What's new
What's new

Mid program restart

Captdave

Titanium
Joined
Sep 24, 2006
Location
Atlanta, GA
Why does everything have to be so complicated :ack2: Manual says When in auto mode, F1 restart, enter block number you want to start from, set axis movement (this makes no sense), then OK. The program starts running from the begining with no spindle or motion.

Anyone have the short Mid program restart for dummies trick/tip?.
 
If your trying to start at a line number just search for the line number in auto mode. It will find the line, then press cycle start.

I usually only put a line number right before the tool change, so the TLO and work offset are called. Not sure how you would restart in the middle of a long cut.
 
I would say to use "Sequence Restart" function.
Select your line number or block number to start on, (They are NOT the same)
Select "Restart" on the F* keys
Type in the line number (N123) or Block number (86)
Press "Ok"
Then press "Sequence Restart" on the control panel.
The Jog feed will be used to bring it to the last point, and you are set.
Cycle start from here

This will ensure the spindle is running, coord. is selected, anything else in the program is executed.
 
I assume you are talking about your mazak captdave? I don't know how that works. On the Haas, you turn program restart on in the parameters, then simply select where in the program you want to restart. The control reads backwards (in the program) to find the correct work offset, tool number, and length offset. Not 100% how it is on finding tool as I have always done the restart with the correct tool already in the spindle.
 
If your on an okuma listen to Mr M, with okuma you can restart ANYWHERE, canned cycles, ANYWHERE. If your on a Mazak, wrong forum, lol
 
This is on a OSP 300 control.

For example here is a hypothetical situation, say one of the many features on the part is a pocket, after the completion of the program the pocket is measured and under sized. Comp the tool and now we just want to rerun the pocket op only.

On other controls we use this would be a simple task, pick the line number that includes the work offset prior to the tool change and the line number at the completions of the op. These are considered start and end markers and the rest of the program will be ignored till the markers are removed.
 
I would position your tool so you have a "line of sight" to the pocket, do the above described method, and then just stop at the optional stop after the tool
 
I would position your tool so you have a "line of sight" to the pocket, do the above described method, and then just stop at the optional stop after the tool

This.
Just make sure you have a clear path to the cut.. because it's going to move in ALL axis at the same time to get to its destination.
 
This isn't exactly a specific answer to your post, but I've started making this standard procedure on all my non-Fanuc control programs...

O1234 (MAIN MACHINING PROGRAM)
(SPOTS, DRILLS, TAPS HOLES, THEN MILLS POCKET)

GOTO 10 (TOOL 1 - SPOT HOLES)
GOTO 20 (TOOL 2 - DRILL HOLES)
GOTO 30 (TOOL 3 - TAP HOLES)
GOTO 40 (TOOL 4 - ROUGH-MILL POCKET)
GOTO 45 (TOOL 4 - FINISH POCKET)

N10(SPOT HOLES)
Machining code goes here...
M1

N20(DRILL HOLES)
Machining code goes here...
M1

And so on....



On an Okuma control, you must be on the "Actual Position" or "Main Program" screen. Cursor down, and select the GOTO_ line that you want. Hold the "INTERLOCK RELEASE" button, and press CYCLE-START and you're off...
 
So on the P300 control, from the maim program page, use number search. Type in the line number (N18540) and you can see the start marker move to that N number, with a direct path to the start point hit cycle start. Tested it with several types of cycles within a program and works perfect.

Aren't Saturday afternoon great for this stuff, nice and quiet and no pressure to get it done now.;)
 
So on the P300 control, from the maim program page, use number search. Type in the line number (N18540) and you can see the start marker move to that N number, with a direct path to the start point hit cycle start. Tested it with several types of cycles within a program and works perfect.

Aren't Saturday afternoon great for this stuff, nice and quiet and no pressure to get it done now.;)

Yep, that's for Number Search... you can also do a Restart anywhere in the program.. just hit Restart and then Sequence Restart..... use the Dry Run feedrate to let ALL axis' move to the position and then hit Cycle Start.
 
Yep, that's for Number Search... you can also do a Restart anywhere in the program.. just hit Restart and then Sequence Restart..... use the Dry Run feedrate to let ALL axis' move to the position and then hit Cycle Start.
Yes, CaptDave, that will not activate any modes before that line in the program. I use it sometimes but prefer actually using the "Restart" F key and the "Sequence Restart" on the control panel. Much safer that way. Glad you are making progress!
 
Yes, CaptDave, that will not activate any modes before that line in the program. I use it sometimes but prefer actually using the "Restart" F key and the "Sequence Restart" on the control panel. Much safer that way. Glad you are making progress!

When testing I started the program at the tool change line to pick up the offsets and M codes.

IIRC correctly, the restart key had you search for a block number as opposed to a line number or am I missing something. The way my CAM is setup it only outputs line numbers only.
 
Block Number OR Line Number. The block number is displayed in the upper RH corner of the "Program" display IIRC. I generally just use line numbers to start on though
 
Wow that all sounds like a royal pain in the ass! I guess if you are familiar with the control (I have never used one) maybe it is easier to do than it sounds? I like the Haas way, turn the parameter on, rerun wherever you like. BUT, that has some drawbacks too, forget to turn it off and your programs slow way down as it is looking for the "correct" offsets and such, even if it is at the beginning of the tool with everything called up.
Question, can you page thru the program to a certain tool and just start at the toolchange line? The Haas, and I think most Fanuc do this with no parameter change or special sequence. I was referring to in the middle of a tool cutting you have to turn this feature on. If you want to start at a toolchange line you just page down to it and hit cycle start.
 
You can do both methods and it needs no parameter change. Just hold down "Interlock Release" and hit the green button
 
Like he said, not a pain in the ass at all, it actually relieves alot of worry knowing the machine will take care of all the worry, as long as you maintain that "line of sight". Ive bounced back and forth from fanuc, siemens, and osp for years and ive always been on the fence, but im finally convinced osp is the best(for me) it feels like the control works for me, the others make me feel like i work for them. Plus tons of memory and easy editing. I cant believe how many fanucs dont have "ex-edit", how is that not a basic function? Mid auto manual and sequence restart are the best functions ive ever seen on a control. I like the others dont get me wrong, but i prefer osp.
 
I'm not sure if this was mentioned yet but if you restart at a line number BE WARNED that the line number is observed by the control in 2 different ways....
Say you have a long program, N100 Facemill, N200 Pocket, N300 Drill etc... If you start the program from the beginning, by the time you get to N300 you may be on line 475 (just a number for example purposes). BUT.. if you Number search from N300 you will be starting at line 1.

This can benefit you or hurt you if you're not careful.
If you have a super long program, you can Number Search to N300 so it's faster AND THEN restart at a line number so you don't have to wait for the control to read from the very beginning of the program. But if you do it this way, your line number starts at 1 from N300.

Hopefully you can follow my gibberish explanation.
 








 
Back
Top