Newbie- New to mazak programming, offset question

[trickhat]

I am new to mazaks, and programming for them. We just inherited 5 horizontal machines, and they are unlike anything else we have in shop. So far, we've gotten along pretty good, but as we learn more we're finding things that could/should have been done different over the years, and we're trying to update some of these things.

One of our ideas includes subprograms, and the use of the [offset] command in the mazatrol programming. We are using camlink to program offline, and I was hoping the offset would shift all the following patterns from the current WPC by that amount, but the preview doesn't show what I expected it to do. Instead of having 3 holes, each offset 1/2 inch (just a test to see if offset did what we hoped), it shows all 3 in the same place. Can anyone tell me what this command does? My searches just turn up general information on how to find fixture offsets, etc.

Models, controls are (HTC-400, M+), (FH-580/40, M+), (FH-4000, M64), (H-500/40N, M32), & (FH580, M+). I appreciate any help.

[jimiscnc]

There may be a possibility the TOOL PATH CHECK you're using does not accurately reflect fixture offset shifts by program.

a check would be to write a abbreviated program example for one hole 4 times 90 degrees. compare the tool path check with the air cut and TRACE DISPLAY while in the air cut.

if matrix, virtual machining may show tool path more accurately than tool path check.

Your problem is probably more a limitation of the display, which doesn't do a robust trreatment for compound angle tool path display and multiple program zero shifts, especially angular. In other words, it will display tool path from one view only and can't follow any rotary shift in the fixture offset.

-jim

[mbi]

Sub programming is very simple once you get the hang of it. First think of a sub program as just another program you can offset and/or rotate. This is how I make a Mazatrol program with a subprogram.

Main program starts like this:

unit 1 .....WPC

unit 2......mms

unit 3...... offset and rotatin if required

unit 4...... subprogram number ( don't worry about the aurgment lines)

unit 5..... Offset and rotation if required

unit 6..... Subprogram number (repeat your offset and subprogram units as much as you want)

unit 7..... Offset back to zero and continue on programming in your main program.

Make a new program (subprogram) start with whatever machining unit you want to make. Program it at zero on the x and y locations. Go back and type in the locations in unit 3 of your main program. This will shift your program to that location. You must put a 1 in on the continue line in the bottom of the sub program. This will allow the sub program to loop into the main program.

Type in the new program number in unit 4 of the main program.

Repeat the process for each subprogram. Caution once you have ran your last subprogram you will have to offset back to zero. You can put as many different sub programs in a main program as you want and you can even put sub programs into sub programs if you want to. This is called nesting. The subprograms will read your original wpc in the main program. You can also use priory numbers if you want. They will jump in and out of subprograms.

If you are programming a horizontal you must make unit 1 an index unit set to zero. This will allow you to run the main program and have automatic indexing in and out of the main or subprograms.

[trickhat]

Thanks for the replies! It's been very helpful, and now we have the framework set up to start updating the old programs.