlash/binding or any free movement on all 3 axis ? I would also check the router for free play both axial & lateral :lol: :lol:
How old is the router because I have read somewhere that CNC work can be a killer for router bearings, never used a router personally because the bearings in the porter cable router fitted to my machine were shot when I got the machine & I replaced the router with a Chinese spindle & VFD :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3277
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Need help with 3d toolpath

Postby ger21 » Mon Aug 07, 2017 1:05 am

I thought the results would be worse with a higher lookahead.
I would try 10, but at some point it might get jerky. Another thing to try is the CV angle settings

What are your acceleration settings? If you are limited in your accel, then their may not be a lot you can do, other than cutting slower. You're running into a limitation of Mach3, which is it's less than stellar trajectory planner.
Gerry
ger21
Vectric Wizard
 
Posts: 854
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: Need help with 3d toolpath

Postby phill05 » Mon Aug 07, 2017 9:34 am

JML,

I have seen a problem like this before, a couple of things you might look at your stepover and clearance pass stepover try using same 5% for both, and create an offset vector around your model say 1/8" when you make the toolpath use selected Vector and 0 offset, be interesting if it works for you too.

Phill
phill05
Vectric Apprentice
 
Posts: 75
Joined: Thu Oct 14, 2010 2:40 pm
Location: Derbyshire UK
Model of CNC Machine: Hybrid re-build

Re: Need help with 3d toolpath

Postby TReischl » Mon Aug 07, 2017 1:47 pm

Forget the material.
Forget the feedrate.
Forget the stepover.

I had this same problem quite a few years ago. Fooled around with CV settings until I was blue in the face. Waste of time.

Finally, I quit looking at the cutter and looked at the stepper motor while it was cutting. The stepper motor was turning ever so slightly every time the Z axis changed direction. Imagine that! The four bolts holding it down had loosened up and allowed the motor to turn a little bit. That was an easy fix.

A few months later, the problem came back. But the motor was nice and tight. This time it was the coupler between the motor and the screw. Its little set screw had backed off a tad and was allowing some backlash. The screw would stop at one side or the other of the flat on the output shaft. Fixed that too.

Oh no, here we go again! This time it was the nut on the Z axis screw. It was worn out and allowing backlash.

I think that makes me a veritable expert on this problem, well maybe not, it is quite possible that someday the router itself will get loose in the mount!

Here is the deal. What you are seeing is the failure of the Z axis to lift the tool to the proper height. It is not the Z axis driving the tool too deep. Remember, gravity is helping when the tool is moving down, it is working against motion when the tool is going up.

The real tipoff to what the problem is indicated by some of those very faint lines that slowly disappear as the tool moves away from the edge and Z is moving slowly as the height changes are less severe.

That is my 2 cents worth. If you cannot find anything in the drive train then it is time to mess with the CV settings as Gerry has suggested. There is no point in playing with CV until you are dead certain that you have no play in the Z axis. First things first. My rule for trouble shooting is to always do the mechanical stuff FIRST, before playing with software. It is easier to find mechanical issues than sit around trying to find some magical software setting to cure the ills.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 1966
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Next

Return to Aspire - General

Who is online

Users browsing this forum: Gundawg and 17 guests