HAAS - How to probe at center everytime for each part automatically?

[Rubens]

Hi everyone... I need some help with this.

I have a few HAAS 3-Axis Mills (Sample of - VF2-YT, 2012) with Renishaw Probing System - and I'm trying to figure out how to probe my parts 'maybe' thru a sub-program prior to running my program so that I can come from the center of each part (or stock), without having to manually indicate that center everytime?

 

 

 

Thanks,

Ruben

[htm01]

use the has quick code probing cycles and you can add right into program

[Machineguy]

Its a little more then that.

I have a example, i'll get to it as soon as I can. Very busy right now.

 

Machineguy

[chris m]

As long as you have SOME idea of where the feature is that you would like to probe (part against a stop, bolted down through fairly precise holes, etc), this is pretty straightforward. Drop me a line, if you'd like.

 

C

[Rubens]

Thanks for your response you guys... Cant wait to get that sample Machineguy.

 

 I know how to work the most probing cycles on the controller, even to probe coming off the center of the stock or center of a hole. Sometimes we need to come off a DATUM which would be on the center of a feature (Aerospace), so if I have multiple parts to run I would like to set up the program so that it can indicate the center for each part (because each part might just be a little different in size), indicate by just pressing Cycle Start, w/o me having to run thru the probing cycle manually.

 

 I've seen this be done before in another company by an operator I had back then. I just did not get around to asking the operator at that time how he set that up. Not sure if that is a Haas Probing Cycle that I don't know of but is available in the cotroller, or if one has to create and wright a sub-program to make the Mill do that at the beginning to every part prior to running my program.

 

 

 

Ruben,

[Machineguy]

The following should work  from a 2010 HAAS machine  to now with the renishaw probe.

 

Run the probe first to set G54 or whatever work coordinate you are using. DO THIS FIRST !

 

Next, you put this at the beginning of the program. Change the G54 to what you are using. 

 

(PROBE BORE-VQC)

G00 G40 G80 G91 G28 Z0

 

G103 P1 (LIMIT BLOCK LOOK-AHEAD TO 1 LINE)

 

T24 M06 (CHANGE TO SPINDLE PROBE TOOL #)

 

G65 P9832 (TURN PROBE ON)

 

G43 H24 (TOOL HEIGHT CALLOUT FOR THE PROBE)

 

G00 G90 G54 X0 Y0 (CENTER OF BORE TO CHECK OR SET)

 

G65 P9810 Z1. F200. (PROTECTED Z MOVE)

 

G65 P9810 G01 Z-.3 F50. (LOCATION OF Z INSIDE THE BORE WHERE YOU WANT TO HIT)

 

G65 P9023 A1. D2. S54. (PROBE BORE MACRO PROGRAM SET G54 D= DIA) 

 

G65 P9833 (TURN PROBE OFF)

 

G00 G91 G28 Z0 (PROBE GOES HOME IN Z)

 

G103 P0 (ENABLE FULL BLOCK LOOK-AHEAD)

 

(CONTINUE ON WITH YOUR PROGRAM HERE)

 

 

Make sure you have nothing in the way of the probe body!

The probe is in protected mode when entering the part. THE BODY IS NOT PROTECTED!

 

This works as long as the bore you are setting hasn't moved more then about .200 from when you initially set the Work Offset.

If you change Diameter, change it in the above program also or you will get a error.

Run this carefully the first time so you see how it works.

 

Machineguy

[Machineguy]

One more thing.

Make sure the probe # and the H # are changed to whatever you are using.

[Rubens]

That's perfect.... Thanks Machineguy, I really appreciate you taking your time to do this!    

[Mic6]

I have a bunch of text files saved and insert them as Manual toolpaths and edit the cycle according to the part.  

 

Attached is PDF that displays formats for the probing cycles.  HTH

Inspection Plus for Haas.pdf

[Machineguy]

Mic6

I do the same thing. Saves a lot of time. I have a lot of jobs with clamp changes, probing, ect.