New Guy with a Problem

[RaceCarbs]

First things first. New guy here. My name is Rick and I live in Tucson, AZ. I've been programming about 24 years and now I want to do something that I've never done before. I know somebody in here should be able to help. First, a brief overview of the situation. I have 8 pieces of material loaded into an 8 position Chick vise on an HS1-RP. Each of the 8 pieces will actually be 2 parts when finished and cut in half. The first op has been done and the parts flipped and reloaded. Now the catch. What I need to do is this. I want to probe the hole (reamed in the first op) in the center of the material, then move to the location in the picture marked G110 and have the probe set G110 then physically move to the G111 position and set G111 and so on with all 8 pieces using G110 thru G125. I can probe all the holes, I just don't how to use that to set all 16 datums automatically (or if it's even possible). Right now I probe the holes and then manually set the datums myself. Thanks in advance for any help you might be able to give me.

[Vern Smith]

Seeing you have a probe I'm assuming you have macros. A macro statement(s) can certainly be written to take the probed location and mathematically revise it into a new Gxxx location. The macro statement can also output the result into the offset table.

I'm not a macro writer but I know it can be done with macros. I'm sure one of the guys on the forum who write macro statements every day will come along shortly. Also, your Haas manual has a fairly large section devoted to writing macros and also tells you where the information the macro will need to make the calculation resides as well as what locations the computed offsets will need to be placed in. It also goes into any necessary settings changes that may be needed as well as the necessary G codes to call the macros and the related sub routines.

In other words, it's doable.

Someone will probably know a way to do it without macros as well.

Vern

[Geof]

Use G52, this seems to be a perfect application; G52 is a command that sets a secondary work zero with reference to your main work zero.

What you need is some way to locate your main work zero; you have the hole that you probe so make this your main work zero, call it Gmmm.

You know the distance(s) from this hole to your intended G110 and G111 locations and these are used in the G52 command:

Gmmm G52 X(distance110) Y(distance110) Z(distance110)

This command uses the Gmmm as a reference point and establishes the G52 secondary work at the point you want your G110.

The machine will continue to use this secondary work zero until you change either Gmmm or give a new G52 command.

To get to your G111 location all you need is another G52 command using the 'distance111' and a main work zero placed at the bottom hole.

Same for the other faces.

Actually if you make your main work zero in the center exactly between the two reference holes you can do it very easily. We have numerous rotating fixtures that consist of a base with a central hole that is used to locate a main work zero; anything up to 32 secondary work zeroes are then referenced from this using G52.

[dcoupar]

#5021 is the current X position (in the Machine Coordinate System), and #5022 is the current Y position.

#7001 is the G110 X, #7002 = G110 Y, etc.

You should be able to probe the hole, move to the G110 zero, and execute the following command:

#7001=#5201 (SET G110 X)
#7002=#5202 (SET G110 Y)

It seems like a waste of motion to actually move to the WCS Zero, though. You should be able to "do the math" in the macro.

[RaceCarbs]

Thanks guys for the help, but I'm still stumped. So here's what happened. I know I'm missing something simple. After several attempts the sample below came the closest. The results are this: I run this through once and it changes G110 and G111 both to exactly what I want in G110 only. If I run it again it changes them both to what I want in G111. From then on it stays with the same G111 results. I know how to tie it in with the probe once I get the results I need. This was simply a test. Thanks again.


%
O1234 (VARIABLE SHIFT TEST)
G00 G90 G40 G80 G49 Z0


G54 X0 Y0
G54 X-2. Y2.
#7001= #5021 (SETS X)
#7002= #5022 (SETS Y)


G54 X0 Y0
G54 X2. Y2.
#7021= #5021 (SETS X)
#7022= #5022 (SETS Y)

G49 Z0
M30
%