CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
August 20, 2019, 20:42:15 pm


Login with username, password and session length


Pages: [1]
  Print  
Author Topic: Choppy motion when doing 3D profile  (Read 585 times)
shorton
Storm Trooper
***
Offline Offline

Posts: 119


View Profile
« on: May 20, 2019, 01:21:25 am »

I was adjusting stepover, & resolution to make a final smoothing pass on my part.  Working to get rid of the scalloping I had with my first settings.  The changes worked in that regard, but the motion on my 3D passes were very rough/choppy.  I took a slow motion video with my iPhone to see what was up.  On a horizontal cut, all was well, but when the bit was going up the inner side of my "bowl" the best way I could describe it is that it was making a small move, pausing and making the next move pausing and so on.  Not moving very fluidly.  I tried up upload the slo-mo video somewhere so I could show, but that in itself was problematic thus the verbal description.  FWIW, Mach3 didn't seem to be pausing and was zipping away with the gcode.

I don't know if it's something I've caused with my setup, a machine limitation, mach3 issue, or what.

Grateful for any pointers.

This happens with the 3DSurface5 or 6 MOPS in the attached file.


* CarleyBowlTest4.zip (164.91 KB - downloaded 33 times.)
« Last Edit: May 20, 2019, 01:36:21 am by shorton » Logged
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1250


View Profile
« Reply #1 on: May 20, 2019, 17:36:43 pm »

In Mach 3 you need to turn off exact stop. 3d cutting is thousands of tiny straight lines approximating the curves. You want to allow Mach 3 to keeping moving from line to line.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3633


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #2 on: May 20, 2019, 18:59:44 pm »

In Mach 3 you need to turn off exact stop. 3d cutting is thousands of tiny straight lines approximating the curves. You want to allow Mach 3 to keeping moving from line to line.

Exactly right except that you need to set the MOP to constant velocity as well.  The Mop will send a GCODE to Mach 3 to change the mode. 

If you find your self defaulting to Constant Velocity you may want to play with the CV limitations in Mach configuration as well, so you don't wind up with circular squares. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
shorton
Storm Trooper
***
Offline Offline

Posts: 119


View Profile
« Reply #3 on: May 20, 2019, 22:06:31 pm »

Thanks guys.  Bob, the problem MOP in the file I attached has velocity mode = CV already.

I'll see if I can turn i toff in Mach3, too.  Although if I understand Bob right, the CV setting in Cambam should be doing it already, right?    Undecided


 

Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5558



View Profile WWW
« Reply #4 on: May 20, 2019, 22:24:08 pm »

Hello

Quote
Although if I understand Bob right, the CV setting in Cambam should be doing it already, right?

Yep, it does.

To be sure, when you're machining, have a look on the Mach3 screen (Program Run) ; there is a LED that show if CV is on.

On my first old machine, I get the same behavior because acceleration was too small compared to the feedrate used for the mop. I see that you're using 150 Inch/min, maybe it's too fast for your acceleration value ?

Also have a look on the "lookAhead" value in the general settings, sometimes increasing the value can solve the problem.

++
David
Logged
shorton
Storm Trooper
***
Offline Offline

Posts: 119


View Profile
« Reply #5 on: May 21, 2019, 00:11:09 am »

Thanks, I'll check those, too.  My machine rapids are set at 200, although it may do 300 w/o stalling in X/Y.  Z slower because it has to lift the Z axis assembly, don't remember it's limits.  I think I've got X-Y Accel. set at 40, but it's been a long time, will have to check.  Will report back on details.

FWIW, I don't think I saw this behavior until I turned down the resolution.  I guess in a linear path the stepover isn't a factor.  I didn't see the choppy behavior in the less granular paths, but it may have been there and just not as noticeable, will double check that, too.

Logged
shorton
Storm Trooper
***
Offline Offline

Posts: 119


View Profile
« Reply #6 on: May 21, 2019, 03:14:35 am »

I checked all the CV settings in Mach3, most were unchecked.  CV was set in gcode by CB, checked, and it was registered/set in Mach3 too.  Fiddled with my accel settings, I had 30ips2 on Z and 40 on X-Y.

Reran the code in air and videoed again, I didn't see the same stop motion I saw the other day when cutting.  Maybe I was at a motor harmonic, or the motors were behaving different when hot.  Anyway, it took slo-mo filming to see ti anyway, so maybe I'm not that bad off.  I saw some others examples I could see much worse problems wiht this issue once I had an idea what to look for.

Thanks as always for the help.  Much appreciated.
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5558



View Profile WWW
« Reply #7 on: May 21, 2019, 03:53:42 am »

Quote
Maybe I was at a motor harmonic, or the motors were behaving different when hot.

Yep ... or a driver that starts to die .. ?

Are you using the // port ?

With // port and a big 3D Gcode I also encounter strange stops (but no steps lose) until I disable the toolpath display in Mach3 (I had an integrated VGA card on a small P4 2.8Ghz PC) ; This happens only one time, and the Gcode was something like 500K lines ...

++
David
Logged
shorton
Storm Trooper
***
Offline Offline

Posts: 119


View Profile
« Reply #8 on: May 21, 2019, 13:37:45 pm »

No, I'm using a UNC100 (I think) USB driver.  That goes to a parallel port in a Geko drive.
Logged
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1250


View Profile
« Reply #9 on: May 21, 2019, 15:18:03 pm »

Turning off toolpath display may help no matter what interface is used. Worth trying.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3633


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #10 on: May 21, 2019, 19:58:26 pm »

Turning off toolpath display may help no matter what interface is used. Worth trying.

Definitely helps on larger jobs.  I put a tool path display button on my home page on all my Mach controlled machines. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
shorton
Storm Trooper
***
Offline Offline

Posts: 119


View Profile
« Reply #11 on: May 23, 2019, 22:24:59 pm »

Turning off toolpath display may help no matter what interface is used. Worth trying.
Thanks.  I'm using a custom screen/skin for Mach3, I'll have to see if I can find where to turn it off. (2010 Screenset I think it's called).
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5558



View Profile WWW
« Reply #12 on: May 23, 2019, 23:26:38 pm »

Hello,

I don't know for the screenset 2010, but on the regular Mach3 screen it's on the Diagnostic panel, just bellow the GCode display > button ToolPath On/Off

If you want to add it to your screen (With MachScreen) ; it's the OEM button 132

++
David
Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3993



View Profile
« Reply #13 on: May 24, 2019, 12:28:51 pm »

Thanks.  I'm using a custom screen/skin for Mach3, I'll have to see if I can find where to turn it off. (2010 Screenset I think it's called).


This is the one, circled in red.

From the manual, "Toolpath On/Off (On State), Toggles toolpath display on/off."


* mach3.jpg (60.36 KB, 1000x515 - viewed 37 times.)
Logged

Made in England
Pages: [1]
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.21 | SMF © 2015, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.161 seconds with 20 queries.

Copyright © 2018 HexRay Ltd. | Sitemap