Incremental Datum Shifting

[99bluemoon]

Hi

Apologies in advance if my question has already been discussed in another thread.

I use mostly Heidenhain and all the programs have individual Datum Shifts in them. They very often have INCREMENTAL DATUM SHIFTS as well. These are contained within labels to allow reading back and forth. This system works very well for what we want.

We have a couple of Haas VF3 and use one of the 26 x available work co-ordinate areas to store the Datums. Currently, if I want another datum in the program I use another area etc.

My question is:

Is there a simple way to use the same procedure as the Heidenhain, ie Incremental Datum Shift, within my programs without having to use one of the 26 x co-ordinates? I will still want to swap around and read these values as and when.

I want to be able to read my main datums then incremental values several times within the job.


Thanks

[txcncman]

Do you have a Haas mill manual?

[Ydna]

Using G52 might do the trick. There have been some threads on it before, and the manual has some info too

[99bluemoon]

Using G52 might do the trick. There have been some threads on it before, and the manual has some info too

I have the manual available and any ideas/examples concerning G52 would be appreciated.

Thanks for any help

[Matt@RFR]

I have the manual available and any ideas/examples concerning G52 would be appreciated.

Thanks for any help

Do a search. There are tons of examples in earlier threads.

[txcncman]

On page 163 of my manual it says:

"G10 Set Offsets (Group 00)
G10 allows the programmer to set offsets within the program. Using G10
replaces the manual entry of offsets (i.e. Tool length and diameter, and work
coordinate offsets)."

I think this is what you are wanting.

[99bluemoon]

Do a search. There are tons of examples in earlier threads.

Thanks.

I have looked at a couple of examples and ideas and will try at work.


My program will basically be:

o00010
.
.
.
G54 (main datum value in offset page)
M98 P200 (milling info)
.
.
I WANT TO MOVE INCREMENTAL ON X BY SAY -100mm
M98 P201
.
.
MOVE AGAIN SAY INCRMENTAL -85mm
M98 P201
.
.

(moving job across bed)

G54
.
.
etc etc


I hope you get what I want. It may be bleedin obvious but I got to ask!

[txcncman]

Thanks.

I have looked at a couple of examples and ideas and will try at work.


My program will basically be:

o00010
.
.
.
G54 (main datum value in offset page)
M98 P200 (milling info)
.
.
I WANT TO MOVE INCREMENTAL ON X BY SAY -100mm
M98 P201
.
.
MOVE AGAIN SAY INCRMENTAL -85mm
M98 P201
.
.

(moving job across bed)

G54
.
.
etc etc


I hope you get what I want. It may be bleedin obvious but I got to ask!

From the Haas manual:

G10 L2 P1 G91 X6.0 {Move coordinate G54 6.0 to the right}

In your example would become:

o00010
.
G54 (main datum value in offset page)
M98 P200 (milling info)
.
I WANT TO MOVE INCREMENTAL ON X BY SAY -100mm
G10 L2 P1 G91 X-100
G90
M98 P201
.
MOVE AGAIN SAY INCRMENTAL -85mm
G10 L2 P1 G91 X-85
G90
M98 P201
.
(moving job across bed)
G54
.
etc etc

[Geof]

txcncman's is probably the only way you can do it incrementally but he missed an important point. At the end of the program you need an additional G10 command that moves the G54 X value back to the beginning.

If you move X-100. then X-85. at the end you have to cancel these by moving X185. at the end of the program.

I prefer to do this sort of thing using G52. The first move would be G52 X100. the second G52 X185. then to cancel these you need G52 X0.

[txcncman]

That is correct. I overlooked this point.

[99bluemoon]

txcncman's is probably the only way you can do it incrementally but he missed an important point. At the end of the program you need an additional G10 command that moves the G54 X value back to the beginning.

If you move X-100. then X-85. at the end you have to cancel these by moving X185. at the end of the program.

I prefer to do this sort of thing using G52. The first move would be G52 X100. the second G52 X185. then to cancel these you need G52 X0.

Thanks.

I have the book at home with me and basically figured this out.However, after reading the G10 commands at various points of the main program, will just entering G54 at any point just make that my current datum from thereon?

[txcncman]

Yes. G54 is modal.