Work offset misbehaving.

[mactec54]

In Mastercam, that Z.5 is my clearance plane.
I use it for several things.
A visual check for my guys to run an operation in single step mode and see that they set everything correctly. It's usually 1" above zero.
Clearance for getting around clamps when I have parts clamped to a plate.
And on some parts, where the depth is critical, we actually run the program to that point and stop it. Set the Operator Z zero there, and check it with a gage pin. We can then jog the tool up or down until it's perfect, see where we arand adjust the tool offset.
It already serves a purpose in my world.

I did change the post yesterday to format the line as G53 G90 G0 Z0. Because I am a fan of things being in a sensible order, even if it doesn't make a difference.

The end of my programs send the table to yet a different zero. One that we set to be easy to swap out whatever part we are running.

G01 X-.0216
G03 X.7126 Y.3309 I0. J1.9885
G03 X.7411 Y.3468 I-.0461 J.1161
G01 G40 X.7652 Y.3647
G00 Z1.
M83
M9
M5
G53 G90 G0 Z0.
G00 G129 X0. Y0.
M30
(PUT ANOTHER PART IN THE MACHINE RIGHT NOW, JERK)
%

I wired a buzzer in to the machine at the M83 solenoid.
I didn't like the way Haas changed there beep some years ago, so I figured out my own.
Works great.

Thats old school craziness using a Gauge pin or anything that is hard to set a Tool or to check a Tool set height, you damage the cutting edges of the cutter by using this technique

Machine some aluminum or hard plastic blocks and use that, to check large Tool offsets or plastic shim down to 007" works very well and is much more forgiving than any hard metal, just rubbing a Gauge Pin or a Gauge Block damages the Cutter the first touch, Plastic is the best Aluminum at a push

Your Clearance Plane is wherever you want to park the Z axis after an operation, you are making things more complicated than they have to be

[HayreAss]

Things aren't complicated at all.
I want my machine to be at the Z machine zero after every tool, and before the program starts.
So it is.
I edited a post, once, years ago, and it has done what I wanted it to do since that day.
My reseller made it do the same when they sent me new posts a while back.
Doesn't get easier or less complicated than that.
Sorry that how I do it offends your sensibilities.

I use a clearance plane, and a safety plane.
I like that, and it's my shop.

Unless someone can tell my why I would NOT want my head parked at machine zero at the beginning of a program, and after every tool, I'll just keep on keeping on.
I haven't seen a reason yet.
I did clean up the code though, it was simple enough.

I'm also OK with verifying the tip of my .026" ball endmills with a gage pin.
Been doing it since I got this 4th axis and started making these parts 6 or 7 years ago.
Made well over a hundred thousand of these parts so far.
Seems to work.
Unless I'm a brute, I'm not going to screw up that non cutting bit of the cutter any more than it's first plunge into titanium anyhow.
Hell, I only have to do it on rare occasion when my engraving seems to be off. (usually because the part diameter varied a little.)
Tenths make a difference on line width when you are only cutting a few thousandths deep with a tiny ball.

We sure have strayed far from "my machine was glitching" here! And I'm OK with that, I enjoy a debate.
You may not accept that it was glitching, but Haas, myself, and my local tech (who is actually sharp, not like a lot of techs) have all accepted the glitch.

[mactec54]

Things aren't complicated at all.
I want my machine to be at the Z machine zero after every tool, and before the program starts.
So it is.
I edited a post, once, years ago, and it has done what I wanted it to do since that day.
My reseller made it do the same when they sent me new posts a while back.
Doesn't get easier or less complicated than that.
Sorry that how I do it offends your sensibilities.

I use a clearance plane, and a safety plane.
I like that, and it's my shop.

Unless someone can tell my why I would NOT want my head parked at machine zero at the beginning of a program, and after every tool, I'll just keep on keeping on.
I haven't seen a reason yet.
I did clean up the code though, it was simple enough.

I'm also OK with verifying the tip of my .026" ball endmills with a gage pin.
Been doing it since I got this 4th axis and started making these parts 6 or 7 years ago.
Made well over a hundred thousand of these parts so far.
Seems to work.
Unless I'm a brute, I'm not going to screw up that non cutting bit of the cutter any more than it's first plunge into titanium anyhow.
Hell, I only have to do it on rare occasion when my engraving seems to be off. (usually because the part diameter varied a little.)
Tenths make a difference on line width when you are only cutting a few thousandths deep with a tiny ball.

We sure have strayed far from "my machine was glitching" here! And I'm OK with that, I enjoy a debate.
You may not accept that it was glitching, but Haas, myself, and my local tech (who is actually sharp, not like a lot of techs) have all accepted the glitch.

Haas did not see what I saw, so they called it a glitch that they could not explain, I put money on it that if your program Format was corrected, (which I think you have corrected) it will never have the so call glitch again.

I want my machine to be at the Z machine zero after every tool, and before the program starts.

Correct there is nothing wrong with that, except it is normally at Z0 position for the start of every program anyway, if it has been programed correctly

There is also the G94 that we never discussed, please enlighten us what that is there for in the program.

Being able to speed up the process you would have made may more parts as well in the same time frame.

[machinehop5]

...good old machinist debate. Mactec is a fun guy to listen to.

We had a G49 debate before, he said dont need it...I say we do. its the old way (Fanuc1980's) to Cancel Tool Comp. on the Safe startup line. Haas does it with reset, M30, H0 or should cancel... maybe there is problem do not know.
https://www.haascnc.com/service/code...value=G49.html

Enjoy,
DJ

[HayreAss]

But Haas did see what you saw, and more too!
You just think the code doesn't work the way I originally posted, when in fact, it works great.
That program made 20 more parts today.
Never changed it.
That particular program has been in the machine, and unchanged since 2020. (Other than me swapping G54 for G56 to test it.)
It's back exactly as it was a week, a month, and a year ago, right now.
Hell, I have close to 60 programs that are all the same, just with different engraving patterns on them.
But 10 of the tools are the same, and start exactly like what I posted. Just with G54,or G55.
It's a stock part, with different decorations...

I have edited my post to make future programs neater, but I have no desire to re-post tried and true programs that already make me money.
And nothing you have said has explained why if what you say is correct, that it cut material when I changed G56 to G54.
G54, 55, and 56 all had the exact same numbers in them.
The same numbers that are there now, after nuking the tool table, recalibrating, and probing again. (You can see them in the pictures I posted.)
If it was defaulting to G54, it still would have cut, like all of the tools did that are programmed at G54.
It was a glitch.
They happen.
You are extremely lucky if you have never encountered an electronic glitch before.

If you can explain why 1 tool, out of 11 was cutting in a location where no work offset was set, other than glitch, I'm all ears.
Oh and it only cut air for 1 operation, it worked fine on others! That tool cuts at G56, and G55.

My guess on G94 is that the post creator added it as a safety line, making sure inverse time isn't active or something.
Doesn't hurt a thing being there.

So where exactly would I gain speed here?
In my header there's a line making sure Z is home. If Z is already home, like you say, no time lost.
At the end of every tool, I send Z home. It has to be home for a tool change anyhow, so again, no time lost.
Where am I losing time?

You seem very confident in your statements, so I don't want to just dismiss you as an argumentative quack.
But you still haven't presented any evidence that I am losing time, or why sending my tool home, when other codes will ALSO do that, is a bad thing.

Perhaps you are unfamiliar with the adage that there is more than one way to skin a cat?

[HayreAss]

...good old machinist debate. Mactec is a fun guy to listen to.

We had a G49 debate before, he said dont need it...I say we do. its the old way (Fanuc1980's) to Cancel Tool Comp. on the Safe startup line. Haas does it with reset, M30, H0 or should cancel... maybe there is problem do not know.
https://www.haascnc.com/service/code...value=G49.html

Enjoy,
DJ

We don't need it in almost every instance.
But it also does no harm if used appropriately.

So, what's the problem?

I get paid for making parts, not for how small my G code is.

[extanker59]

We make a lot of prototypes here and we put G53 Z0; M01; at the end of every tool so that, if needed, we can check the part before the next tool without having to manually move the tool away.

[HayreAss]

We make a lot of prototypes here and we put G53 Z0; M01; at the end of every tool so that, if needed, we can check the part before the next tool without having to manually move the tool away.

Right.
Why wouldn't you?

I was thinking last night about why I had G0 in mine, and I remember an instance some time ago where the machine was slowly traveling to Z home.
Mastercam was doing something strange, and finishing the part on a feed move. Don't remember how, or why. (It may have been a compensation cancelling move at the retract plane or something)
Pretty sure that I added the G0 to the post then.
No good reason not to, since I am not hand coding that.

[extanker59]

From 1990 to 2002, I worked at a place where I didn't have CAM. Later I used AutoCAD to determine points and hand wrote all the programs. Furthermore, for the first 5 years of that I had to hand input every program into the controller. No CAD or computer. I was on a mission to reduce the number of keys I had to press. I have a picture of me sitting in a chair thats on a table so I could input the programs into the controller while sitting. What a goofball.

When I first started with CAM, I was very annoyed by the unnecessary redundant G code. Lol. I have learned to accept it. Make good parts and I don't care anymore. Removing line numbers helped a lot for program size. The machines I recommended they buy all have large memories.

I worked with our CAMWorks reseller to get programs similar to my old hand written ones. So I know a portion of the posted output is just to make me comfortable. I'm OK with that.

[mactec54]

Right.
Why wouldn't you?

I was thinking last night about why I had G0 in mine, and I remember an instance some time ago where the machine was slowly traveling to Z home.
Mastercam was doing something strange, and finishing the part on a feed move. Don't remember how, or why. (It may have been a compensation cancelling move at the retract plane or something)
Pretty sure that I added the G0 to the post then.
No good reason not to, since I am not hand coding that.

Yes, you would have to have a G0 in the G53 line for it to work as intended, if the last move before it was a G1, if it was a G0 then this is Modal and would not be needed in the G53 Line
as I said there is no problem having it in the line, format is key to having reliable free running code.

Old controls needed the full string regardless, (G53G90G0) Most New / Modern Controls can use it just as G53------ and what axis you want it to move and were, nothing wrong with G53G0---- though

So, your control does not get confused, and has another (Glitch) Code format is key to trouble free running those who instruct at Haas, or any other machine manufacture will tell you the same

[HayreAss]

Yes, you would have to have a G0 in the G53 line for it to work as intended, if the last move before it was a G1, if it was a G0 then this is Modal and would not be needed in the G53 Line
as I said there is no problem having it in the line, format is key to having reliable free running code.

Old controls needed the full string regardless, (G53G90G0) Most New / Modern Controls can use it just as G53------ and what axis you want it to move and were, nothing wrong with G53G0---- though

So, your control does not get confused, and has another (Glitch) Code format is key to trouble free running those who instruct at Haas, or any other machine manufacture will tell you the same

So, no word on where I'm losing time? You have unequivocally stated that would have made many more parts in the same timeframe...

And nothing on where it was getting those numbers to cut air, if not a glitch? I posted the offset table clearly showing the offsets...
Remember, the program is back to running fine now after clearing the offset table.

Looking around this forum, I see many instances of folks running the exact same line format that I am on that program. Haas has the file and didn't say 'Hey, you should change that'
My guess is that it's a pretty standard format, even if it doesn't fit in to your style guide under best practices.

You stirred a lot of $h1t over a simple question about if anyone has seen an issue like I saw, but mostly just about wanting other folks to write programs the same as you.
The G49 is a decent example.
No, it's not needed.
But if a dude wants it in his safe startup line because it makes him feel warm and fuzzy, who cares?
It does no harm, and could possibly do good in some freak instance.
I don't know other machines, so they may need it.
In which case, it IS best practice to put it in there, so it's instinct when moving between machines.

[HayreAss]

(...)

There is no time savings between me telling the machine to go to Z home, and the tool change doing the same thing.
It simply bothers you how I choose to do it.
Rather than say that, you throw out BS like 'you would have made many more parts as well in the same time frame' when in fact, no more parts would have been made in the same time.

The problem, was a glitch, or something off in the controls background. Verified by the manufacturer.
Nobody can see a different problem, except you.
And you can't explain what it is.
The only 'explanations' offered, have been incorrect.

The question asked, and advice sought was for this control, not a different one.
If the code works on this control, statements like ' the control would not read the G56 in this line', are patently false.
It does indeed read G56 in that line.
It reads the work offset just fine in that line, as evidenced by the fact that the program is still running, and further evidenced by others running the same code.
In case that wasn't enough evidence, I predict it will run fine again tomorrow.
Time will tell.

As far as I, the manufacturer, or anyone other than you can tell, I did nothing wrong in the programming.
The code works.
I have no problem admitting when I make a mistake. And have even stated that I changed my post to write future programs a little differently.
But those changes are simply for style, and standardization, NOT because this machine requires it that way.
It doesn't.
It ran that program 20 more times today, and will again tomorrow, and the day after...
Even though you have assured me that 'the control would not read the G56 in this line', it will in fact read it the next time I push the green button.
Just like it did the last time.

I've stated the things I don't know about.
No secret there.
Either state the HARM in having redundancies built in to a safety line, or get over yourself and accept that different folks do things different ways, and leave them alone about it.

My employees are free to work, or not work for me if they don't like me. They are paid well, their schedule is flexible when they need it to be, and they don't have me sweating them over nonsense.
I listen when they have ideas, and implement those ideas when they make sense. I'd wager that you've never heard a good idea that wasn't your own.
(...)

[burs]

Hello guys, please remember the netiquette in the forum, thank you. I will have to tidy up a bit in a few posts in this thread.

[HayreAss]

Hello guys, please remember the netiquette in the forum, thank you. I will have to tidy up a bit in a few posts in this thread.

It feels like you really should just delete my entire reply, since the post I am replying to was deleted.
Hell, the only actual insult that I made is still there!

[mactec54]

It feels like you really should just delete my entire reply, since the post I am replying to was deleted.
Hell, the only actual insult that I made is still there!

I'm not the one that sets how you want to Format your programing, your machine uses RS274D code standards is where it all comes from, all machine controls / manufactures use this standard here if an article which starts almost from the begging which has been quite well done, this has been presented by Autodesk, and Note the Code Format this is the correct way all code should be written, so it does not confuse the control of which action it needs to perform, can it be in written in other ways yes it can and most do write it different from this example, the problem with writing it in a different format is you never know when a single word of code is not going to be read correct, the machine will either just do nothing or crash, they call it a (GLITCH)

https://www.autodesk.com/products/fu...entals-g-code/

[machinehop5]

...Burs, please just close this thread and Mactec you need to see a Doctor.

DJ

[HayreAss]

No, they don't call that a glitch they call that an error, or a crash if it crashes.
A glitch is when it is NOT behaving as expected. Differently than it is presenting itself, etc...
As happened with my machine.
Like it or not.

An example would be when a machine corrects itself after clearing a work table, and re entering the exact same numbers.

[metalmayhem]

Where is it written that the offset call must be on a different line ?
I've worked on numerous controls in my career and not one ever required this . I spent 9 yrs working on a bunch of haas . I programmed almost daily with cam or hand code , and my lines after a tool change always started g0g90g54(55,56) x.. y.. s..m3 . Never had a problem because of this .

Unless this is something new from haas within the last 5 yrs then it's pretty common format straight across the board

[HayreAss]

It's not.
He just really, really wants it to be.

[extanker59]

Where is it written that the offset call must be on a different line ?
I've worked on numerous controls in my career and not one ever required this . I spent 9 yrs working on a bunch of haas . I programmed almost daily with cam or hand code , and my lines after a tool change always started g0g90g54(55,56) x.. y.. s..m3 . Never had a problem because of this .

Unless this is something new from haas within the last 5 yrs then it's pretty common format straight across the board

Someone may read this who needs information. Here is a sample of a part running as we type;

N22 (1 MM DIA. 4 FLUTE, CRB EM)
T22 M06
G00 G90 G58 X.028 Y.0985 S11000 M03
G43 Z1. H22 M08 T24
Z.1

This works. Other ways work as well. This is what I'm used to and will continue.
I wrote earlier that I omitted line numbers but I should have clarified that I asked our reseller post writer to add a line number to match the tool number. Makes it easier to get to the tool.
Also, the G43 Z1. is a safe height that we can visually verify before a crash. I've seen people go straight to Z.015 and I might if it was a long running repeat job. I once hand wrote a lathe job that needed every second to count so, after proving the program, I adjusted it to remove as much of the air time as possible.

Still, after all these years it's a fun job, isn't it?
I'd like to tell people to take it easy but sometimes that backfires on me.