Hello Guest it is December 15, 2019, 12:44:46 PM

Author Topic: Unexpected Crop Circles  (Read 6531 times)

0 Members and 1 Guest are viewing this topic.

Offline PaulWC

*
  •  125 125
    • View Profile
Re: Unexpected Crop Circles
« Reply #10 on: May 19, 2013, 01:37:53 PM »
Did not see crop circles or any other anomalies in toolpath view. Code ran fine in CutViewer Mill simulator. Problem showed with two different code sources.

I've attached the code I was running when I was there to see it happen (client's machine). Wide circle occurred at line 5788, a G3 line of code... far past the first G3 in the program. For what I observed, it appeared the math logic randomly lost it's place.

The attached file has the G90.1 line added, but was not there during the run.

Offline ger21

*
  • *
  •  6,291 6,291
    • View Profile
    • The CNC Woodworker
Re: Unexpected Crop Circles
« Reply #11 on: May 19, 2013, 02:44:03 PM »
Quote
The attached file has the G90.1 line added, but was not there during the run.

It should be G91.1

It won't run with G90.1. I get an error when I load it into mach3. Change it to G91.1 and it's fine.
Gerry

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

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

Offline PaulWC

*
  •  125 125
    • View Profile
Re: Unexpected Crop Circles
« Reply #12 on: May 19, 2013, 03:13:50 PM »
I have to admit... I'm confused by the use of absolute distance combined with incremental IJ?

On line 5788 the XY coordinates are absolute, which goes along with the G90 placed in the header by MeshCAM.

In addition to changing the G90.1 to G91.1, should General Config also be changed to Incremental IJ?

I could use some clarification instruction. Just do it because it works is not a real confidence builder.  ;)

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Unexpected Crop Circles
« Reply #13 on: May 19, 2013, 04:11:18 PM »
Is that the code that you are showing a pic of in the first post?
Hood

Offline PaulWC

*
  •  125 125
    • View Profile
Re: Unexpected Crop Circles
« Reply #14 on: May 19, 2013, 04:41:27 PM »
No... The pic was sent to me by the client after running the attached code. The previous attached code was the one I ran at his site and witnessed the behavior.

Offline ger21

*
  • *
  •  6,291 6,291
    • View Profile
    • The CNC Woodworker
Re: Unexpected Crop Circles
« Reply #15 on: May 19, 2013, 05:13:45 PM »
I have to admit... I'm confused by the use of absolute distance combined with incremental IJ?

That's what 99% of CAM programs output.

Quote

In addition to changing the G90.1 to G91.1, should General Config also be changed to Incremental IJ?


IJ mode is modal. If your g-code has a G91.1 in it, it is changing it in General Config, and it should remain Incremental until you change it, or run code with a G90.1 in it, which will change it back to Absolute IJ.

It's good practice to have your CAM software add the G90.1 or G91.1 to your g-code, which will automatically set Mach3 to the correct IJ mode for that particular code. In almost all cases, this would be G91.1.
Gerry

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

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

Offline PaulWC

*
  •  125 125
    • View Profile
Re: Unexpected Crop Circles
« Reply #16 on: May 19, 2013, 07:48:36 PM »
Well... I started this topic saying I had Mental cobwebs to clear out!  :o

Thanks to all for the assistance.

Paul

Offline PaulWC

*
  •  125 125
    • View Profile
Re: Unexpected Crop Circles
« Reply #17 on: May 19, 2013, 09:41:00 PM »


IJ mode is modal. If your g-code has a G91.1 in it, it is changing it in General Config, and it should remain Incremental until you change it, or run code with a G90.1 in it, which will change it back to Absolute IJ.

It's good practice to have your CAM software add the G90.1 or G91.1 to your g-code, which will automatically set Mach3 to the correct IJ mode for that particular code. In almost all cases, this would be G91.1.
[/quote]

I looked at General Config after loading my code with added G91.1, and the Absolute IJ button is still selected?

I modified my MeshCAM Mach3 Post Processor to include the G91.1. And I emailed a note to the MeshCAM author asking for his input on the issue. I'm guessing a large percentage of his customers are running Mach3 systems.

Paul

Offline ger21

*
  • *
  •  6,291 6,291
    • View Profile
    • The CNC Woodworker
Re: Unexpected Crop Circles
« Reply #18 on: May 19, 2013, 10:23:23 PM »
Quote
I looked at General Config after loading my code with added G91.1, and the Absolute IJ button is still selected?

Run the g-code, then look at it. It will be changed.
 However, it doesn't appear to be modal between sessions, so you should probably change it in General Config, in case your g-code doesn't specify the mode.

I've been using MeshCAM since the very first beta version. I normally don't use arc fitting, but I have my post modified as well.
Gerry

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

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

Offline PaulWC

*
  •  125 125
    • View Profile
Re: Unexpected Crop Circles
« Reply #19 on: May 20, 2013, 02:32:13 AM »
And... Presto! There it is!  ::)

Once again, assuming brought unwanted results. I assumed the pre-scan of the code would trigger the change.

Oh well... cycled dry with machine off. No harm, no foul, nothing to break... all good.

I'm not a Beta user of MeshCAM, but Robert called me personally to thank me for my license purchase. Sadly, the five years I spent away from my shop while machining for a paycheck, along with four strokes, put a dent in the 64+ year old gray cells.  :(

Thanks, Paul