FIXTURE OFFSETS

[BAD DOG]

I AM PROGRAMMING 50 PARTS ALL HELD IN 1 FIXTURE, EACH PART HAS 21 HOLES DIFFERENT DEPTHS.


I WANT TO DRILL ALL HOLES ON 1 PART THEN MOVE TO THE NEXT WITHOUT CALLING AN OFFSET.

THE PARTS ARE IN 5 ROWS OF 10 IN A PRECISION BUILT FIXTURE. PICKING TOOL PATHS ON EVERY PART ON THE C.A.M. WILL TAKE TO LONG.

I WANT TO AVOID THE RAPID TIME FROM PART TO PART.

ALL PARTS ARE THE SAME,,,, ANY SUGGESTIONS

BAD DOG

[fuzzyracing1967]

Not as hard as you may think, write a program to do one part (this will be the sub program),then just move in x-y to do next part and call sub program again.
So lets say you call right rear corner of fixture your part home,then you call out sub program and make the part,then when you go back to your main program you simply move in x-y.

example


G40 G49 T2 M06 (DRILL)
G00 G90 G54 X0 Y0 S500 M03 (PART ZERO)
G43 H02 Z2. M08
M98 P2 ( CALL OUT SUB)
(SUB PROGRAM)
G73 X0 Y0 Z-1.375 R0.1 Q0.3 F5.
X-.5
X-.6
Y-.5
X-.6
X1.1
M99
X-1. (MOVE TO 2ND PART)
M98 P2
AND SO FORTH

on your machine you may have a differant m to call out sub program or go back to main,this would be for a haas.

[HuFlungDung]

Sounds like a prime application for G52 Global work coordinate Offset shift. I'm not well versed enough in its use to say off the top of my head how its done exactly, but a search on the forum for G52 should bring it up.

[Mazaholic]

I think i would use a combination of both suggestions.
There is only a limited number of work offsets.
I'd give each row a work offset and then only move in one axis for each part in the row.

[Geof]

Sounds like a prime application for G52 Global work coordinate Offset shift. I'm not well versed enough in its use to say off the top of my head how its done exactly, but a search on the forum for G52 should bring it up.

Yes.

Put the main work zero, G54 for instance, at a reference point on the fixture; then the G52 coordinates are taken with reference to this location. The program would be something like this;

G54
G52 (X, Y for first part position)
Call subroutine
G52 (X, Y for second part position)
Call subroutine
etc
etc
etc
G52 (X, Y for fiftieth part position)
Call subroutine
M30

When the machine is setup for the job only the G54 coordinates need to be entered, all the G52's are in the program.

[Mazaholic]

Yes.

Put the main work zero, G54 for instance, at a reference point on the fixture; then the G52 coordinates are taken with reference to this location. The program would be something like this;

G54
G52 (X, Y for first part position)
Call subroutine
G52 (X, Y for second part position)
Call subroutine
etc
etc
etc
G52 (X, Y for fiftieth part position)
Call subroutine
M30

When the machine is setup for the job only the G54 coordinates need to be entered, all the G52's are in the program.

Well i'll be a...
I always figured there had to be a way to do that.

I've never had to run that many parts at once so i guess i never took the time to look it up.
I've always just used the G54 G55 G56 G57..ect

[Geof]

Well i'll be a...
I always figured there had to be a way to do that.

I've never had to run that many parts at once so i guess i never took the time to look it up.
I've always just used the G54 G55 G56 G57..ect

Took me a while to get clued in, but now we use G52 extensively. So far the maximum number of locations I have done is 32.

What I find very convenient is when I am making a fixture that will hold several parts I can use the G52 coordinates for machining the fixture, and these are the same coordinates that go into the part program.

Conversely, with some of our older fixtures that were made in a hurry and are not very accurate, I can dial into the specific part location and determine the G52 coordinates that are correct for that location. This way I compensate for errors in the fixture.

[fizzissist]

If the fixturing places the parts in a consistent position and doesn't move...why not just simply program as though there were one single part with 1050 (50x21) holes? If you know the location of each part, then you know the location of the holes. Would make for a beautifully long program...

If you have macro capability and the part placement is uniform, just write a simple macro that shifts the fixture offset by the X or Y (or both) difference part-to-part.

Macros are great for family-of-parts where something is always changing and you don't want to have to keep rewriting the program.

One real handy one I wrote is for an O-ring groove. We do a lot of different size grooves, and I didn't like the way Mastercrash does them (and I got bored fighting it), so I now punch in a few prompted specifics like min/max and mean diameter, how deep/pass, finish allowance, cutter dia, an entrance angle for radius'ing the entry/exit, spindle speed and feed, and away it goes.

The nice thing about G52 like Geof & Mazaholic are saying is that the X,Y coordinates of each new location are right there plain to see in the program.

[beege]

Another way is using "macro modal", G66

G66P1000XaYb
XcYd
XeYf

Where P1000 => O1000, which would be the subprogram, including the G52
The "a", "b"... etc, would be the arguments passed to the G52 variables in the sub

[BAD DOG]

that won't work,,,because the drill drills at 5 different depths on one part,,,imagine holes at -.1 -.2 -.3 etc... deep I want to avoid all the rapid moves to each part. The way it is now all the -.1 holes are drilled in each part the machine then returns to the first and drills the -.2 holes thus it spends a lot of time in rapid mode.

bad dog

[BAD DOG]

sound like g52 is the way to go

bad dog

[BAD DOG]

right now the program is a long one because I know each parts location as far as I can tell the g52 will reset the sbroutine to the new x,y location so I can still use cutter comp.

Is there a g52 cancel or does the g54 at the beginning of the next subroutine cancel it.

bad dog