G53 Machine Coordinates and G90 / G91

[Donkey Hotey]

I had a problem today that really stumped me. I'm dealing with a new seat of Mastercam and their latest Haas post. It seems that one setting or another seems to be using G91 after an operation. Being modal until the next operation, is what caused me the problem.

When I am building programs in Mastercam, I do manual entries like the following for part flips:

G53 X-30.0 Y0.0 Z0.0
M00
(Flip part against back jaw)

The idea is to position the table up front, where the operator (me) can change the part and restart. Now the problem:

I ran the program and for some reason, it was sending the table to the upper right corner of the cabinet at every one of those entries. Today, I moved the vise and the same program suddenly had an 'X travel' alarm.

That pointed to some kind of relative referencing problem with G90 vs G91. That did turn out to be the problem It was taking my G53 move and interpreting it in relative coordinates.

And finally my question to all of you who knew this and are laughing at me: WTF would I ever do with relative machine coordinates? I mean--seriously--if I want to move up 10" in Z, I sure as heck don't need to declare G53 to do it. I can stay in my current work system and just call the machine move. What difference would G53 make?

A machine coordinate is machine coordinate. What have Gene's software guys been smoking or what obvious use have I obviously overlooked for using relative machine coordinates?

[colton_m]

Well there is one logical possibility,

If you had an extremely long tool and wanted to dodge clamps when sending the table towards the door for a part-flip...

Technically you could call the machine co-ordinate system, then select g91 and move the table to the left or right in X to a safe distance (without doing any math). then add a g90 and send y to 0 (bringing the table towards the door.

G53 G91 X3.0 G90 Y0.

I agree with you though it seems strange

[Donkey Hotey]

Originally Posted by colton_m Technically you could call the machine co-ordinate system, then select g91 and move the table to the left or right in X to a safe distance (without doing any math).

I don't need G53 to do that move. That's my point: a relative move is a relative move, no G53 required.

[Geof]

To some extent work coordinates, G54, 55, etc., are irrelevant when you are in G91 incremental mode. If your machine was in G91 and you had the command G54X10. Y10. Z10.0 you would not be surprised if the machine simply made the incremental move. Why should you be surprised if it behaves the same way when you specify G53 while in incremental?

[Donkey Hotey]

It bothers me because I don't consider it a work offset. It's a commanded, machine position. Again: what use is there for an incremental machine coordinate?

I'm stumped because some programmer at Haas had to decide how G53 would behave in the code. I see an advantage to it always being non-modal machine coordinates. I don't see any advantage to incremental. What am I missing?

[Geof]

Originally Posted by Donkey Hotey It bothers me because I don't consider it a work offset. It's a commanded, machine position.....

I think you are looking at it wrong; but then again maybe I am because I am currently in New Zealand with an upside down view.

G54 is a work coordinate system that uses a position defined by you in machine coordinate. You have no problem with making an incremental move when G54 is active.

G53 uses the machine coordinates as the work coordinate system; no different than leaving G54 at 0.0 for all the axes. The machine treats all work coordinate systems the same with respect to incremental moves; i.e., it does not use them, it just does the incremental shift.

P.S. don't expect another immediate reply, I am going offline to take in my washing and get ready for dinner.

[Ydna]

The main case where I use G53 is specifically in incremental situations, but it's not actually something that *couldn't* be done using a G91 incremental code instead. In my case I'm calling a number subroutine (0 through 9) for serial numbers based on a macro that increments for each part. I move the G53 over by the width of the number for each digit....but the only reason I do this though is because I originally posted the number code in G90 absolute and haven't gone back to re-post each of the digit programs

I could think of reasons to use G53 in some manually-programmed cases but ultimately I think it's just another way of doing the same job by coming at it from a different angle (figuratively).

[ach59]

I think if you just use
G90G28X-30.Y0Z0
you will get what what you want

[Donkey Hotey]

Yeah, there are a dozen ways around the problem but, the fact remains that there is no valid use for relative G53 addressing.

"What is your address?"

"Three houses from the corner."

"No, what is your mailing address?"

"North of the big brick house."

"How about GPS coordinates?"

"On which planet?"

Your address is your address. In a CNC machine, a machine coordinate is a machine coordinate...period. That's how G53 should work.

It's been a learning experience and a disappointing one at that.

Now if I could find out why/how Mastercam is inserting that stupid move, I could kill it. On a VF-5XT, when it goes home, the table is off on the left side of the cabinet and the left vise is completely inaccessable. That means I have to manually edit everything that comes out of Mastercam.

[Ydna]

You might be able to find the code in the Masterclam post script. Not sure if you have experience with that before, but some codes are in the script but others are buried in the actual "operations" that can't be edited. It might be worth a look though.
If you send me the post I can give it a whirl if you don't want to bother. I only say that since I've never ran into that with any of the posts I use....I'm kinda thankful too

[Donkey Hotey]

I took a 5-minute look through the post and came up with nothing. I'm going to dig deeper next week. Thanks for the offer, though.