Hello Guest it is July 11, 2020, 11:21:02 PM

Author Topic: Turning Syntax  (Read 4622 times)

0 Members and 1 Guest are viewing this topic.

Turning Syntax
« on: May 25, 2009, 09:25:04 PM »
I'm running a program to do some simple turning (shown below -just the bit with the arc move in) and all goes fine until it gets to the arc move.  I just end up with a straight line between atart point and end point.  is there something wrong with my code, or do I need to change some mach settings.

Also, if the software is configured in imperial (I have imperial leadscrews) can I get it to default to metric units or do i need to configure the machine in metric (which is dd figures with an imperial leadscrew, but possibe).

Regards
Kevin

N03190 Z-7.
N03200 X9.8
N03210 G00 Z-0.4
N03220 G01 X9.4
N03230 Z-7.
N03240 X9.6
N03250 G00 Z-0.4
N03260 G01 X9.2
N03270 Z-7.
N03280 X9.4
N03290 G00 Z-0.4
N03300 G01 X9.
N03310 Z-7.
N03320 X9.2
N03330 X19.8
N03340 G01 X21. Z-8.2 R1.2
N03350 G00 X25.8
N03360 X25.885 Z0.323
N03370 M30

Offline Chip

*
  • *
  •  2,055 2,055
  • Gainesville Florida USA
    • View Profile
Re: Turning Syntax
« Reply #1 on: May 25, 2009, 09:43:23 PM »
Hi, Kevin

You've got a G01 in the code instead of a G03 or G02.

N03190 Z-7.
N03200 X9.8
N03210 G00 Z-0.4
N03220 G01 X9.4
N03230 Z-7.
N03240 X9.6
N03250 G00 Z-0.4
N03260 G01 X9.2
N03270 Z-7.
N03280 X9.4
N03290 G00 Z-0.4
N03300 G01 X9.
N03310 Z-7.
N03320 X9.2
N03330 X19.8
N03340 G03 X21. Z-8.2 R1.2 ;******************
N03350 G00 X25.8
N03360 X25.885 Z0.323
N03370 M30

Chip
Re: Turning Syntax
« Reply #2 on: May 25, 2009, 10:08:08 PM »
DOH!!!! That was the wrong code, I was experimenting with some settings when I did that (I thought I'd deleted it). This was the code I meant to post

N03350 G00 Z-0.4
N03360 G01 X9.
N03370 Z-7.
N03380 X9.2
N03390 X19.8
N03400 G02 X21. Z-8.2 I19.8 K-8.2
N03410 G00 X25.8
N03420 X25.885 Z0.323
N03430 M30

Offline Chip

*
  • *
  •  2,055 2,055
  • Gainesville Florida USA
    • View Profile
Re: Turning Syntax
« Reply #3 on: May 25, 2009, 10:49:03 PM »
Hi, Kevin

You need to set IJ's to ABS mode ( put a pre-amble in the top of your code ).

Also changed the G02 to G03, What are you posting code with. ?

G90.1 ;----------IJ ABS set pre-amble

N03350 G00 Z-0.4
N03360 G01 X9.
N03370 Z-7.
N03380 X9.2
N03390 X19.8
N03400 G03 X21. Z-8.2 I19.8 K-8.2 ; G02 changed to G03
N03410 G00 X25.8
N03420 X25.885 Z0.323

G91.1 ;----------IJ ABS set post-amble set's back to IJ INC

N03430 M30

%

Chip
« Last Edit: May 25, 2009, 10:58:45 PM by Chip »
Re: Turning Syntax
« Reply #4 on: May 25, 2009, 11:43:44 PM »
Thanks, I'm missing the G90.1 The start of my code looks like this

N00010 G21 G40 G99
N00020 G97 T0000 S500 M03 G54
N00030 G00 X26.113 Z0.421
N00040 X28.14 Z-0.4
N00050 G94 G01 X25.4 F30

It's programmed in Xturn (part of the XCad, Xmill package that then became Excalibur and then seemed to dissapear).  Is it best to use the G90.1 to set IJ moves to ABS or just change the postprocessor to output them as incrimental (either is easy).

Regards
Kevin
Re: Turning Syntax
« Reply #5 on: May 26, 2009, 12:09:13 AM »
I'm confused about G02/G03 as mine seem to be the other way round -see pic

Offline Chip

*
  • *
  •  2,055 2,055
  • Gainesville Florida USA
    • View Profile
Re: Turning Syntax
« Reply #6 on: May 26, 2009, 01:07:47 AM »
Hi, Kevin

In your Post is best in the long run, The big thing is setting Mach and leaving Mach in the same Control State after you've run different G Code files, So a good pre-amble to configure the Control is very Important.

There's a Initialization String in Config, General Configuration Page for Start-Up, But it doesn't treat the settings as separate line values, So it won't truly reset Mach in some case's, Probably one of the biggest Issues New User's Have.

In your posted code Snippet's I wasn't paying attention to your X axis setting's, There Backwards -X should move cutter left.

Chip
« Last Edit: May 26, 2009, 01:47:18 AM by Chip »
Re: Turning Syntax
« Reply #7 on: May 26, 2009, 01:41:27 AM »
Thanks for the advice.  I'm not worried about the X or Z axis settings -I know which way they are going, and it matches the postprocessor settings in the cam.  The important thing was the G90.1 setting, just tried the program with that in and it worked great -no more chamfers instead of arcs.  Is it important to put the G91.1 in at the end?

Regards
Kevin

Offline Chip

*
  • *
  •  2,055 2,055
  • Gainesville Florida USA
    • View Profile
Re: Turning Syntax
« Reply #8 on: May 26, 2009, 01:49:18 AM »
Hi, Kevin

You Should Be, I edited my post Above.

Chip
Re: Turning Syntax
« Reply #9 on: May 27, 2009, 01:53:01 AM »
Hi,

Double checked my axis today, and everything seems to be the right way round.  Plus moves away from the job and minus takes me in to the job on both axis, and they travel the same way as the cursor keys whan I jog.  All seems to be going well.

Is there a feed rate overide on turn, I can't see it anywhere.

Regards
kevin