Hello Guest it is October 18, 2019, 06:02:47 AM

Author Topic: Loading one Gcode file after Another Problem's  (Read 5748 times)

0 Members and 1 Guest are viewing this topic.

Offline Chip

*
  • *
  •  2,056 2,056
  • Gainesville Florida USA
    • View Profile
Loading one Gcode file after Another Problem's
« on: November 11, 2006, 10:45:57 AM »
Hi, ALL

After running this code, Any Gcode file I load with a G02,G03 I get this error, "Radius to end of arc differs from radius to start on Line number #**"  (** is line # of first G02,G03), on Status window and Lasterror's File.

(Tooth2.txt)
G90 G80 G40 G91.1; same thing with or without this code
m98 p11 l11; Setting's, A set to 0.5
m30

o11;-----------------------------one deg. step
g91
g01 x.5 y-.0 z-.5 a32.727272 f100; A axis 11 equal spaces 360 turn
g00 x-.5 y.0 z.5 a-32.727272
g00 a32.727272
m99
%

A re-start seem's to resolve this until this Gcode is Run again. Am I missing a Gcode cancel or is it a Bug ?

Any help would be Appreciated.

Thank's Chip
« Last Edit: November 11, 2006, 05:57:59 PM by afn09556 »

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Loading one Gcode file after Another Problem's
« Reply #1 on: November 11, 2006, 12:54:13 PM »
Incorrect I,J Mode.?
« Last Edit: November 11, 2006, 06:33:40 PM by afn09556 »
Gerry

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

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

Offline Graham Waterworth

*
  • *
  •  1,889 1,889
  • Yorkshire Dales, England
    • View Profile
Re: Loading one Gcode file after Another Problem's
« Reply #2 on: November 11, 2006, 01:43:21 PM »
Hi Chip,

The code looks ok apart from :-

I would remove the G91.1 (G92.1 maybe?), re-run Mach and then try your g02/03

The only other thing I can think of is it may be a good idea to put a G90 on a line before your M30 just in case the other programs don't have it in the start up.

Graham.
« Last Edit: November 11, 2006, 06:34:06 PM by afn09556 »
Without engineers the world stops

Offline Chip

*
  • *
  •  2,056 2,056
  • Gainesville Florida USA
    • View Profile
Re:Loading one Gcode file after Another Problem's
« Reply #3 on: November 11, 2006, 03:20:12 PM »
Hi, Gerry and Graham

It appears that the Gcode interpreter Mach3R2.0.009, isn't reading the G90 G80 G40 G91.1 when I load the Gcode File below, after running Tooht2.txt.

It doesn't change Mach3 back to Distance Mode, ABS -  G90, If I start Mach3 with the below file, It works fine.

It has the, G90 G80 G40 G91.1 in it as generated by LazyCom

It should read each file and set the propper Modes each time just like from a fresh startup.   

Thank's for the Input, Chip
« Last Edit: November 11, 2006, 06:34:25 PM by afn09556 »

Offline Graham Waterworth

*
  • *
  •  1,889 1,889
  • Yorkshire Dales, England
    • View Profile
Re: Loading one Gcode file after Another Problem's
« Reply #4 on: November 12, 2006, 03:32:27 AM »
G91.1

I don't know that one and I can't find any reference to it in the manual.

What is it?

This is what google found :-

FAR Part 91 Sec. G91.1 effective as of 09/30/1963
Federal Aviation Regulation. Hide details for Sec. G91.1 Sec. G91.1 ... G91.1 Section 1.   ;D ;)

Graham.
« Last Edit: November 12, 2006, 03:37:47 AM by Graham Waterworth »
Without engineers the world stops

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Loading one Gcode file after Another Problem's
« Reply #5 on: November 12, 2006, 07:22:38 AM »
G90.1 - set IJ mode to absolute
G91.1 - set IJ mode to incremental

It's in the manual I'm looking at.
Gerry

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

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Loading one Gcode file after Another Problem's
« Reply #6 on: November 12, 2006, 06:48:44 PM »
Also try putting the G90 on a single line and I think you will be happy ;)
Fixing problems one post at a time ;)

www.newfangledsolutions.com
www.machsupport.com

Offline Chip

*
  • *
  •  2,056 2,056
  • Gainesville Florida USA
    • View Profile
Re: Loading one Gcode file after Another Problem's
« Reply #7 on: November 12, 2006, 10:46:56 PM »
Hi, Brian

I figured it out earlier today added some LED's on Diag. page and made some changes to LazyCam's, Post Gcode option's page, been chasing my tail, pounding 16 penny. nail's in a wall (with my head), Posting answers to question's, where I can, Just a Mach sick-o-hear.
Learned allot over the past year (time flies when your have-n fun), our IR water jet cutter conversion working  nice, several other machine's. in the work's.

The Gcode (test55Dotpolyline58.txt) was generated by LazyCam, The problem is that, LC Posting Options, PreAmble, PostAmble ( Release 2.66) are setup incorrectly or Mach3 can't read and process multi-Gcode command's on one line yet.

In 2.66 the setup was as fallows.

Pre.
G90 G80 G40
Post.
G40 G80 M30

I Changed them to.

Pre.
G90
G80
G40

Post.
G40
G80
G90
M30

All is well now, Gust a Bug, you pick it, LazyCam, Mach3 or Both.
OK some operator error hear also.

Thank's Chip



Re: Loading one Gcode file after Another Problem's
« Reply #8 on: November 12, 2006, 11:00:03 PM »
Good to see that you got it to work and I have talked to Art about it :)
Fixing problems one post at a time ;)

www.newfangledsolutions.com
www.machsupport.com

Offline Chip

*
  • *
  •  2,056 2,056
  • Gainesville Florida USA
    • View Profile
Re: Loading one Gcode file after Another Problem's
« Reply #9 on: November 14, 2006, 09:16:15 PM »
Hi Brian

I have done some futher checking it appears that the G90 with G91.1 or G90 with G90.1, in the same line is what is causing the ABS Mode not to reset / change.

Use my XML I'll send it Email, Diag page has Additional I J led's to view.

N10 (*****)
N11 G90;-------------ABS
N12 G91;-------------INC
N13 G90 G91.1;-------NO ABS, IJ INC
N14 G90 G90.1;-------NO ABS, INCH
N15 G90 G20;---------ABS, INCH
N16 G90.1;-----------IJ ABS
N17 G91 G21;---------INC, MM
N18 G90 G20;---------ABS, INCH
N19 G91 G21;---------INC, MM
N20 G90.1;-----------IJ ABS
M30
%

Thank's, Chip