Changing tool diameter in the tool offset screen

[Donkey Hotey]

Man, I love threads like this. I had no idea what to use G10 for and now I've got all kinds of ideas. Thanks guys!

[Geof]

Originally Posted by Donkey Hotey Man, I love threads like this. I had no idea what to use G10 for and now I've got all kinds of ideas. Thanks guys!

Maybe now we should introduce you to G52?

[dapoling]

Originally Posted by dapoling Vern if you could post your code where this happen it maybe helpful as some program their tool prep and paths a little different then others. When you stopped the cycle of from running did you hit reset. When starting the tool cutting again did you start it from the very beginning or at least calling up the tool change portion of your code. When reading M6T1 this will also set your H and D active at this point. Some machine you can go right into a G41 with out calling up your D value as it is already active. Dave

Excuse me the H and D is called up when the G43 used with your H offset and when you make a move with a G41 or G42 called up with your current D offset.
However the H and D are modal.

[SeymourDumore]

Ok, just so everyone is on the same page.

T1 M06 calls nothing but a toolchange. Neither length or diameter offset is read in, only Tool1 is put in spindle.

G43 by itself does nothing. It does not call the current tool's length.
Neither does G41 or G42 call the current tool's diameter by itself automatically, but it will call the previous D value!!!

So. To properly make sure that correct offsets are used, I do the following.
Each and every one of my toolchanges are done in this strict format:

(TOOL DESCRIPTION)
T1 M06
G00 G43 H01 D01

This way immediately after the tool is put in the spindle, it's appropriate offsets are also registered.
This is the only place the H and D words are called. Nowhere else within the body of the program is D called again unless there is special need to adjust some dimension and a different dia offs. is needed for that tool.

Special note: For this to work properly, you must make sure that "Program Restart" parameter is set to ON!!!

[dapoling]

In a Haas if a H or D is not placed with the appropriate G code as G43 will use the last H Offset used, this also will happen in G41 or G42 with the D value (this is not common in any other machine that I know of).

Seymour the way you are calling up your H and D work just fine, although I think this has more to do with personal choice or company policy.

Case in point I have worked with companies that used more then one D value assigned to one tool instead of correcting their program or setup to use one D value.
Thus calling up the D in the G41 D1 X1. F10. and any subsequent G41 or G42 call up also contained the same of different D value.
Either way is fine and this falls back to the ease of finding the code you are looking for while first run or editing, you will know where to look in the program with out reading the entire program.

The only time I use Program Restart is to get a tool back into a cutting path if I was just to restart at the tool change I just leave it off. This again is a personal preference or company policy.

[SeymourDumore]

That would be correct. Note that I've said D is not called again, unless due to special requirement a diff. offset is needed for the same tool.

Besides the advantage of immediate display of the proper offset, anytime you need to change a tool to a different station, you need to only change it in one place, right at the toolchange.
Find/replace works wonderful, but still does not beat a single overwrite.

[duenow]

Originally Posted by Geof Maybe now we should introduce you to G52?

I love G52,I run the same set of step jaws & G52 is 0 on a 1/4" plate. Run a 1/2" plate & just set G52 .250 on Z. Also handy for X & Y.

[joehernandez]

can i get the machine to ingore the d-code offset

[Geof]

Originally Posted by joehernandez can i get the machine to ingore the d-code offset

G40 cancels tool diameter offsets and the machine will then ignore them until you program either G41 Dnn or D42 Dnn.

At the top of your program you should have a 'safety line' to cancel all offset values and set iitial conditions. We use G00 G17 G20 G40 G49 G80 G90 G98

[SeymourDumore]

Actually D0 works just as good without having to edit the code to remove existing G4x commands.
In fact you gotta specify D0 on a G12 or G13 block as it automatically calls the active D-word.