Need Help!- Offset Help Maybe?

[Doubleddaved]

Been using this Haas control (VF8/50)for about 1 1/2 weeks now and I still have a few questions.
I mainly drill tubesheets with hundreds of holes,when my drill needs sharpening or to be replaced is there a way that I can single block the program, raise the head, take the drill out, do what I have to do and reset the length offset,and take off right where I left off at?
Haas support says I can't do it,I would have to reset the machine,do what I have to do and then start over.
My Mazak with Fanuc control allows me to do that and it's almost 30 years old,I find it hard to believe that Haas can't do it.
Let me know if anyone found a way around this.
Thanks Again
Dave

[drewmeister]

insert a line number on that particular hole IE. n1. change the drill and search for n1. i believe that the control will read all the codes before the n1 like g43 g54 and h value. 5% rapid is your friend here!

[dapoling]

You will need to turn on auto restart and select the hole location and cycle start.
The auto restart will run through programing from the beginning with out table movements until just before the location you selected and will pick up from there.

With out auto start on it will take off from where you picked, which can be bad, raise you z up to clear all clamps and material or machine tooling.

[ltmquik]

On our HAAS we have tool management routines. You can set up multiple tools of the same size and tyep and set their offsets. Then you can tell the control to change out the tool at a set Spindle Load or number of uses. It will then pick up the alternate tool and start machining. I do not know if this function will work in the middle of a canned cycle.

You would have to do what the other person suggested. You can simply add line numbers to your code if you do not have them already and use the Edit and Search commands to forward to the point you left off at. I usually go one line lower in the code because the control reads and executes the line above the one the cursor is on. Again, set your rapid to 5% and Feed Off until you are comfortable with what you are doing.

[Doubleddaved]

I'm using a subroutine that has all the hole locations.Would I still be able to use restart using subroutines?

[dapoling]

To do what you want, you need one program and use program restart.
Is there some reason you need these split into different sub programs?
as posted in the other thread you are posting.
http://www.cnczone.com/forums/showthread.php?t=54493#6

[-Chris-]

Can you break your routne into several parts, a size of witch you know is about time for a sharp tool. program them each to a different tool station with the same drill size in it. If you have a 24 station turret you have a lot of capacity. -Chris-

[gar]

080318-1043 EST USA

Doubleddaved:

You need to provide more information:

What is a "tubesheet"? Is this a flat sheet? Are the holes in a regular pattern, or randomly located? Are more than one tool type and size used?

I do not use restart but use other techniques. However, if you are not doing loops, then I would expect that restart could work into your subroutine. This is based on the asumption that HAAS is simply reading all instructions up to the first encounter of the point where the particular line for restart is located. This assumes only one useage of a particular subroutine and maybe no nesting.

.

[Geof]

Originally Posted by Doubleddaved I'm using a subroutine that has all the hole locations.Would I still be able to use restart using subroutines?

You can Restart within a subroutine.

[Geof]

Originally Posted by Doubleddaved .....when my drill needs sharpening or to be replaced is there a way that I can single block the program, raise the head, take the drill out, do what I have to do and reset the length offset,and take off right where I left off at?......

Yes I think there is.

How many drills do you typically wear out in a cycle?

Take this number of drills and mount them in toolholders.

Put each one in the machine and set the length offset for that drill.

Make a record of the offset and keep that record with that drill.

Edit your program and after enough holes to dull the drill put in G53 Z0. to take the Z axis home and a M00 followed by a spindle restart and G43 H0n for the tool number of the drill.

Start the program with any drill and run it to the first M00.

Swap in a new drill and change the length offset value to the one you recorded for this drill.

Run to the next M00 and do the same.

etc.

etc.