[laka]

Most machines i've ran will let you manually move around to different lines in a program once the previous line has been completed with Single Block on. Can't seem to figure this out on our Haas.

[Geof]

Never heard of it and I have had lots of Haas machines for many years.

I must say it sounds like a strange requirement. You mean you can jump ahead or back in a running program? What happens about all the operations in the blocks you have jumped past?

[HuFlungDung]

Setting 36 'Program restart' affects the way the control restarts a program. When ON, the entire program is re-read up to the point where you choose to begin. This simply ensures that all necessary positioning moves and miscellaneous functions have been properly executed.

Now, if you like to live in the danger zone, turn that setting OFF and be wary of what happens if the current tool begins to cut, perhaps not knowing what work offset should be used, what the tool diameter is (if comp was used), what the tool length is (if it was altered). Personally, I'd always begin from a tool change if I had this setting off, because I don't assume too much modality from one operation to the next. But there may be circumstances where you could use direct execution to your advantage. But I'd suggest that setting 36 should be turned back ON for day to day use, especially if more than one guy is running the machine, because we all carry around our assumptions

[laka]

Perfect, thanks!


Geof: This is actually very handy for many reasons. Say you bust a tool mid cycle and have to load a new one, you wouldn't necessarily want to re-run the whole program cutting air to get to where you had left of.

I used to use it many times when running a long cycle and stopping the machine at end of the day and starting back at the line number I left at. On our Yasnac machine, I would run the tool change line all the way up to the G43 line, and just page down through the program to where I wanted to start. You definately need to be careful, but it is a handy feature.

[Geof]

You phrased your question poorly, you don't want to move around you want to move down to a start point somewhere in the program. As HFD describes,yes, Haas does that. The one time Program Restart can give problems is when you are using G101 to mirror axes. Starting immediately below the G101 line can cause bad things to happen.

[double a-ron]

I leave 36 off and start from a tool change. Unless I need to start in the middle of a series of g83 holes.

[Black08Chally]

I'll put a GOTO666 in after all the start up lines, then an N666 where I want to pick up.....Make sure your initial Z is high enough to clear any XY repositions as it goes from the 'GOTO' to line 666. You probably will have to put a feed rate in on your first linear move after the 666 as well as sometimes it alarms out if you are relying on the first one after the startup lines.

[WallyL7]

I'll put a GOTO666 in after all the start up lines, then an N666 where I want to pick up.....Make sure your initial Z is high enough to clear any XY repositions as it goes from the 'GOTO' to line 666. You probably will have to put a feed rate in on your first linear move after the 666 as well as sometimes it alarms out if you are relying on the first one after the startup lines.

That sounds pretty sketchy. So, you just add in a N666 if you need to start on a specific line? then you erase it when your done? Setting 36 takes care of all of your adding GOTO stuff to every single program since it reads the program from the beginning...Interesting you chose the number of the beast though!!lol!


however, I'm with Double A-ron on this. I only turn it "on" if I have a legitimate reason to start in the middle of a tool. Otherwise, I start at the tool call, and all the modals are there with feedrates, etc...Leaving it on makes me crazy with all the extra time waiting for it to read the program, go to the previous position, or even load the last tool in(chair)

[Black08Chally]

That sounds pretty sketchy. So, you just add in a N666 if you need to start on a specific line? then you erase it when your done? Setting 36 takes care of all of your adding GOTO stuff to every single program since it reads the program from the beginning...Interesting you chose the number of the beast though!!lol!


however, I'm with Double A-ron on this. I only turn it "on" if I have a legitimate reason to start in the middle of a tool. Otherwise, I start at the tool call, and all the modals are there with feedrates, etc...Leaving it on makes me crazy with all the extra time waiting for it to read the program, go to the previous position, or even load the last tool in(chair)

I always use 666 since I can easily type 'N666' in edit mode, then hit arrow down and find if it is in the program. If I get a not found then I know if I forget to remove the 'GOTO666' line it will alarm out with 'GOTO P OR N LINE NOT FOUND' or something like that. It allows me to choose exactly where to run up to, skip ahead to and and remove when I'm done. Since 666 means evil, I don't let it exist in a program, and if I do find it, I investigate why it was put there.

[Geof]

That sounds pretty sketchy. ...

Could be less sketchy than simply turning 36 off because you don't want to wait for the machine to scan the program.

If you are reading in offsets and tool dias from G10 lines at the head of the program and 36 if off they will not be picked up if you scroll down and start anywhere below the G10 lines.

If you put the GOTO below the G10 lines they will be picked up before the jump.

Yes, No? Do I have it right or wrong?

I keep 36 ON, I am a patient and cautious guy.

[WallyL7]

Could be less sketchy than simply turning 36 off because you don't want to wait for the machine to scan the program.

If you are reading in offsets and tool dias from G10 lines at the head of the program and 36 if off they will not be picked up if you scroll down and start anywhere below the G10 lines.

If you put the GOTO below the G10 lines they will be picked up before the jump.

Yes, No? Do I have it right or wrong?

I keep 36 ON, I am a patient and cautious guy.

How is that method less sketchy than setting 36? It certainly is faster to turn it on and start from mid cycle when you need to than to ALWAYS add GOTO lines. Personally, it is a rare thing for me to have to mid cycle start, so for me to add it to every program would just add a lot of extra time...and to add it to even one program would take more time than turning on 36 and waiting for the machine to read through the program...just sayin.


Don't misunderstand, I get that we all have our little nuances and tastes regarding how we do things. I think if this works great for him, then he should run with it, but, I think the majority of users are better off with setting 36.



There is less room for error with 36. It always homes the -Z- axis first (which he even said you need to make sure with his method that you have enough -Z- clearance first - potential disaster if you don't)...So, being patient and cautious is only more necessary with that system.

I understand you are a patient and cautious guy, Geof, but don't mistake my - - - not ALWAYS wanting to wait for the control to read through the program when I am simply running each tool one at a time - - - for not being cautious.


You remember I ran your program on my machine a while back

[Geof]

I think the meaning I intended didn't come through in what I wrote so I will do it differently.

In declining order of safety (the way I rate them):

Setting 36 ON is safest and slowest; painfully slow if you have a load of 38 parts and want to restart the last tool on the last part.

Putting in a line number and a GOTO, with the GOTO after any essential commands that have to be read at the top of the program such as G10 commands. I would intermediate in safety and slowness because you have to do some editing and then remove it.

Setting 36 OFF is the fastest and riskiest if you forget you have stuff that must be read ahead of your start point. Also risky to have the machine in regular use with Setting 36 OF,F just in case you where looking at something down in the body of the program and then forget to hit Reset before Cycle Start.

Incidentally has anyone found that sometimes in a Restart on a program with subroutines the machine will hang up on a subroutine call.?

[spy008]

Ok, so you're running a program and your last operation is withe some kind of an endmill(or whatever) and it breaks so you want to replace it touch off and run the program from where you left off?

Well, if you have the line # where you want to restart then:

edit>N#(whatever the line # is)>(down arrow)>mem>current commands>cycle start


The machine will scroll thru the program til it reaches the line# you input and then start at that line#.

If you want to start w/a particular tool#

edit>T7(or whatever your tool# is)>down arrow>mem>current commands>cycle start

machine will skip down to your tool# then run from that point.


Is that what you were wanting to do?

[WallyL7]

You are pretty close, spy.

Your N# example is right. If you have a line with N### on it (somewhere mid cycle)...and you want to start from that line, with setting 36 "on", scroll to that line, hit cycle start, control reads entire program, and starts from that line. (actually starts one position before)

In your second example, Setting 36 would be "off" , scroll to a tool call (assuming all modals are called for each tool), hit cycle start, and that tool starts like it normally would have if it were just running through the program - but without the control having to read everything ahead of it.

If you leave the setting 36 on, the entire program gets read every time you start within the program.

[tc26]

One problem I've had with a setting 36 on restart is that cutter comp (g41, g42) often times causes the control to red light alarm with regard to the cutter comp.
This happens on programs that run through just fine when run from beginning to end.
I have contacted the factory about this issue and they didn't offer any satisfactory solutions.

[KenFoulks]

One problem I've had with a setting 36 on restart is that cutter comp (g41, g42) often times causes the control to red light alarm with regard to the cutter comp.
This happens on programs that run through just fine when run from beginning to end.
I have contacted the factory about this issue and they didn't offer any satisfactory solutions.

Where are you starting the program, before G41 or in the middle of a tool path? How old is your mill, do you know the software version?

I would also like to apologize for your unsatisfactory factory customer service experience.

[tc26]

We have four VF2SS. Software ranges from M13.12N to M16.09A.
I am restarting on a Z postion above the work.
X and Y have finished a pass and tool has moved to a Z postion above the work.
I try to restart at that Z position. Some times it will run, other times not.
Again these programs have no problem with cutter comp when run from beginning to end.
The factory advised me to add some extra x,y lines for the restart.
Not a good solution for what I consider a software problem.
I used to run old General Electric and Cincinnati controls that allowed the user to single block through the program and execute the commands that were needed, then jump ahead to the line to be restarted. I never had any trouble doing so.
Thanks for the reply.

[KenFoulks]

When you place the cursor for program restart, you are telling the control the first block you want to execute. In this case, the move to the Z position above the part. In order to execute program restart properly, everything that was true on the block before the block where the cursor is must be true. The machine is going to move to the position of the block before your Z move. If the coolant was on it is going to be activated again during the program restart. Once everything is the same as it was on the block before the block with the cursor, the control will execute the block you have chosen for restart. If you want to start running from the Z position, place the cursor on the block after the move to the Z position. Please try this and tell us if you continue to get the cutter comp alarms.

I understand how your old Cincinnati controls used to work. Haas will not be adopting this functionality.

[tc26]

Thanks, I will try that at the next opportunity.

[tc26]

Ken,
I tried what you suggested today.
It does not work.
Here is my program.
The end mills are 2" dia.
T2 has dia comp .008 in the tool data.
A restart on an XY move after a z clearance move results in a red light alarm.
Program runs through as it should when run from start to end.

%
O02222

( 8.6614 X 8.6614 )
( CORNERS .020 X 45 DEG )

( VF2 )

( X & Y ZERO TOP RIGHT CORNER )
( Z ZERO TOP OF PART )

( T2 2.0 DIA ROUGH )
( T3 2.0 DIA FINISH )
( COMP IS ON BOTH TOOLS )

( ROUGH )
G91 G28 Z0
G28 Y0
G0 G90 G54 X-12.4
T2 M6
M0
( !!! CLAMPS TIGHT ??? )

G0 G90 G54 X-11.9144 Y.731 M88
G43 D2 H2 Z1. M31
M8
S5000 M3
G41 X-12.0144 Y.831
G4 P3.
Z-.95
G1 X-9.7144 F4.
X-1.093
X1.907
G0 Z1.
X-11.9144 Y.463
Z-.95
G1 X-9.7144
X-1.093
X1.907
G0 Z1.
X-11.9144 Y.195
Z-.95
G1 X-9.7144
X-1.093
X1.907
G0 Z1.
( ROUGH )
X.755 Y.593
Z-.95
G1 Y-1.407
Y-10.0284
Y-12.0284
G0 Z1.
X.509 Y.593
Z-.95
G1 Y-1.407
Y-10.0284
Y-12.0284
G0 Z1.
( ROUGH )
X-11.4734
Z-.95
G1 Y-10.0284
Y-1.407
Y.593
G0 Z1.
X-11.3164 Y-12.0284
Z-.95
G1 Y-10.0284
Y-1.407
Y.593
G0 Z1.
( ROUGH )
X-1.4072 Y.7515
Z-.95
G1 X-.5587 Y-.097
X.217 Y-.8727
Y-10.5628
X-.5587 Y-11.3384
X-10.2488
X-11.0244 Y-10.5628
Y-.8727
X-10.2488 Y-.097
X-.5587
X-.1587
G0 Z1.
X-1.5149 Y.4915
Z-.95
G1 X-.6664 Y-.357
X-.043 Y-.9804
Y-10.4551
X-.6664 Y-11.0784
X-10.1411
X-10.7644 Y-10.4551
Y-.9804
X-10.1411 Y-.357
X-.6664
X-.2664
G0 Z1. M5
G40 X-.3664 Y-.457 M33
G91 G28 Z0 M89
G28 D0 Y0 M9
G0 G90 G54 X-12.4
M98 P2

( FINISH )
G91 G28 Z0
G28 Y0
G0 G90 G54 X-12.4
T3 M6
M1
G0 G90 G54 X-1.6273 Y.5615 M88
G43 D3 H3 Z1. M31
M8
S5000 M3
G41 X-1.5273 Y.4615
G4 P3.
Z-.94
G1 X-.6788 Y-.387 F4.
X-.073 Y-.9928
Y-10.4426
X-.6788 Y-11.0484
X-10.1286
X-10.7344 Y-10.4426
Y-.9928
X-10.1286 Y-.387
X-.6788
X-.2788
G0 Z1. M5
G40 X-.3788 Y-.487 M33
G91 G28 Z0 M89
G28 D0 Y0 M9
G0 G90 G54 X-12.4
M98 P2
M30
%