Hello,
I am working on a Stama with 840C controller and have the following problem:
Before calling L81, I have to start the first drill position in the main program (because otherwise the machine would start somewhere in the working space) then I call the rest of the drill positions in the subprogram.
My question: How can I program that all drill positions are in the subprogram?
So that I don’t have to preposition them in the main program.
With a Fanuc its possible with L0 (G81 z-10 r2 L0 )
So far i couldn't find out anything on the 840C and PA was no help either.
With best regards
Alexander
Thread: drill positions in subprogram
Results 1 to 4 of 4
-
06-27-2011, 09:55 PM #1
- Join Date
- Dec 2009
- Posts
- 31
-
06-27-2011, 10:25 PM #2
- Join Date
- Jul 2009
- Posts
- 249
hello Schura,
I have worked with a Stama before and I need to tell you that your plan doesn’t work there.
I don’t know if your write your programs in Stama in surface or parameter, like we did it. However even with the parameter programming it did not work.
The first position always comes from the cycle and in the cycle there is usually the call to the subprogram.
It doesn’t work in any other way!
If anybody knows more please let me know. otherwise I have to search for the stama programming.
Greetings from Barnim
Stefan<b><u><!--fonto:Comic Sans MS--><span style="font-family:Comic Sans MS"><!--/fonto--><!--coloro:#FF0000--><span style="color:#FF0000"><!--/coloro--><!--sizeo:4--><span style="font-size:14pt;line-height:100%"><!--/sizeo-->Ich weis nicht alles, ich lerne viel, <br />aber leider wird einem selbst das <br />lernen heute erschwert<!--sizec--></span><!--/sizec--><!--colorc--></span><!--/colorc--><!--fontc--></span><!--/fontc--></u></b>
-
06-28-2011, 08:15 PM #3
Junior Member
- Join Date
- Apr 2003
- Posts
- 220
Hello
Write R28=81
And in the sub program hold L=R28 or G=R28
I believe R28 is also the value that you take with the pitch circle for the drill cycle.
Extract from a program
R28=81 R2=2 R3=-15 R10=50
L110
%SPF110
( drill picture M8 )
G0 X20 Y85 G=R28
X45 Y146.1
X63.4 Y303.2
X15 Y341.1
X15 Y443.1
G80
Greetings Matthias
-
06-30-2011, 06:50 PM #4
- Join Date
- Dec 2008
- Posts
- 469
Hello
Write R28=81
And in the sub program hold L=R28 or G=R28
I believe R28 is also the value that you take with the pitch circle for the drill cycle.
Extract from a program
R28=81 R2=2 R3=-15 R10=50
L110
%SPF110
( drill picture M8 )
G0 X20 Y85 G=R28
X45 Y146.1
X63.4 Y303.2
X15 Y341.1
X15 Y443.1
G80
Greetings Matthias
Hello
That right what you say.
Start the position in the main program.
Call the cycle
R28=81 R2=2 R3=3 R10=2 (for example)
And in the subprogram define 1 start-up position again
X20 Y85
G=R28
And then the other coordinates,
G80 to deselect the cycle
This definition is also good for other drill or thread cycles.
G81=Centering
83= Deep hole drilling
G84=thread cutting
G85
G86
Alternative- spindle +rubbing cycle book
Greetings and success
Wokle1
Reply With Quote
Posting Permissions
