[mdred68]

I've had my tormach for about three months and im pleased with the machine. Recently i had a job with an unusual shape. While i was tweeking in some of the dimensions i tried to use a G41 command to adjust the tool path. After working for an hour on the problem i called tormach for help. The tech on the phone told me that mach 3 doesn't recognize G41, or G42. He told me to go back to sprut cam and change the size of the tool and repost the job. This will take an aweful long time. Does anyone out there have a better solution? Why would tormach put G41 and G42 in their list of G codes and why would they have verbage in their manual about the command?

[saabaero]

I have used cutter compensation numerous times when I needed a precise fit and needed to work up on the finished size. In Sprutcam I set the compensation to control which puts the toolpath right on the 2D contour. For some reason the Tormach post doesn't include the G41/G42 code so I enter it manually. The entry and exit lead-in are important and I include a linear lead-in move at a right angle that is longer than the diameter of the cutter. If you don't have a lot of room you can perform the move above the workpiece then advance the "Z" axis before starting the actual cut. I do the same thing on the exit move.
The actual code can be found in my reply to a Sprutcam forum threading question.

http://www.cnczone.com/forums/sprutc...utcam_7_a.html

[davidperry3]

I found out the hard way that cutter comp does not work on the tormach. It causes an odd jump in the tool path. If you watch carefully right before the first cut it makes an odd move away from the part (to the right) then moves on normally (way too slow I know).

[nomedia="http://www.youtube.com/watch?v=fj5wqxAig5M"]YouTube - Tormach Thread Milling 1018 Steel[/nomedia]

I was brand new with the machine and cnc so I did not catch the problem. Every third part the machine had missed enough steps to go out of tolerance on the part. Eventually I called Tormach and they said never use radius comp. This is a great pain to me becaus so many of the wizards use G41/G42. If I want to do any helical machining I have to run inside and do it in Sprut (I dont want to hand write that much code).

Tormach can you fix this?

[ger21]

Cutter Comp works fine in Mach3, so I'm not sure why it doesn't on the Tormach. I don't think they can just take it out. What version of Mach3 is it?

Also, if it's making an "odd jump", perhaps you don't have a proper lead in move, which is required.

[Scott_M]

It works in Tormach's version of Mach 3. I am not sure why they say it is "not supported".
But it is real easy to get in trouble. You must have safe entry and exit moves. If space won't permit, it must be applied or cancelled above the part.

Scott

[saabaero]

I agree with Scott_M and ger21 the key is in using the correct lead in and lead out. I have only used it with a 2D contouring operations but have used it many times without problem.

Try this code to create a left hand thread using cutter diameter compensation.

G21 (Metric)
(2D Contouring)
M998
T35 G43 H35 M6
(0.500" thread mill)
S3500 M3
G0 X24. Y0. Z5. ('compensation switch out' lead in for cutter comp.)
G42 (turn cutter comp. on)
G1 Z0. F100 M8
X8.
G3 X8 Y0 Z-1. I-7.99999 J0.00001 F200 (start 1mm above part)
X8 Y0 Z-1. I-7.99999 J0.00001 (repeated 16 more times while "Z" increments 1mm each time)
...
G1 X24. ('compensation switch out' lead out for cutter comp.)
G0 Z1.
G40 (turn cutter comp. off)

[davidperry3]

These are screen shots of a short thread mill program done with the newfangled wizard. The missed step is clear on the lead in and out but it is also there on the larger curve. Interestingly the program knows that this is going to happen the curves in purple are the programed path but the white arcs are what will happen.

[benji2505]

I frequently work with radius comp, because I measure my cutter every 20 parts or so and then correct the radius in the tool table.

With the correct lead-in and lead-out I have not had a single problem with the radius comp. I would refer to the manual for the correct lead-in and lead out.

[davidperry3]

In 6.8.1 of the Tormach manual they say "avoid the use of G41 and G42 commands". They mean it, I have a pile of dead parts to prove it.

[300sniper]

i don't have my manual near me but i swear they had a section explaining how to use g41/42. it's a first generation manual if that means anything.

i have honestly only tried radius comp one time and a bunch of weird arcs appeared on the screen. i never did diagnose why that was happening but i think i asked the question here a few years ago.

[Freddy Bastard]

I use cutter comp everydays. The best way to use it is in WEAR mode. So your CAM system comp the tool and output a G41-G42. On the machine, you just adjust the wear of the tool ie: -.001". And you have to comp on a line move (G01) so the lead-in and lead-out are very important. If Tormach told you it don't work, then, they are completely wrong. I program my part in Mastercam, and set the comp to WEAR. I would stay away from CONTROL comp (the cam, don't compensate the tool but output a G41-G42)

[ger21]

I would stay away from CONTROL comp (the cam, don't compensate the tool but output a G41-G42)

I do it this way on almost all of my parts with Mach3 and don't have any problems.

Note that there are some issues with comp in Mach3 that will be addressed in the next version (4), which is probably still a long way from release, and even longer for a Tormach release. What those issues are I don't know, as I haven't seen them.

One thing I noticed in the past was that Mach3 changed the way G41/G42 works with an arc lead in move. I use an AutoCAD macro to create my code, and needed to change the way I did arc lead-in moves. This was a year or two ago, though.

Looking at your screen shot, it looks like the length of the lead-in move is less than the tool radius (P 0.0625), which is a bad thing. Perhaps the Wizard was written to work with older versions of Mach3, and got broken in newer versions? Do you have the latest revision of the Newfangled wizards, as they are updated periodically to fix bugs. You can get it somewhere on the Mach forum.

[BobWarfield]

Note that there are some issues with comp in Mach3 that will be addressed in the next version (4), which is probably still a long way from release, and even longer for a Tormach release. What those issues are I don't know, as I haven't seen them.

That's why Tormach is recommending not to use cutter comp, dollars to donuts.

I have heard a number of reports from different folks that cutter comp is "iffy" in Mach3. I have heard from a number of folks that say it works great. Kinda like this thread, LOL.

From those who've been able to elaborate, the impression I get is that if you do everything exactly the way Mach wants it, it will work most of the time. But, "exactly the way Mach wants it" is supposedly not exactly how the rest of the CNC world operates.

To make things more exciting, the differences are apparently not documented, and there are concerns that if 4.0 "fixes" the differences so that it works like Fanuc et al, then the folks that got it to work will be unhappy as their code quits working.

One step Brian should take is documenting the issues so people know what to do now, and what it will be like later.

Cutter comp is a messy business to build in software (he said while working with it in the G-Wizard G-Code Editor), but it sure is useful to machinists.

Cheers,

BW

[ger21]

To make things more exciting, the differences are apparently not documented, and there are concerns that if 4.0 "fixes" the differences so that it works like Fanuc et al, then the folks that got it to work will be unhappy as their code quits working.

One step Brian should take is documenting the issues so people know what to do now, and what it will be like later.

What it will be like "Later" is documented on the Mach forum. Unless of course it changes before then.
New Cutter Comp code and Examples

[BobWarfield]

What it will be like "Later" is documented on the Mach forum. Unless of course it changes before then.
New Cutter Comp code and Examples

ger, that thread is a better example of the problem. It talks about 3.x, but not really 4.x. It is filled with little issues and it ends without having answered your question. To top it all off, the thread starts in 2008, ends in 2009, and here we are in 2010 still wondering about cutter comp.

Maybe it's just a hard concept and it's all user error, but it sure doesn't seem like it. Interestingly, a search on G41 in the Mach forums shows tons of traffic with tons of problems 2 years later.

Like I said, the impression one gets is that it is very buggy, but enough people get it to work that maybe rather than bugs there are just some relatively undocumented limitations or styles that have to be followed for success.

If the limitations could be well documented, maybe people would quit viewing them as bugs and get on with using the feature more successfully. Seems like probably there are some post options for CAM programs that could be documented that lead to higher reliability.

Cheers,

BW

[ger21]

I haven't read it in a long time, but the thread was about a revised comp test version, with the comp code that would be in V4. Afaik, the comp worked perfectly in the test version if you followed the rules in the first post. However, that version had some other bugs (not comp related) that prevented it from being used and was removed. It was 3.43.000 I think.

I read most if not all of the comp posts on the Mach forum, and imo it's almost always an issue of incorrect lead in moves (or lack of them).

If you do a G1 lead in move that's longer than the tool radius, and make sure all inside radii are larger than the tool radius (you'll get an error message if you violate that one), it works for me 100% of the time.

There is a bug, that G41/G42 does not work in subroutines.