Re-starting program in the middle on a Haas TL?

Hi!

Somehow, I don't get it.
Say I do have a CNC-program with 3 tools. After tool #3 is finished, I see that I do have to tune the offset a bit to get to size. How do I start the code right at the tool #3? I only get errors like "x-axis overrun". Does the code have to have some prerequisites to work? Some parameters to set?

Other related question is:
A tool makes to certain shape divided into several parts. How could I just let re-run one part of that shape? I already got so far to place an M00 at the end.


TIA,
Nick

Setting 36 (Program Restart) will allow you to perform both actions but enabling this setting is very tricky. This setting will allow the control to run everything above the line you are starting on; this will load all of the offsets, cutter comp, and G-codes that should be active. If you are unfamiliar with this setting, use extreme caution and disable the setting after using it.

Nick

As Ken has stated, the Program Restart setting would allow the lathe to examine the entire program, run it in memory and it would pick up the motions right at the block you've specified.
Unfortunately, on the lathe this might lead to some unwanted ( and freakin' scary) motions. On mills I have this turned on and is flawless, but not on the lathes. It has scared the living daylights out of me a few times.

With that said tough, it is very easy and reliable to start a Haas ( or Fanuc for that matter ) in the middle of the program as long as your toolcalls are properly defined.
Perhaps if you could post your entire code we can figure out what and why is happening.

Ah, I missed the answers, so it took some time for this one ...

Thanks, setting 36 was off on mine. But as you warned me, I'd like to be educated too, before I get freakin' motions.
My basic understanding is, that if I re-start the program at a reasonable place, the interpreter goes back and collects missing information like Txx, G54, Sxxx, M3, M8 etc. and then starts working.
So what "freaking scary" motions do I have to expect? I hope it doesn't make some random G0 just for fun.

What do I have to expect?

But I'm aware that it might require some planing ahead where to re-start.

There is no specific code, it was more a generic question. It came to my mind in the following situation:
I need to make a highly precise dimension. The QCTP isn't precise enough (albeit it is a Multifix). So I need to tweak the tool offset a tad to get there for every part.

My solution now is (and that worked good enough):
Cut to say 39.0 mm, retract tool and have a M0 to stop the program so I can measure. Adjust the tool offset and then have a complete block (Txx G54; G96 S200 etc.) providing enough information to start right there (after the M0). Then finish to 41.005 mm (with the same tool and parameters of course).
What I didn't like is, that I have to maintain parameters (F and S) at two places. So I was looking for a more elegant way.

Rethinking that, I realize that I don't need to re-start, I just have to hit cycle start after the program halted at M0 and I did my adjustments. Right? <scratchingMyHead>


Nick

Just wondering what tolerance are you trying to hold?

Athack

Just wondering what tolerance are you trying to hold?

Click to expand...

+/- 3 µm.


Nick

Nick

My tool calls are always specified as this:
G00 G97 T101 S600 M03
G00 Xstart Zstart
G96 S300 M08
rest of the code


This is true in all normal tool calls or if there is an M00 or M01 for the purposes you're attempting.
About the only time I don't specify the details with a toolcall is if I'm only switching an offset number for the same tool. Example would be a groove tool with dir 3 and dir 4 offsets.
If you specify the calls as above, then you're always safe to put the cursor on the G00 G97 TX0X ... line and restart from there as long as you're in G54. If not, then just put the G5X in the same block as the toolcall and then you're set.

Thanks Seymor, I got the pattern. I wasn't that much off
I always use G5x in conjunction with a Txx.


Nick

If you want to restart the program in the middle of the program, I'm pretty sure you can do it by putting the program in graphics mode, and then single stepping through the program until the point that you want to restart.

At this point, check that the tool is correct, press "current commands" and then hit the green button.

What I usually do is program an M00 like you, take measurement and decide where to start again. To start, hit reset and then scroll to position you want to run again or scroll to next block after the M00 and push cycle start.