Newbie- Need help..M98 P...L...

[GJewell]

Any info would be appreciated in helping me get this set-up; I need to run multiple parts of the same geometry. (sometimes 100, 250 or more) Parts are very simple..OD x ID x cut-off.
Material is teflon or nylon. I have a program that was written to do this, but it is for older fanuc controllers. It uses G50 as home or toolchange position. From what I understand the HAAS GT-20 has to use G54. I programmed the older prgm in the controller and it will not work.. Being new to programming I am lost. Thanks in advance for your help.

[APP]

You don't have a book?


Basically you are going to put the same value that you use in the g50 line, in the offset of the tool. When you call the tool change, it picks up the xz value.


If you want to post the program, I could help you get through it.

[Geof]

Originally Posted by GJewell ..... It uses G50 as home or toolchange position. From what I understand the HAAS GT-20 has to use G54....

On the GT20, like all Haas, G54 is the default Work Coordinate system. I don't exactly get what you mean by using G54 for a tool change. You can move the turret home and one way to do that is G28. This is not essential because you only need to move far enough away from the work so that the next tool clears as it comes around. But the GT20 is so small it doesn't waste much time going all the way home.

The easy way to do what you want is to make your program into a subroutine which is called with an L count on the M97 line. We have many programs on our GT20 that operate this way. Like this:

O00000

Bunch of stuff

M97 P1000 L250

Bunch of stuff
G28
M30
----
N1000

Your program

M99

[GJewell]

Thanks for having a look at this. This is the subprogram that was used on the older machine. The X and Z dim. on lines with G50 are hypothetical. The X and Z there would normally be where the turret goes to for tool change. On this machine we would want it to go home (I think) due to the short Z travel. Also, If you could show me the correct structure for the main program that would call this one, would be appreciated.



(SUBPROGRAM FOR O00004)

(ID)

T0400S500M03

G50X1Z.1

T0404

G00X2.5Z.1

G01Z0.0F.004

X2.032

X2.002Z-.015

Z-.075

G00X1.975

Z.1

X1Z.1

T0400

M01

(OD)

T0300S500M03

G50X2Z.1

T0303

G00X2.336Z.1

G01Z0.0F.004

X2.366Z-.015

Z-.050

X2.336Z-.065

Z-.107

G00X2.5

Z.1

X2Z.1

T0300

M01

(CUT OFF)

T0200S500M03

G50X2Z.1

T0202

G00X2.5Z.5

Z-.060

G01X1.950F.003

G00X2.5

Z.5

X2Z.1

T0200

M01

W-.108

M99

[GJewell]

I have just posted a subprogram that is used for making multiple parts of the same geometry. This program comes from a friend who has an older machine of different make. Would you look at that post and help me to modify it to work with the GT20?
Also, how would the main prgm be structured to call up the sub?
Thank you for any help you can offer on this

[Geof]

Here is an example of a program from our GT20 that uses two tools in subroutines and parts off two pieces per bar advance. You can load this into yours and put in some tool offsets for tools 1, 7 & 8, to make it run so you can follow it in Graphics.

Tool 1 is a stop and when Block Delete is on the program just moves the stop into position so the stock can be advanced to the stop at the start of a new bar.

After doing the two parts the program returns to Tool 1 and positions it for the bar to be advanced again.

This machine has a manual chuck and the spindle orientation command is to orient the chuck for getting the chuck key in. If you do not have spindle orientation you will need to delete this command