Haas Probing Question

[Mic6]

(moved to the correct forum)

Sup People, I'd like to preface this post by saying that I'm extremely green in the whole macro world, so with that said...

 

 

My part is a 1.5 square bar of 7075. It's held in machined jaws that hold it by the corners at 45° It's 48" long, so it's held in 2 vices. I rough/finish the first 24", open the jaws and advance the part to finish the second 24". What I'm trying to do is probe the Y wall and the Z floor so I can get as good of a blend as possible.

I went through the Inspection Plus book and pieced together some cycles. I've figured out how to pick up the Y axis successfully and the blend looks pretty good. I keep getting errors in the "Z" portion,

 

N25 G91 G28 Z0
G80 G49 G40 G20 G1
T25 M6 (Spindle Probe )
G0 G90 G54 X25. Y-.3
G43 H25 Z4.0 T21
G65 P9832 <------------------Probe on
G65 P9810 Z-.5 F60. <------Protected move
G65 P9811 Y0 S2<-------Probe Y wall
G54 Y-.625<--------Move away from wall to "Y" middle of Z surface
G65 P9810 Z-.75 F30.<-------Protected move
G65 P9811 Z-.89 S55<--------Probe Z surface.  Here is where I get macro statement errors
G65 P9810 Z4.0
G65 P9833
G91 G28 Z0.
G10 L2 P2Z.886(Raise G55 Z offset  blend clearance)

 

The G10 line isn't working how I want. How would I go about probing the finished floor, then from there put a +Z value to raise the Z offset back to my part 0, being the programmed cut depth. What I have now just wipes the Z register and loads the Z.886, which then gives me over travel errors. I'm using positive offsets. Any ideas?

 

You can see below the 2 surfaces I'm trying to blend. The right side is the previously milled surface.

 

 

 

[Joe788]

When you probe the floor in the Z axis with Z-.89 in the macro call, you're not setting the origin -.89 down from the part. You're actually telling it, "This surface is supposed to be -.89, if it's not -.89, adjust the offset by however much is needed to make this -.89"

 

You don't need a G10 line.

 

 

Haven't used the Inspection Plus Macros on a Haas, but I've used them quite a bit on other machines. What is the S55?

 

On Fanuc and Mazak machines it would be S1. to S6. for G54 through G59, and S101. through S.... for G54.1P1-P300

 

Also, always put a decimal after the S number.

[Mic6]

S55 is G55 that works.

 

Oh ok, so I should be doing a protected positioning move to Z-.8, then then take a hit on the Z surface? But once/if that surface is set to 0, I want to bring it up to .886(which is my programmed cut depth. I'm probing the floor manually and bringing it up now, and it blends oh so perfect. That what the G10 line was trying to do.

Thanks for the response Joe

 

edit: I suppose I could set my Z 0 at that surface, then change my toolpaths for the 2nd half to cut at Z0 and change me retracts accordingly...

[Joe788]

S55 is G55 that works.

 

Oh ok, so I should be doing a protected positioning move to Z-.8, then then take a hit on the Z surface? But once/if that surface is set to 0, I want to bring it up to .886(which is my programmed cut depth. I'm probing the floor manually and bringing it up now, and it blends oh so perfect. That what the G10 line was trying to do.

Thanks for the response Joe

 

edit: I suppose I could set my Z 0 at that surface, then change my toolpaths for the 2nd half to cut at Z0 and change me retracts accordingly...

 

In your program, what is the Z depth of the finish cuts? That's the number you want to have in the G65P9811Znnn call.

 

If you call G65P9811Z-.89S55., the next tool you bring in at G55 Z-.89 will cut at the exact same height as the surface you just probed.

 

Also, you don't need to protected position down to Z-.8 You can just call the 9811 from wherever, and it will keep going until it either gets to the surface, or travels past where the surface should be by a small amount.

 

If you want to add to G55 incrementally, just do:

 

G91G10L2P2Znnnn

[Mic6]

Finished cut depth is Z-.886

Instead of S55, I meant S2

 

I was running this code and it moved to position and probed Z and retracted, but it didn't change the G55 Z offset at all.

 

G65 P9811 G54 X23.265 Y-.46 F60.
G65 P9810 Z-.75 F30.
G65 P9811 Z-.890 S2  <------Put .890 so it would go past.  I'll change to Z-.886 and try again
G65 P9810 Z4.0
G65 P9833
G91 G28 Z0.

[Joe788]

You don't want to program it to go past the depth. It will do that on it's own.

 

Move the probe over the finished surface you're trying to match,

 

Then call this:

 

G65P9811Z-.886S2.

 

Make sure you've got a decimal after the 2.

 

That will move your G55 Z offset so that exactly .886 above that surface is Z0. When you take your finish cuts at G55 Z-.886, you'll be matched right to the probed surface.

[Mic6]

FTMW! Thanks a lot Joe. Works sick!

 

[Joe788]

[Mic6]

Probing Video

[Rocketmachinist]

So are you doing so many parts that using probe single surface would have taken too long?

[Mic6]

It's only 40 parts, but each one has to be milled,indexed, 2 surfaces probed, machined, flipped and

Done again. This way its cake. Machine, slide to next position, clamp, cycle start and the blends are

Perfectly feathered.