Official Luthiers Forum!

Solely owned and operated by Lance Kragenbrink
It is currently Mon Dec 18, 2017 4:05 am


All times are UTC - 5 hours





Post new topic Reply to topic  [ 9 posts ] 
Author Message
PostPosted: Thu Feb 04, 2016 5:42 pm 
Offline
Mahogany
Mahogany
User avatar

Joined: Fri Dec 13, 2013 4:51 pm
Posts: 43
Location: Peterborough, Ontario, Canada
First name: Alexander
Country: Canada
Focus: Build
Status: Professional
Hey everyone.

I have some toolpaths where I cut out a guitar neck. While doing any straight cuts, my CNC router runs great. When I get into doing the heel or volute carve on the guitar neck, the CNC is going through A LOT of little code to make the moves and it can start to shudder / jitter pretty bad. It shakes the whole CNC.

I am running those paths at 50 IPM but Mach 3 only says it makes it to 10-15 IPM for all those lines.

I don't know anything about CV mode but could it be that? Or would it be my post processor for Mastercam X4?


Any help would be greatly appreciated.
Thanks.


Top
 Profile  
 
PostPosted: Thu Feb 04, 2016 5:45 pm 
Offline
Cocobolo
Cocobolo

Joined: Wed Jan 08, 2014 7:58 pm
Posts: 147
First name: Leo
Last Name: Pedersen
City: Bowen Island
State: British Columbia
Zip/Postal Code: V0N 1G2
Country: Canada
Focus: Build
Status: Amateur
I'm still learning about CV issues but if my understanding is correct you should make sure that Mach3 is not in Exact Stop mode.


Sent from my iPhone using Tapatalk


Top
 Profile  
 
PostPosted: Thu Feb 04, 2016 6:15 pm 
Offline
Mahogany
Mahogany
User avatar

Joined: Fri Dec 13, 2013 4:51 pm
Posts: 43
Location: Peterborough, Ontario, Canada
First name: Alexander
Country: Canada
Focus: Build
Status: Professional
Durero wrote:
I'm still learning about CV issues but if my understanding is correct you should make sure that Mach3 is not in Exact Stop mode.


I will check and see if it is. Thanks.


Top
 Profile  
 
PostPosted: Fri Feb 05, 2016 3:23 pm 
Offline
Cocobolo
Cocobolo

Joined: Fri Dec 01, 2006 6:44 pm
Posts: 437
Location: Australia
First name: Allen
Last Name: McFarlen
City: Mt. Sheridan
State: Qld.
Zip/Postal Code: 4868
Country: Australia
Focus: Build
Status: Professional
I had some jittery moves on some curves a couple of weeks ago. Using Fusion360 and the Mach3 post processor.

It turned out that the code being generated had lots of little moves in some of the tighter curves. So what fixed it was to turn on smoothing for the tool path and altering the resolution. It also reduced the files size from 87kb down to 15kb. A really significant number of lines to do the same thing, but better.

Idon't know if those options are available in your software, but certainly worth a look.

_________________
Allen R. McFarlen
Barron River Guitars & Ukuleles
Facebook
Cairns, Australia


Top
 Profile  
 
PostPosted: Sat Feb 06, 2016 3:20 pm 
Offline
Contributing Member
Contributing Member
User avatar

Joined: Thu Jun 12, 2008 6:59 am
Posts: 1904
Location: Rochester Michigan
The problem is your CV settings. Oh, and by the way, Mach 3 has a terrible CV trajectory planner. I'm no longer using Mach 3 so I don't remember the exact settings but you need to play with your lookahead and tolerance settings but keep in mind, as far as I know, there's no way to know exactly what your maximum error will be and through experience, I know that Mach 3 is quite inconsistent when it comes to CV tolerance.

Keep in mind though that as you tune your machine to be faster, the parts will get less precise.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com


Top
 Profile  
 
PostPosted: Fri Feb 12, 2016 6:53 pm 
Offline
Mahogany
Mahogany
User avatar

Joined: Fri Dec 13, 2013 4:51 pm
Posts: 43
Location: Peterborough, Ontario, Canada
First name: Alexander
Country: Canada
Focus: Build
Status: Professional
Hey guys.

It turned out that my cam post processor was writing the gcode to turn off CV mode. That was making my toolpaths run in exact stop mode and create a very jerky motion.


Top
 Profile  
 
PostPosted: Sat Feb 13, 2016 10:52 am 
Offline
Contributing Member
Contributing Member

Joined: Mon Dec 27, 2004 11:25 pm
Posts: 7173
Location: United States
Andy, what are you using instead of Mach3 now?

_________________
"I want to know what kind of pickups Vince Gill uses in his Tele, because if I had those, as good of a player as I am, I'm sure I could make it sound like that.
Only badly."


Top
 Profile  
 
PostPosted: Sun Feb 14, 2016 4:56 pm 
Offline
Contributing Member
Contributing Member
User avatar

Joined: Thu Jun 12, 2008 6:59 am
Posts: 1904
Location: Rochester Michigan
I'm using UCCNC/UC100 combo. The ups are that the trajectory planner is far superior to Mach 3. I'm able to double my accels because it doesn't violate accel settings like Mach 3 does. Machine runs far smoother and much more predictably than Mach3. The CV planner is also adjustable for tolerance.

The down side is that it's still not fully featured. It doesn't support G18 or 19 and even worse that it will just do a G17 move when it comes across a G2 or G3 move. There's a few other goofy things about it but at the moment, I prefer it over Mach 3 because the TP is so much better.

I have a part I'll be making with a 4th axis and I'll have to revert to Mach 3 for that because UCCNC doesn't support a 4th axis as a rotary axis so it's very difficult to get it to move fast enough.

I have another machine that I'm setting up with Kflop right now and intend on using KmotionCNC. This has been taking me forever to get going unfortunately. If Kmotion does what everyone says it does, I'll probably switch my first machine over to it as well.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com


Top
 Profile  
 
PostPosted: Sun Oct 23, 2016 7:17 pm 
Offline
Cocobolo
Cocobolo

Joined: Tue Mar 04, 2008 10:55 pm
Posts: 404
Location: Dallas, Texas
Andy Birko wrote:
The problem is your CV settings. Oh, and by the way, Mach 3 has a terrible CV trajectory planner. I'm no longer using Mach 3 so I don't remember the exact settings but you need to play with your lookahead and tolerance settings but keep in mind, as far as I know, there's no way to know exactly what your maximum error will be and through experience, I know that Mach 3 is quite inconsistent when it comes to CV tolerance.

Keep in mind though that as you tune your machine to be faster, the parts will get less precise.


I agree with Andy on this. What I have done in mach3 when faced with this type of code is to set it for plasma mode. That being said any SQUARE corners will have some rounding as Plasma mode keeps the cutter moving so as not to have plasma heat stop at any point as Mach thinks it is a plasma cutter, when in reality it is a mill/router . This also works well with 2.5D or 3d work that is jerking. IN those though you would want to up your Z feed rate since all axis are being used in that instance so you get a consistent flow for the machine.
Just my observation using MACH3 for 10years.
MK

_________________
I'm outside looking in, just farther from the window than most.


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 9 posts ] 

All times are UTC - 5 hours


Who is online

Users browsing this forum: No registered users and 1 guest


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Jump to:  
cron
Powered by phpBB® Forum Software © phpBB Group
phpBB customization services by 2by2host.com