[bigatom]

Hi all, Just to keep the ProMiCA thread alive.

I have a SX3 with ProMiCA conversion and IC3A.

Currently building an adaptor to make the IC3A pin compatible with a Mesa 5i25 i/o card as used by Tormach's PathPilot software.

Almost there, I have movement and home switches, can't ESTOP from the IC3A big red button yet. After sorting that just need to change a couple of config files to fix steps/mm and the like.

I've given up on Mach3, I tried to make my G code a bit more sophisticated using tool radius compensation G41 on G02 and G03 moves which resulted in three broken tool bits. Checked things out cutting air, cut a couple of parts, all going well then BANG, a G00 move to X0 Y0. Played with the G code a lot, worked most of the time then a random G00 would come out of nowhere.

Other thing was Mach4 licensing, did the right thing and bought a Mach3 license, Mach4 comes along and I'm expected to pay full price with no discount, don't mind paying something but full price again? Also, the demo version only runs a couple of minutes, not long enough to make any assessment.

[RCaffin]

all going well then BANG, a G00 move to X0 Y0. Played with the G code a lot, worked most of the time then a random G00 would come out of nowhere.

Curious. I don't think I have heard of that happening before in a reproducible manner.
Tool compensation can be tricky, but random G0s creeping in? Somehow, I doubt it.

Cheers
Roger

[bigatom]

Hi Rodger,

Thanks for your comment, I can understand your scepticism. I've used Mach3 for several years without problems until this.

I searched for any mentions of the problem and found one reference to unplanned G00 moves. Lots on personal preferences for different versions of Mach3 that particular users considered the 'best' for tool radius comp.

I've attached my g code for you (or anyone) to point out where I'm going wrong, but please no comments on style or " I would have done it this way", just why this particular example of a valid g code program crashes tool bits.

It cuts a 13mm boss 2.75mm high on the end of a bit of 17mm bar. X0,Y0 is the centre of the bar, Z0 is the previously surfaced end of the bar.

If you think it should be fine I invite you to run it several times and see if it works for you

[RCaffin]

Hi bigatom

Well, the code runs fine for me, but I have a couple of doubts. And yes, most of them are around G41.

First of all, I don't really trust Mach3 with G41. You have to get the lead-in right, and I am not convinced Mach3 does this right every time. Maybe I screwed up, or maybe there is a bit of a bug there (among many others).

The line after the one with g41 at the start should be a no-op: g01 x-12.75 to where the cutter already is. How this interacts with G41 might be of concern.

My understanding is that Mach3 still has problems with 360 degree G2 and G3 moves. I always break them into two-off 180 degree moves, and never have any problems.

I see that you are cutting a 13 mm boss with a 10 mm cutter with tool with cutter radius compensation turned ON, but you don't seem to have defined the cutter radius inside the script. OK, it was done beforehand? Leaving that sort of thing undefined worries me.

Cheers
Roger

[bigatom]

Hello Rodger,

Did you run it several times with hears tuned for a rapid move?

I gave Mach3 every chance of getting it right, cut air then adjusted Z offset, it would work, reload the stock, adjust Z offset it might work again or it might do the G00 move.

After a crash I'd reboot and start again an get the same thing, of course it would never fault when cutting air, only when actually cutting but that's just the way the world works.

Despite your mention of the null move after G41 would you agree the program is valid and should work?

Shouldn't have to break a 360 move in to two 180s, it should just work. That sort of thing is why I lost faith in Mach3, what other problems are lurking to catch me out.

The tool diameter was set in the tool table to 3 decimal places. I thought that was the way to do it. I could then change to another size tool and not touch the program. Also I could change the diameter in the table down a fraction and end up with a smaller part and home in on a press fit.

[RCaffin]

Hi bigatom

No, I didn't cut any metal. But yes, the program looks quite valid to me.
Can you identify what line the program was at when the G0 happened?

I will be off the air for much of next week and unable to reply.

Cheers
Roger

[bigatom]

Can you identify what line the program was at when the G0 happened?

Could never be sure, but could be line 15 or 16 or just before line 15.

[mactec54]

The program as posted is not a valid program like it is, there are lots of problems, if trying to use G41 it has to be implemented correctly, the way you have it there will be a crash, because it can't offset the tool

(cut boss 13mm 2.75 mm deep)
%
G80 G21 G17 G50 G90
G49 G40 G64 G00 ( G00 G49 & G50 should not be in this safety line )
M3
G00 Z 50.0 F 400 ( You can't change this to a feed move, G00 is rapid move only )
G00 X 0.0 Y 0.0
T1 (10mm 4 flute endcut)
M06 G43 H1
S 1475
F51
G00 X -20.0
G00 Y +6.5 ( You can't use a + sign, it should be just G00 Y 6.5 )
G00 Z 0.0
M08
G41 G01 X -12.75 Y 6.5 ( You have no feed move, you need a F--- )
G01 X -12.75 ( This is not valid for cutter comp )
G01 X 0.0 Y 6.5
G02 X 0.0 Y 6.5 I 0.0 J -6.5 Z -1.5
G02 X 0.0 Y 6.5 I 0.0 J -6.5 Z -2.75
G02 X 0.0 Y 6.5 I 0.0 J -6.5 Z -2.75
G01 X 20
G01 Z -3
G01 Y -6.5
G01 X 12.75
G01 X 0.0
G02 X 0.0 Y -6.5 I 0.0 J 6.5
G01 X -12.75
G40 G01 X -20
M09
G00 Z 50
G00 X 0 Y 0
M05
M02
% ( Percent sign at start & end of program )

Not sure what you are trying to do with your cutter comp, but it is no correct

Will Mach3 run this program yes it will, Mach3 will run almost anything you through at it, but will not always execute it correctly, because of bad coding, would I run this on my machines No I would not, It will break tools

[bigatom]

Hi Mactec45,

Don't know what the G00 and G50 are doing there at the top, didn't know G49 was a problem. The lines at the top are my standard setup lines I've used for years, must have had a one finger typing failure at sometime.

The program went through many, many changes, F400 on G00 is a hang over from a previous G01, '+" signs as far as I know are OK, and feedrate is set with F51.

I take note of your comments but still have doubts about Mach3, it works some of the time and crashes now and then. Inconsistent behaviour in any software is not a good sign.

[mactec54]

Hi Mactec45,

Don't know what the G00 and G50 are doing there at the top, didn't know G49 was a problem. The lines at the top are my standard setup lines I've used for years, must have had a one finger typing failure at sometime.

The program went through many, many changes, F400 on G00 is a hang over from a previous G01, '+" signs as far as I know are OK, and feedrate is set with F51.

I take note of your comments but still have doubts about Mach3, it works some of the time and crashes now and then. Inconsistent behaviour in any software is not a good sign.

G49 cancel tool offsets, you don't use this unless you are doing tool changes with out a tool call T1 & G43 H 1 is not in use, you are using it so should not do this,

Plus + sign is not ok to use

Where you have the Feed F51. it is not valid, once you use a G00 then you need a Feed call for your next move like G01 X-12.75Y 6.5 F51. this feed is then valid until your next G00 move

[RCaffin]

Hi Mactec

Plus + sign is not ok to use

UM. I respectfully disagree. According to the Mach3Mill manual:
A number consists of (1) an optional plus or minus sign, followed by (2) zero to many digits, followed, possibly, by (3) one decimal point, followed by (4) zero to many digits - provided that there is at least one digit somewhere in the number.

Where you have the Feed F51. it is not valid, once you use a G00 then you need a Feed call for your next move like G01 X-12.75Y 6.5 F51. this feed is then valid until your next G00 move

UM again.
I have some problems with this idea. I have been machining with Mach3 on a semi-commercial basis 'for a few years', and I have found a Feed command to be totally persistent until the next Feed command. Switching between G00 and G01 has never required a new feed command for me. YMMV

Cheers
Roger

[bigatom]

Hello Rodger,

I've been using "+" for years, not required but sometimes as a reminder to me about something.

There were several fixed number formats tears ago, maybe they didn't allow "+", I don't know.

As you say "F" once set is there till the next "F".

Ken

[mactec54]

Hello Rodger,

I've been using "+" for years, not required but sometimes as a reminder to me about something.

There were several fixed number formats tears ago, maybe they didn't allow "+", I don't know.

As you say "F" once set is there till the next "F".

Ken

Whether you have been using it for years or not, it is incorrect, the only time a + Plus is used is when you are using Macro B programing format, ( #1 = [#2 * #3] + #4 ), it has no place in any normal G-Code Programing

As for the F= Feed is Modal so is active all the time until changed, It is how you used it, that it is not normal for G-code programing

Mach3 was made very forgiving, and will run almost anything you through at it, Try adding a + in the real world, and you would either crash the machine, or if it is smart enough it will just fault out

[RCaffin]

Hi Mactec

Do you know where Art got the Mach3Mill manual from? He did not write it all himself. Large parts of it are lifted straight out of the NIST RS274 NGC Interpreter reference manual. This applies especially to the section on g-code. The quote I gave about number format is an exact copy of the NIST V3 manual, section 3.3.2.1 on page 17.

I am aware that many CAM generators may stick the F command in whenever they enter G01 mode, but that is a feature of the CAM SW, not of the NIST definition or requirements. Microsoft does things like that too when converting a doc to HTML for instance, but their HTML is execrable crap. The F command is modal, and always has been for NIST-compliant systems. I cannot speak to systems which are not NIST-compliant.

If adding a '+' sign can crash a machine, then that machine is not NIST compliant. But I am intrigued: what actual brands of machines do this? Do tell, please!
As far as I can see, there is no prohibition on using '+' signs in Macro B either.

Cheers
Roger

[mactec54]

Hi Mactec

Do you know where Art got the Mach3Mill manual from? He did not write it all himself. Large parts of it are lifted straight out of the NIST RS274 NGC Interpreter reference manual. This applies especially to the section on g-code. The quote I gave about number format is an exact copy of the NIST V3 manual, section 3.3.2.1 on page 17.

The + sign is only used in macro programing, and then it is very rear that it is ever used, it also has to be used in a special way/ format

I am aware that many CAM generators may stick the F command in whenever they enter G01 mode, but that is a feature of the CAM SW, not of the NIST definition or requirements.The F command is modal, and always has been for NIST-compliant systems. I cannot speak to systems which are not NIST-compliant.

I already stated that the F command is Modal, It has nothing to do with cam programs, It how G-Code Programs are Formated that counts

If adding a '+' sign can crash a machine, then that machine is not NIST compliant.
As far as I can see, there is no prohibition on using '+' signs in Macro B either

I already stated that the + sign is used for Macro B programing, below is what you quoted you obviously don't understand what has been written in the NIST RS274 Manual

[RCaffin]

Hi Mactec

I can see we will have to agree to disagree.
I interpret the first bullet point in 3.3.2.1 literally - as does Mach3.

But I would still like to know exactly what machine will crash if it tries to execute g01 x+3 .

Cheers
Roger

[mactec54]

Hi Mactec

I can see we will have to agree to disagree.
I interpret the first bullet point in 3.3.2.1 literally - as does Mach3.

But I would still like to know exactly what machine will crash if it tries to execute g01 x+3 .

They won't always crash, they just will not run or Fault out, until the program is corrected ( Macro Programing Not Supported )

Any machine control that does not support Macro Programing, which is most, this is a costly add on, Fanuc 0i series is the only control that support Custom Macro B Programs and only if it is activated

Regular Macro's most controls support it, Only if you pay the extra to have it activated

Mach3 supports it, because it can use Macro Programs, your Quote of 3.3.2.1 is reference to Macro Programing, Not regular G-Code Programing and the + sign has a function, not the way you have Quoted it, but is used as per the example I posted

It's fun using Macros if you know how to program and use them

[RCaffin]

Hi Mactec

your Quote of 3.3.2.1 is reference to Macro Programing,

The Chapter is headed 3 Input: the RS274/NGC Language. The 1st para is This section describes the input language, RS274/NGC. This section is intended for NC programmers, machine operators, developers and researchers.
Section 3.3 Format of a Line includes the following text:
Spaces and tabs are allowed anywhere on a line of code and do not change the meaning of the line, except inside comments. This makes some strange-looking input legal. The line “g0x +0. 12 34y 7” is equivalent to “g0 x+0.1234 y7”, for example.
In this case the NIST Standard explicitely includes the '+' sign in a number as part of a g-code statement. The word 'Macro' does not occur in this chapter.

Now, whether Fanuc or others using antique hardware-based interpreters can handle the '+' as part of a number - that's another matter. Maybe they can, maybe they can't. But if they can't, then they are in violation of the NIST Standard.

Cheers
Roger

[mactec54]

RCaffin

Wow I already posted all that, no they do not say the word macro, go down the page it soon changes into macro programing examples, but do not say it is, if you don't know what macro programing is then there is plenty of information on the web that could help you understand what it is all about

None of these controls or manufactures are in any violation of any NIST standard I have never found a mainstream control that the G-code programing is not to the RS274 Spec's, add on's are a different story they can be any flavor the manufacturer chooses to suit for there machine

[RCaffin]

Hi Mactec

go down the page it soon changes into macro programing examples,

Can you give me some concrete examples please? All I can see in section 3 is standard g-code, but perhaps I am missing something?

if you don't know what macro programing is then there is plenty of information on the web that could help you understand what it is all about

Well, I think I know what I mean by macro programming, but perhaps I don't understand what you mean.

For the record: I started Assembly Language programming around 1970. I have written science programs, device drivers, database kernals and database systems, debugged operating systems and compilers for major commercial companies, and (I claim to) have forgotten more assembly languages than I can count (some were better designed than others). I have designed and built custom robotics systems for industrial use, real-time image analysis systems for the robots (both were a complete success), and medical image analysis systems for cancer research. I have been a committee member and chairman of an international computer society. Computing and Real Time Control are 'not new' to me.

I think I know what the word 'macro' means for me, but other uses may be different.

Cheers
Roger