Hello Guest it is May 11, 2021, 09:27:38 PM

Author Topic: G49 on Mach3 Mill  (Read 6602 times)

0 Members and 1 Guest are viewing this topic.

Offline rcaffin

*
  •  1,035 1,035
    • View Profile
Re: G49 on Mach3 Mill
« Reply #10 on: February 03, 2018, 05:01:30 AM »
Ah so. I see.

You could write a small VB program to read your file in and write it back out again, skipping every G43 found along the way.
I will assume that any g43 instruction will appear as G43 H~, so you would really have to find "G43 H" and any following number.
Fairly mechanical in use. Testing to be done with a large block of foam.

Cheers
Roger

Offline Davek0974

*
  •  2,606 2,606
    • View Profile
    • DD Metal Products Ltd
Re: G49 on Mach3 Mill
« Reply #11 on: February 03, 2018, 05:54:00 AM »
My post seems to go G43 Zfeed start height Hnn

IIRC there needs to be an axis call on the G43 line, maybe wrong though, either way it works fine with the G43's deleted.
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline rcaffin

*
  •  1,035 1,035
    • View Profile
Re: G49 on Mach3 Mill
« Reply #12 on: February 03, 2018, 03:49:17 PM »
Hi Dave
With all due respect to whoever wrote your postP, writing G43 Zfeed start height Hnn is just plain obscure.
I know some manuals pack up instructions from different groups - maybe to reduce the number of lines in the program, but today there is no justification for that. The Haas manual uses G43 H01 Z0.1 M08 (M08 = coolant on) as an example, but it is not clear whether the Zn is applied before or after the G43 H01 is applied.

Well, you could just filter out the entire G43 line and optionally leave the Z bit in.

Cheers
Roger

Offline Davek0974

*
  •  2,606 2,606
    • View Profile
    • DD Metal Products Ltd
Re: G49 on Mach3 Mill
« Reply #13 on: February 03, 2018, 04:15:32 PM »
It was the original post that comes with F360, no idea of author ;)

Looks like this...
Code: [Select]
(T3  D=6. CR=0. TAPER=90DEG - ZMIN=-2. - CENTER DRILL)
(T6  D=12. CR=0. - ZMIN=-2.5 - FLAT END MILL)
(T8  D=8.1 CR=0. TAPER=118DEG - ZMIN=-10. - DRILL)
(T10  D=6.1 CR=0. TAPER=118DEG - ZMIN=-10. - DRILL)
(T15  D=10. CR=0. TAPER=45DEG - ZMIN=-2. - CHAMFER MILL)
(T98  D=6. CR=0. - ZMIN=-10. - RIGHT HAND TAP)
N10 G90 G94 G91.1 G40 G49 G17
N15 G21
N20 G53 G0 Z0.
N25 G90

(DRILL1)
N30 M5
N35 M9
N40 T3 M6
N45 S3000 M3
N50 G54
N55 M7
N65 G0 X6.259 Y43.837
N70 G43 Z25. H0
N80 Z5.
N85 G98 G81 X6.259 Y43.837 Z-2. R5. F535.

It's always followed by another Z call so the one on the G43 line is always not needed and it runs fine if i just delete those lines.

I could build a small VB6 app that scans and deletes or maybe one that copies all the g-code from my transport USB stick to the hard drive and  at the same time filters them, wouldn't be hard.

Wouldn't know how to build the code into the "File Open" function though :)

And this is the Vectric Aspire Post....
Code: [Select]
(Toolpaths used in this file:)
(Slots)
(Profile 1)
(Tools used in this file: )
(1 = T1 - 2mm Carbide YG)
N110 G00 G21 G17 G90 G40 G49 G80
N120 G71 G91.1
N130 T1 M06
N140 (T1 - 2mm Carbide YG)
N150 G00 G43 Z23.000 H1
N160 G00 Z23.000
N170 S23200 M03
N180 M07
N190 (Toolpath:- Slots)
« Last Edit: February 03, 2018, 04:18:15 PM by Davek0974 »
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline rcaffin

*
  •  1,035 1,035
    • View Profile
Re: G49 on Mach3 Mill
« Reply #14 on: February 03, 2018, 06:02:56 PM »
I doubt it can be put into 'File Open' in Mach3: the hooks are not there.
VB is probably the way to go. I have done that before to filter stuff out of a file produced by LazyCam.

I note you point that the G43 is followed by the same move command on the next line. I suspect the author of the post did not know what to do there either! The Haas manual includes a Z~ but does NOT explain it adequately; the Mach3 manual omits the Z~ from the G43 line. Me, I strongly favour simple program lines - partly because of my programming style.

Cheers
Roger

Offline Davek0974

*
  •  2,606 2,606
    • View Profile
    • DD Metal Products Ltd
Re: G49 on Mach3 Mill
« Reply #15 on: February 04, 2018, 03:02:00 AM »
Yes, i might write a little import app to filter it out.

I am sure i read somewhere that Mach ignored the G43 line unless there was an axis move in the same block.
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline rcaffin

*
  •  1,035 1,035
    • View Profile
Re: G49 on Mach3 Mill
« Reply #16 on: February 04, 2018, 03:25:35 AM »
Mach ignored the G43 line unless there was an axis move in the same block
I haven't seen anything like that, but I miss things. If you ever find the source, please post it.
I can't find it in the Mach3Mill_1.84 manual though.
But then ... there are more than a few things missing! For instance, don't try creating a macro with the name M60.

Cheers
Roger

Offline Davek0974

*
  •  2,606 2,606
    • View Profile
    • DD Metal Products Ltd
Re: G49 on Mach3 Mill
« Reply #17 on: February 04, 2018, 03:31:46 AM »
LOL, thats like saying "try creating a macro called M60 ...." :) :)


I'll try find it again but then i tend to read so much it might even have been in a manual for Fadal, Haas, who knows :)

It cant just be a spoof memory though as both the posts I use mainly have the Z move in the G43 line followed by another Z move.

I might try sheet-cam later on, i only use that on the plasma so no tools anyway but it has a Mach post IIRC.
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline Davek0974

*
  •  2,606 2,606
    • View Profile
    • DD Metal Products Ltd
Re: G49 on Mach3 Mill
« Reply #18 on: February 04, 2018, 03:54:49 AM »
Does seem pretty common, here's a link to some Fanuc shortcodes...
http://www.mmattera.com/g-code/gcodes.html

It lists an axis move on all compensation moves.
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives.
Plasma table, Mach3 V062, Step motors, C&CNC THC.

Offline rcaffin

*
  •  1,035 1,035
    • View Profile
Re: G49 on Mach3 Mill
« Reply #19 on: February 04, 2018, 03:57:39 AM »
both the posts I use mainly have the Z move in the G43 line followed by another Z move.
Could be copied from the Haas/Fanuc manual - as you have noted.

I spent two days trying to get my M60 macro to work, but it kept coming up with a weird error msg. I changed the name to M70 and it worked immediately. I think there may be something in the archive here about M60 as well. I suspect 'they' reserved it but never got the code (in Mach3) finished.

Cheers
Roger