HAAS DS30-SSY with M97 Looping

Good afternoon,
I am having a couple head scratchers with my DS30-SSY while attempting to run out a Macro Program I have made. The first thing I am curious about is when I press stop at any point in time and resume into the program I lose the loop counter. Does anyone know of a way to maybe manipulate this? The real problem occurs when an operator stops the program and starts the program again from the start. This resets the counter again at the value listed at the beginning of my code. I will post this code and would love to hear what anyone may think could be a quick fix here.

My second concern isn’t really with the DS30-SSY it more so falls on the programming software side of things however I am sure you can manipulate the Haas to run it how I am thinking. I am using an inserted drill to blast through the center of my part and coming back with that same drill to turn the ID to size. How would I go about offsetting my tool? The first OP wants to use the tool centerline and the second wants to use the corner. My thought was that I could change the actual X dimension in the code so that it is no longer cutting on X0. I am unsure if that is the best way to cheat your machine though. If anyone else has a good idea for this please let me know! Anything is greatly appreciated, thanks ahead of time!

Here is the start to my code where I am using M97:

O12345
M97 P1 L45 (Call sub-program O0100 – repeat subprogram 45 times)
M30
G20

(TOOL - 3 OFFSET - 3)
(DCLNL 12 4B INSERT - CNMG 12 04 08-PM)
N1 T0303

Set the Insert that is cutting the bore into another tool offset. Then call the tool with corresponding offset you set the tool to in the program.

Quote:

---

Set the Insert that is cutting the bore into another tool offset. Then call the tool with corresponding offset you set the tool to in the program.

---

Facepalm. I should have known that; much appreciation! Do you have any experience with the M97 and looping command? I am running a full bar at a time and producing 47 parts per bar; I just want to be able to stop the program and maintain its current loop count, but I do not know if that is something that is an option. Thanks again for the explanation on that offset tool set-up. With some things involving lathe CNC centers I am still green and mostly self taught so I appreciate that information!

I would think that within the loop you set a counter

#500=0
#501=45

M97 P1 L[45-#100] (Call sub-program O0100 – repeat subprogram 45 times)


(TOOL - 3 OFFSET - 3)
(DCLNL 12 4B INSERT - CNMG 12 04 08-PM)
N1 T0303

#500=#500+1


M99

Quote:

---

Originally Posted by rcs60

I would think that within the loop you set a counter

---

That's a really good idea, I could get away with that and put it directly at the top to act the same as the loop call-out and still be functional after an insert change or machine stop then I could have the counter wiped in the code after it sees my M30. Excellent idea! I will give this a try and see what I come up with, I appreciate that a ton!

if the M98PxxxxL[45-#501] Doesn't work
you could try this

N1(SET COUNTER)
#500=0
#501=45

N2
IF[#500GE#501]GOTO3
M98PxxxxL1
#500=#500+1
GOTO2

N3
M30

THE #500 WOULD RETAIN THE VALUE IF THE CONTROL WAS TURNED OF OR RESET
BUT WOULD HAVE TO BE RESTARTED ON N2

Thanks that actually worked excellently! I have it running and the Macro keeps track of it now. Thank you very much for the help on this! I apologize it took me so long to get back to you but I had to wait until I saw the parts again. Worked like a charm though!

you are welcome and i am glad it works for you