What's new
What's new

Haas "Run from here"

Tryhard

Aluminum
Joined
Oct 26, 2019

Not sure if my terminology is right, but I've used this function on other controllers. Just that nothing jumps out at me on the Haas keypad for this type of command. Not sure if it even exists on my controller.

Does anyone know if it is possible to do a "run from here" on a Haas VF non-ngc classic controller? As in scroll down to a particular section/tool change and continue where you were interrupted on a long run program. If so, how?

Need to be able to do this after a tool change fault or broken tool replacement.
 
Its setting 36 on both control versions, NGC and preNGC, its called PROGRAM RESTART.

Turn the setting on and you are good to go, you can start from any line, you can even start with the wrong tool in the spindle, wrong wcs, it reads program from the begining to the line you choose, and it will force wcs change and tool change if needed.

Sent from my SM-G965F using Tapatalk
 
Its setting 36 on both control versions, NGC and preNGC, its called PROGRAM RESTART.

Turn the setting on and you are good to go, you can start from any line, you can even start with the wrong tool in the spindle, wrong wcs, it reads program from the begining to the line you choose, and it will force wcs change and tool change if needed.

Sent from my SM-G965F using Tapatalk

Thank you. I'll check it out!
 
Just a caution, the machine will move to the last XYZ position before the line you choose to restart at.
 
Its setting 36 on both control versions, NGC and preNGC, its called PROGRAM RESTART.

Turn the setting on and you are good to go, you can start from any line, you can even start with the wrong tool in the spindle, wrong wcs, it reads program from the begining to the line you choose, and it will force wcs change and tool change if needed.

Sent from my SM-G965F using Tapatalk

My setting #36 was turned OFF.
Turned it on and worked just fine. Afterward, I also tried same thing with it turned off. Didn't think it would let me, but it started up. I cancelled it out quickly not certain if the machine still had the program start routines in memory.

Wouldn't think it's a good idea, but has anyone tried continuing a program without the "Program Restart" turned on?
 
I program with a "safety line" at the beginning of each tool. I restart at the beginning of a tool all the time without "Program Restart".

Program Restart is mostly for restarting in the middle of a tool.
 
I program with a "safety line" at the beginning of each tool. I restart at the beginning of a tool all the time without "Program Restart".

Program Restart is mostly for restarting in the middle of a tool.

On Haas machines you can start (without program reset enabled) at any tool change line without issue. As booze said, it is mostly for restarting something like a long surfacing program or such...
 
I don't know how big your programs are, but here's a little trick that may or may not be of use.

Say you have an endmill that does lots of roughing. Hundreds of lines of code.
Your endmill breaks somewhere in the middle of the program. Hit Feed Hold. Do not hit Reset yet.

Setting 31 - Reset Program Pointer: Turn this OFF.

Now hit Reset. This will not reset the cursor to the beginning of the program. The cursor will stay on the same line it was on when you hit Feed Hold.

Now you can go into Edit, insert a line no. (N1000), change your endmill, turn on Program Restart and restart where you endmill broke (N1000) without having to cut air up to that point.

Make sure to change all your settings back when you're done to avoid any nasty surprises.
 
Program will start from where your courser is in the program with Setting 36 On or OFF.

The difference is one Setting has the machine read through the entire program turning on or off Offsets, coolant, Speeds, feeds, puts the last Tool used, goes to the last position - then changes to the present Tool and starts from that SAFE programed position. Very good mindless Setting that avoids any complications...Only on Lengthy programs it can take awhile for machine to read through.

The other option is turn that Setting off and hit start. It runs the line its one with the tool and offsets that were last called up at the position its in. So if machine has a drill in a hole At X0 Y0 Z-2.00 and the line your on has a GO X3.3...the machine is making a Rapid move in to X 3.3. Could be a G90 or G91, no retract before move...spindle may be on..or not.

Great for long programs and you know Program can run from that point as all your settings are given after the Start is pressed.

Few of my programs are long enough to outweigh the benefits of having machine run through the program.


I had one gent turn the option off as he frequently started and stopped having to wait a couple seconds here and a couple there. He wanted to optimize the time. Unfortunately he would loose time when tooling took a short cut or coolant wasn't turned on or the P-cool didn't catch the count change. We had words and I changed back...the other issue was the other guys didn't know about the difference and just hit start. Not Good. Point is...set it up the way it works for you...but consider it something that needs to be across the board for all machines. Unless guys are assined to specific machines.
 








 
Back
Top