Hello Guest it is November 19, 2019, 12:58:48 PM

Author Topic: Hesitates with tabs in profile toolpath  (Read 3920 times)

0 Members and 1 Guest are viewing this topic.

Offline P_D_B

*
  •  35 35
    • View Profile
Hesitates with tabs in profile toolpath
« on: December 04, 2013, 10:41:20 PM »
I think I know the answer to this but I just want to make sure first.  I have the current Mach3 release.  I use Aspire for CAM.  I output toolpaths with the Mach2_3_ATC_Arcs_inch.pp.  Whenever I select add tabs to toolpath it adds extra points on each pass depth cut instead of the one that needs it.  This causes a jerking that is not noticeable until you get over 125 ipm.  Examples next and question below.

Example code with tabs
N190X0.0000Y0.0000F100.0
N200G00X1.4486Y5.7766Z2.7500
N210G00X1.4486Y5.7766Z1.0000
N220G1X1.4486Y5.7766Z0.3750F20.0
N230G1X1.2878Y6.0577Z0.3750F100.0
N240G1X1.2111Y6.2003Z0.3750
N250G1X1.1344Y6.3430Z0.3750
N260G1X0.9887Y6.6322Z0.3750
N270G2X-0.2500Y12.0000I11.0113J5.3678
N280G2X12.0000Y24.2500I12.2500J0.0000
N290G2X20.6786Y20.6454I0.0000J-12.2500
N300G1X20.9065Y20.4105Z0.3750
N310G1X21.0172Y20.2901Z0.3750
N320G1X21.1280Y20.1696Z0.3750
N330G1X21.3429Y19.9229Z0.3750
N340G2X24.2500Y12.0000I-9.3429J-7.9229
N350G2X12.0000Y-0.2500I-12.2500J0.0000
N360G2X1.4486Y5.7766I0.0000J12.2500
N370G1X1.4486Y5.7766Z0.0000F20.0
N380G1X1.2878Y6.0577Z0.0667F100.0
N390G1X1.2111Y6.2003Z0.1000
N400G1X1.1344Y6.3430Z0.0667
N410G1X0.9887Y6.6322Z0.0000
N420G2X-0.2500Y12.0000I11.0113J5.3678
N430G2X12.0000Y24.2500I12.2500J0.0000
N440G2X20.6786Y20.6454I0.0000J-12.2500
N450G1X20.9065Y20.4105Z0.0667
N460G1X21.0172Y20.2901Z0.1000
N470G1X21.1280Y20.1696Z0.0667
N480G1X21.3429Y19.9229Z0.0000
N490G2X24.2500Y12.0000I-9.3429J-7.9229
N500G2X12.0000Y-0.2500I-12.2500J0.0000
N510G2X1.4486Y5.7766I0.0000J12.2500
N520G00X1.4486Y5.7766Z2.7500

Example code with without tabs
N190X0.0000Y0.0000F100.0
N200G00X12.0000Y-0.2500Z2.7500
N210G00X12.0000Y-0.2500Z1.0000
N220G1X12.0000Y-0.2500Z0.3750F20.0
N230G2X-0.2500Y12.0000I0.0000J12.2500F100.0
N240G2X12.0000Y24.2500I12.2500J0.0000
N250G2X24.2500Y12.0000I0.0000J-12.2500
N260G2X12.0000Y-0.2500I-12.2500J0.0000
N270G1X12.0000Y-0.2500Z0.0000F20.0
N280G2X-0.2500Y12.0000I0.0000J12.2500F100.0
N290G2X12.0000Y24.2500I12.2500J0.0000
N300G2X24.2500Y12.0000I0.0000J-12.2500
N310G2X12.0000Y-0.2500I-12.2500J0.0000
N320G00X12.0000Y-0.2500Z2.7500

First off, should it react this way with the hesitation? I thought it read the next point so it would be able to maintain constant velocity?  If this is normal operation, is there a way to minimize it or do I just have edit the gcode?  I don't understand why they have them on every pass depth that does not require a movement in the Z axis. 
------------------------------------------------------------
Remember Einstein said this...."We can't solve problems by using the same kind of thinking we used when we created them."
__________________________________

Pete

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Hesitates with tabs in profile toolpath
« Reply #1 on: December 04, 2013, 11:09:00 PM »
Make sure CV distance and CV feedrate are off, and increase the lookahead if it's set at 20. Not sure if these will help or not. I've seen others ask this before.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline P_D_B

*
  •  35 35
    • View Profile
Re: Hesitates with tabs in profile toolpath
« Reply #2 on: December 05, 2013, 05:07:43 PM »
It had already tried turning off the CV controls and my look ahead lines are at 200.
------------------------------------------------------------
Remember Einstein said this...."We can't solve problems by using the same kind of thinking we used when we created them."
__________________________________

Pete

Offline P_D_B

*
  •  35 35
    • View Profile
Re: Hesitates with tabs in profile toolpath
« Reply #3 on: December 05, 2013, 07:05:34 PM »
Ok, on the settings page I have checked that CV feedrate is off.  I have tried with both the CV controls on and off in the general config page.  It is occurring when Z ramps back down to Zero or directly after, like the 4th & 5th lines below
4th & 5th lines  here
N300G1X20.9065Y20.4105Z0.3750
N310G1X21.0172Y20.2901Z0.3750
N320G1X21.1280Y20.1696Z0.3750
N330G1X21.3429Y19.9229Z0.3750
N340G2X24.2500Y12.0000I-9.3429J-7.9229
4th & 5th lines  here
N450G1X20.9065Y20.4105Z0.0667
N460G1X21.0172Y20.2901Z0.1000
N470G1X21.1280Y20.1696Z0.0667
N480G1X21.3429Y19.9229Z0.0000
N490G2X24.2500Y12.0000I-9.3429J-7.9229
------------------------------------------------------------
Remember Einstein said this...."We can't solve problems by using the same kind of thinking we used when we created them."
__________________________________

Pete

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Hesitates with tabs in profile toolpath
« Reply #4 on: December 05, 2013, 07:11:53 PM »
What do you have Stop CV on angles< set to?
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline P_D_B

*
  •  35 35
    • View Profile
Re: Hesitates with tabs in profile toolpath
« Reply #5 on: December 05, 2013, 08:14:06 PM »
Stop CV on angles is 65.  Does not matter if it is enabled or not.  Same reaction. 

I think it is the transition between the G1 and G2.  Feed Rate Override does exacerbate it.  But I have been trying to find info you on the forum.  I have not seen any problems like a lot of the other threads.  I have only had problems with tabs on profile cuts.  My velocity is 500 and accel is 25.  I may play with the accel some more
 
------------------------------------------------------------
Remember Einstein said this...."We can't solve problems by using the same kind of thinking we used when we created them."
__________________________________

Pete

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Hesitates with tabs in profile toolpath
« Reply #6 on: December 05, 2013, 08:40:42 PM »
I happen to be a beta tester for Aspire. A few years ago, one of the other testers knew of several people experiencing what you are. Several other Mach3 users did not experience the problem, and claimed the issue was caused by CV settings. I just went back and read through the messages, and no specific settings were mentioned to eliminate the problem, and the original poster never followed up with any resolution.

So, unfortunately, I don't have any answer on how to eliminate it. I never use tabs, so haven't come across this issue.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline P_D_B

*
  •  35 35
    • View Profile
Re: Hesitates with tabs in profile toolpath
« Reply #7 on: December 05, 2013, 09:17:13 PM »
Gerry,
Unfortunately I have no other cam software to compare it against.  I can increase my accel to 90 before missing steps with the same velocity setting.  I saw many posts with people saying about troubles with v-carving and this problem.  I don't seem to be experiencing that, well at least I never noticed it. No problems with 3D work either.  I have noticed it with all profiles that have a tab though.  All my tabs I try to place them on straight lines.  The closest thing I have seen for an explanation for this is here from reply 30 through 33  http://www.machsupport.com/forum/index.php/topic,1724.msg11211.html#msg11211
I will generate code for a plain rectangle with a profile and a profile with tabs.  I will post back what I find.
------------------------------------------------------------
Remember Einstein said this...."We can't solve problems by using the same kind of thinking we used when we created them."
__________________________________

Pete

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Hesitates with tabs in profile toolpath
« Reply #8 on: December 05, 2013, 09:30:31 PM »
In your first post, you asked about why the tabs were present on every pass. The answer to that, is that it's just how the algorithm that Vectric uses works. It's apparently something that they can't easily change, so it's been that way through probably every version of Aspire and V Carve Pro. It's Vectric's opinion that this shouldn't be an issue, and I tend to agree.

I read through the posts you linked to above. I think that the issue here is a possible bug (or limitation) in Mach3's trajectory planner. I've run into similar situations where Mach3 would  "hesitate" at a transition from a straight line to a tangent arc. Technically, it shouldn't, but I've seen it happen.
Which means that there probably isn't a fix to your problem. Unless you can find some magical combination of CV settings that helps.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline P_D_B

*
  •  35 35
    • View Profile
Re: Hesitates with tabs in profile toolpath
« Reply #9 on: December 05, 2013, 09:45:44 PM »
Gerry,
I would agree with you. I generated two toolpaths for a rectangle.  One profile path with 2 pass depths without tabs and one with 4 tabs.  Both ran flawless.  You are correct.  I was looking back through the problem tabs programs and they were always on an arc.  I misspoke (sorry mistyped) before, I started noticing it when I was cutting 3D puzzles to put together.  These always had tabs on the arcs.  The larger circle that the sample code above was for a lid.  It too was on an arc.  I can live with it but it is rather annoying.  Maybe Mach4 will have a solution for it.  Thank you for your time and answers with this.   It is greatly appreciated and does not go unnoticed.
------------------------------------------------------------
Remember Einstein said this...."We can't solve problems by using the same kind of thinking we used when we created them."
__________________________________

Pete