Hello Guest it is October 17, 2019, 02:18:35 AM

Author Topic: mach 3 tool offset issue  (Read 2838 times)

0 Members and 1 Guest are viewing this topic.

mach 3 tool offset issue
« on: April 12, 2017, 04:01:40 PM »
Hi.  I am a new to gcode and cnc.  Trying very hard to learn the basics.  I have a harbor freight mill I converted and I am running mach 3.  I am having a hard time running a very simple program.  The problem is with the tool offset.  The program will run sometimes once and sometimes not at all.  If it runs right, I will try and rewind it and run it again and it just goes crazy.  Cutting anywhere and not following any gcode.  I setup the tool diameter in mach 3 at .250.

What am I doing wrong.  It will run without the g41, but then the offset it wrong.  It has something to do with g41 I am pretty sure.  

Here is my code:
%part 1%
G20 G91 G41
G0 X.50 Y.50 Z0
G1 Z -.05 F10
G1 Y1
G1 X1
G1 Y-1
G1 X-1

Any explanation of this would be greatly appreciated.  

Thank you,


Offline Graham Waterworth

  • *
  •  1,889 1,889
  • Yorkshire Dales, England
    • View Profile
Re: mach 3 tool offset issue
« Reply #1 on: April 16, 2017, 04:10:01 PM »
Hi Michael,

for a start you are working in incremental mode so to run the program more than once you have to make sure the first run of the program ends at the same place as it started.

It is much better to work in Absolute (G90) mode.

G20 G90
G00 X.5 Y.5 Z0
G01 Z-.05 F10.
G00 Z0

Without engineers the world stops

Offline ger21

  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: mach 3 tool offset issue
« Reply #2 on: April 16, 2017, 07:33:32 PM »
And you're not using G41 properly.
You should be applying the G41 comp during a lead in move, and turning it off with G40 on a lead out move.

2010 Screenset

JointCAM Dovetail and Box Joint software
Re: mach 3 tool offset issue
« Reply #3 on: April 17, 2017, 02:38:53 PM »
G41 is modal, stays in effect until canceled by G40. I used to use it all the time and it works well as long as you understand the gotchas. I always apply g41 before any move down in the Z into the part. I also use a very short .01" move right after g41 so it gets applied and I can see it went the right way. If you try to do an inside corner that has a radius smaller than radius comp many controls will give you the dreaded 'crop circles' where it goes around the outside of the path destroying your part. Always cancel g41 when done, and never cancel while still touching the part. Hope this helps
Re: mach 3 tool offset issue
« Reply #4 on: April 17, 2017, 08:51:19 PM »
I switched to absolute and it fixed the problem,  the program is now repeatable. I need to read up on g41.  I dont understand the lead in and out.  I undertand g41 being modal.  I really appreciate the help.  Gcode on the surface seems easy, but then you get into the finer points and it gets crazy quick.

Offline RICH

  • *
  •  7,367 7,367
    • View Profile
Re: mach 3 tool offset issue
« Reply #5 on: April 18, 2017, 06:41:31 AM »
The attached file provides some info on cutter compensation and includes some
posts by Graham and Gerry.

There is a lot of info on cnc programing  but You may want to consider purchasing CNC Programming Handbook by Smid.

Re: mach 3 tool offset issue
« Reply #6 on: April 18, 2017, 01:44:06 PM »
When mach 3 sees a g41 it moves the tool to the side of the path when it makes the NEXT move. So you need that to happen before you lower the tool into the material. Otherwise the tool will gouge out the starting point. When you cancel with g40 the tool moves  back to be centered on the next move, gouging out the finish point unless you are clear of the material. Once you ruin half a dozen parts you'll get the idea!