We are having trouble programing a bar feeder on an SL20. We can get the stock to load and the push rod to activate, but can not get the stock where we want it. Does anyone have a sample program that works that I can load and pick apart to see this thing operate?

we are just getting ours running too. on current commands page press page up until you get to the bar feed page. enter all your length #'s there. then jog the rod to push a bar flush with the chuck/collet face. go into mdi and enter g105 Q2. machine will push bar entered length on bar feed page. the end of my program just has a G105 in it, then the control references all your parameters on the bar feed page again.

look in your bar feed manual on page 17-18

We figured it out. We found the screen with all the variables. Also that you can use I J and K as over rides. It's pretty interesting to see the thing work.

OK I have an order of 5000 pcs for my SL10. part is 2.5 long from 1/4 inch alum. I face center and drill an1/8th inch hole about 3/4 inch deep na dpart it off. The initial push is set at .35. I face center and drill it. Call a G105 and push it 2.645. Dandy....
Now I got to push the green button 5000 times. How do I get it to repeat the 13 times for one bar?
Yes I have the bar length in the page and the number of pcs per bar in there as well. And THEN.....How do I get the thing to automaticaly load another bar so it'll just run the stinkin job??????
Can ya tell I'm just a tiny bit frustrated?

...Now I got to push the green button 5000 times....

Isn't that what you hire Green Button Pushers for? :D

Au Contrare'
That's why them Green B utton Pushers got ME!!!! So they can have work to push the green button for!
So what I got to do to make this thing run?

Au Contrare'
That's why them Green B utton Pushers got ME!!!! So they can have work to push the green button for!
So what I got to do to make this thing run?

Don't ask me...I was too cheeeeep to buy the fancy Haas barfeed and built my own.

Can't you put things into a subroutine that you call 13 times or something like that?

Well, Yea, I'm thinkin I can. But I've not done that before and thus have no idea how it's done....
Hence my question

Well, Yea, I'm thinkin I can. But I've not done that before and thus have no idea how it's done....
Hence my question

Something like this, there is stuff missing of course;


Program Name
Subroutine call M97 P1000 L13
Home axes G28
Stop program M30
------
N1000
All your stuff for doing the first push
Face and drill
Second push
Part off
M99

What this does is go to line N1000, runs through the sequence, push, face, drill, push and part off and repeats this 13 times.

This doesn't help you start a new bar and I have no idea how that is done. One thing I do know is that if you just let the stub end from the first bar drop out into the chip tray and you have a chip auger you may need a new one when it grinds itself apart on the bar stub.

If you like I can find one of our programs that does this subroutine stuff and post it. You could load it and look at it in graphcs to see the sequence.

That would be very cool.
So, if I understand you correctly, the program that calls "my" program is the "O" numbered program and the sub ("My" program) is labeled with a "P"?

That would be very cool.
So, if I understand you correctly, the program that calls "my" program is the "O" numbered program and the sub ("My" program) is labeled with a "P"?

No the "My" program is tacked on the bottom of the "O" program right after the M30 and starts with line number N1000. The command M97 P1000 L13 just says; "scan through this program until you find line N1000 and start from there. When you reach the M99 command return here and do it again until the L number has counted down to zero then return to the next line down".

P is just the label used on Haas, Fanuc uses O I think.

M97 is an internal subroutine call to an extension (subroutine) on the bottom of the program doing the calling.

M98 is an external subprogram call to a completely separate program.

Ahhhh....
Thanks, I'll go give that a try.

Ahhhh....
Thanks, I'll go give that a try.

You can also call a subroutine from a subroutine; we need to do this on some of our lathe programs that use the barfeed. You can have the subroutine starting at N2000 tacked on below the M99 in the first subroutine and then you can call this either from the "O" program or from the "N1000" subroutine. When the L count is not present of course the subroutine returns to the line immediately below the M97 and only does the subroutine once.

I have found sometimes that it is best to plot things on a piece of paper in a flow chart and describe to yourself what is going on; it can get confusing when you get past about 3 subroutines. But I have also found subroutines very useful because you can have shorter programs and you can have different tools using the same set of coordinates so if you need to edit you only have one place to change.

Geof
That worked nicely. Thanks

just set the initial push for your starting position. then figure your part length and cutoff. if you use a toolsetting probe then adjust your z+ probe offset setting.
then just put a g115 in your program.

I've recently had to work on our lathe for a bit, and I fought the bar feeder for a week. Always hitting the wrong Q code and sending it searching for a bar that doesn't exist...
Here's what I found works best for the way we run the servo:

G105 Q6 - use this after loading program and setting up everything else, punch in all numbers in the bar feed page. This will unload the feeder -- you still will have to manually remove anything in the chuck.

next:
G105 Q4 - use this next, it will sweep the tray, load a bar, measure it, then pushrod and end in V axis jog. His handle jog and bump the stock until it barely clears the jaws.

finally:
G105 Q2 - set jaw height: wil push out stock to spec. amt.

and thats it for setup, you're ready to run.

End of program should look like this:

%
o0000
.
.
.
G105 Q0;
M01;
M99;
%

That will loop around until your length has been burned up, or max parts.
Hope this helps.

Some got to it before I did .

Change the g30 at end of program with a g99 and it will run continuously.

No need for macro's of subprograms and other subprograms. I generaly do my set up with the g30 in place and change to g99 when program works flawlessly.

Swain