[VWbmx]

Hey everybody.
My company has a Haas VF2SS and I'm new to g-code and am wondering how to use a subroutine on a mill patern.

I'm trying to write a code for one mill patern about the origin and then move the mill patern using subroutines to 3 locations.

My question is:
How do I write the code? Absolute or Incremental?

Right now I have it writen in Absolute and I'm trying to move the subroutine in absoulte.
Something like this:

G00 G55 G90 X-1. Y0;
M97 P1000;
G00 G55 G90 X-.2 Y0;
M97 P1000;
G00 G55 G90 X.9 Y0;
M97 P1000;
M30;

N1000;
G00 G91 X0 Y0;
G00 Z.25;
G01 Z-.25 F10.;
G01 X-1. Y-2. F20.;
G02 X1. R1.;
G01 Y2.;
G02 X-1. R1.;
G01 Y-2.;
G01 Z.25 F100.;
M99;
Do I need to rewrite this Subroutine in Incremental?

Thanks in advance for your help!

[HuFlungDung]

Easiest way is to use a unique workshift for each location. Run the first part at G54, second one at G55, third at G56.

This makes it easy to adjust the datum of each pattern simply by studying the values in the offset register and adjusting the X and/or Y values to reflect how far the patterns are from each other.

You might also research the usage of G52, as this permits setting a datum at any point you like, then jumping to a subroutine written in absolute and the absolute code will regard the G52 as the absolute zero until it is cancelled. I call that an advanced technique because I have not used it myself yet

[Geof]

Write it in absolute and either use three work zeroes, G54, G55, G56 each located for the positions of three parts as Hu suggests or use G52 also as Hu suggests. It is six of one half a dozen of the other really; G52 sets a supplementary work zero with reference to your main work zero.

EDIT: Hu's reply wasn't there when I clicked on REPLY; obviously great minds think alike.

[VWbmx]

Thanks for the sppedy Sunday replies!!!

In the back of my head I was thinking I should use the different work coords.

I'll try that now and let ya know.

[psychomill]

On the flip side ,... there's nothing wrong with your original thought process of using an incremental sub either. You can simply position your pattern where ever you want based on one work offset. You don't need to keep calling the workoffset either. And you still maintain the same adjustability as G52 or other methods...

There are a number of ways to accomplish the same task... Hu's offset method allows to adjust from Work offset page. The others are updated by positioning in the program.. You can also set your positions to variables and simulate Work offset page function but that may be 'advanced' for now as well....

[VWbmx]

YES!!! That worked!!! I used G55 as the center of my part. In MDI, I moved over the distances to the center of each patern and called them G56, G57 and G58 respectivly in OFFSETS and ran the program in the GRAPHICS screen. It looks great!

Thanks again for your help!
Allan

[nabil_elbadri]

hi all , i just wonder about the sub rotine start (M97) ???
in the program that vw bmx already written!!!!!
as i know it should be M98 to call sub program , if there is another code (M code ) to call sub programme pls let me know
thnx all

[JWK42]

The M97 is a local Sub Routine call. The local sub is included in the main program and is located after the M30 and before the % at the end of the program file and always ends with a M99
In "M97 P1000" the P1000 is the first line number of the Sub as in VWbmx's example. This may be a Haas only feature. I don't know if Fanuc controls use local subs.

I like to use G97 local subs because all the code for a part is included in one file. It makes backup a lot easier.

[Geof]

hi all , i just wonder about the sub rotine start (M97) ???
in the program that vw bmx already written!!!!!
as i know it should be M98 to call sub program ....

It's a Haas thing. Very convenient as mentioned above you have all the code in one file. Haas also allows almost unlimited nesting of subroutines.

[psychomill]

The M97 is a local Sub Routine call......This may be a Haas only feature. I don't know if Fanuc controls use local subs.

FANUC = NO
YASNAC = YES
MAZATROL = YES
MITSUBISHI = YES

OTHERS= ???

Although it's not M97 on the other controls but the way it works is all the same...

[COOLSKODA]

im studying programming and just wondered how sub routine G97 for hass worked with rgards to drilling, i center drill, drill and ream several different holes. is this possible in sub-routine, if so how would it be inputted?

regards

[Geof]

I seem to recall I used M97 (I think this is what you mean but you typed G97) in a drill canned cycle.

I was spotting, drilling and tapping and had all the hole coordinates in a subroutine which I called after setting up the canned cycle.

I will play with one of my machines and see if it works I could be remembering it incorrectly.

EDIT: Yes it works here is how to set up the program (with some stuff missing of course).

Blah
Blah
Spot Drill
G82 Z-.2 F? R? L0
M97 P1000
G80
Blah
Blah
Drill
G83 Z-2. Q? F? R? L0
M97 P1000
G80
Blah
Blah
Tap
G84 Z-.2 F? R? L0
M97 P1000
G80
Blah
Blah
M30
N1000 All the hole coordinates
M99

Some things to note:

The L0 in the canned cycle command means that the machine does not perform the cycle until it reads the first set of coordinates in the subroutine.

SETTING 28; CAN CYCLE ACT W/O X/Y has to be turned ON so you can omit the X and Y coordinates in the canned cycle line.

[COOLSKODA]

thanks, i am trying to get my head round it, im looking at the hass booklet, what is confusing me the most is the z axis alterations.

[Geof]

thanks, i am trying to get my head round it, im looking at the hass booklet, what is confusing me the most is the z axis alterations.

Do you mean the ability to change Z in the list of coordinates?

This is possible on a Haas; you can drill to different depths at each location like this:

X-1. Y-1. Z-1.5
X-2. Y-1. Z-0.5
X-3. Y-1. Z-2.5
X-4. Y-1. Z-1.5
X-5. Y-1.
X-6. Y-1.
X-7. Y-1.

The last three holes will all be Z-1.5 because that is the last read Z depth. You could also omit the Y-1. if the Y coordinate does not change.

You can also change the work coordinate: You may want to repeat the hole pattern at several locations so you set up the canned cycle like my example and go to the subroutine and then change the work coordinate and go back

G54
Canned cycle
M97 P1000
G55 M97 P1000
G56 M97 P1000
G57 M97 P1000
etc
G80

[COOLSKODA]

thanks again, i have done it the work co-ordinate way, what you have just explained as backed up what i have done.

i am also struggle with g150 (general purpose pocket milling) again i am looking at the hass manual, and for the pocket a sub-program i used, but i can't see an m97 in their example, why is a sub-program needed?

regards

[Geof]

....i am also struggle with g150 (general purpose pocket milling) .... why is a sub-program needed?

regards

Because Haas says so.

That is one of the things you just gotta do; the pocket coordinates have to be in a separate program.

I think the G150 line is actually a macro call to a hidden macro, and inside this macro there is probably the M98 that calls the pocket coordinate program.