Haas probe for flatness in Z axis

[david]

Recently retired from machining and working with Okuma mills. Now I am working with a Haas vertical machine with a classic control part time. I am familiar with Renishaw probing routines for the Okuma's but am learning the routines for the Haas. I would like to confirm flatness in the Z axis with a tolerance after Z is set.

Example;

G65 P9832 (Probe On)
G65 P9810 X3. Y0. F200. 
G65 P9810 Z1. F50. 
G65 P9811 Z0. Q0.4 S1. (PROB Z)

G65 P9810 X-3. Y0. F200. 

What kind of code is needed here to verify flatness within .001"

G65 P9833(Probe OFF)

 

Thank you for any suggestions.

[rgrin]

I can picture what you want but I can't think through how you would have to write the macro.  I think you would have to store each point as their own variable since you're baked in routine will just overwrite each one into the same variable.

For instance, my machine is set to write my probe points to #108 so after each probe point you would have to write #500 = [#108] and change the #500 variable for each probe point. That will give you an array of as many points as you want.

The hard part that I haven't figured out yet is how to parse thru those variables. You would need to find the one with least deviation and the one with the most deviation and then subtract their values from eachother to see if their relative deviation is more than .001". Brute forcing to find you min/max deviation is not hard, but the only way I can think is test each one against eachother with LT (Less than) or GT (Greater than)  statements and that will be extremely cumbersome to write.

Hopefully someone more MACRO B inclined will chime in as this is something I have wanted for awhile for some process inspection, but just haven't needed enough to justify the time spent yet

[david]

Thank you rgrin. I was hoping it would simpler than writing a group of if then greater than and less than statements. I know it's not an OSP control but for an Okuma it would be, "CALL OO10 PMOD=3 PEI=0 PEE=.001", simple and short.

[crazy^millman]

5 hours ago, david said:

Recently retired from machining and working with Okuma mills. Now I am working with a Haas vertical machine with a classic control part time. I am familiar with Renishaw probing routines for the Okuma's but am learning the routines for the Haas. I would like to confirm flatness in the Z axis with a tolerance after Z is set.

Example;

G65 P9832 (Probe On)
G65 P9810 X3. Y0. F200. 
G65 P9810 Z1. F50. 
G65 P9811 Z0. Q0.4 S1. (PROB Z)

G65 P9810 X-3. Y0. F200. 

What kind of code is needed here to verify flatness within .001"

G65 P9833(Probe OFF)

 

Thank you for any suggestions.

The cycle itself is what you want to use and define the tolerance inside of the macro when called. HAAS is good about having the documentation online, but on this they seem to fall short.

HAAS WIPS

[Colin Gilchrist]

Here is the manual from 2008. This is what is possible "out of the box", and I believe you'll have to write multiple single surface probe points (P9811), store the result variables, and write your own Macro logic to test the results of multiple points to determine "flatness" of a surface.

Look at Chapter 3 for the "Optional Inputs". In this case I think you want "H" for the +- tolerance value. 

If you are simply trying to determine "is my single measurement point within a +- tolerance value of the target, you'd do the following:

G65 P9811 Z0. H0.001 Q0.4 S1. (PROB Z)

Format 
G65 P9811 Xx or Yy or Zz [Ee Ff Hh Mm Qq Ss Tt Uu Vv Ww] where [  ] denote optional inputs 

english---renishaw-inspection-plus---programming-manual---2008.pdf

[david]

Thank you for all the responses.

Colin, would the following command work for verifying flatness, "G65 P9811 Z0. H0.001 Q0.4  (PROB Z)"  ? By omitting the "S1.",  would it only check the value of Z?

 

[Colin Gilchrist]

Provided you've already activated the G54 work offset, yes.

This is measuring Z-Axis "position", at only a single point, and the H0.001 tells the macro the +/- tolerance of the target Z position (in your case Z-Zero of the active work offset).

You're verifying Z-Axis Position, with a +-0.001 tolerance. You call it "flatness", but it is really just positional tolerance.

[rgrin]

I think the issue with that is it would effectively mean he needs to control his z-axis position to +/-.0005" for that check to work.  If the part doesn't require it already, that shoots the difficulty level of making that part way up IMO.  So either you have the challenge of maintaining z-axis height part to part to +/-.0005" and have to make sure you control it to the same point every time you set it up. OR you do the work and write the macro logic and save yourself the headache for the future. If it's going to be a repeat part, I would lean towards writing the logic personally.

[rgrin]

I just realized the easy way to make Colin and David's work. (Maybe it was obvious to them/others but it just dawned on me).  I would use a separate work offset for checking the part. So if you're machining in G54, I would check it in G59 or something.  After machining is complete, I would call the probe up and reset G59 to the top of the part and probe it and set the current value of G59 offset.  THEN you could use the H.001 tolerance to see if all subsequent probe points are within whatever spec you want.

Seems so simple now....

[david]

Over the years running Okuma's our supervisors has needed something for other employees to do and if we needed a parts loader, we would get a worker for a day or so. After the temporary worker loaded the part and forgot to seat it down or didn't clean the chips off the vise, I would have a scrap part. On a good day it was the first operation so not a lot of time was lost. So we started having the probe verify the part was flat before  the tools started cutting. Here is what  probe program for an Okuma.

CALL OO83 (Probe On)
G15 H1
X3 Y0
G56 H60
CALL O9810 PZ=.4 PF=200
CALL OO10 PMOD=3 PEI=0.000
CALL OO20 PHN=1 PZ=0.000

CALL O9810 PX=-3 PY=0 PF=200
CALL OO10 PMOD=3 PEI=0 PEE=.001 (This line was all it took)

CALL O9810 PZ=2 PF=200
CALL OO84 (Probe Off)

Now I realize I'm using a Haas but its still a Renishaw spindle probe. Hopefully its simpler than writing macros. If it isn't, then it is what it is. I like challenges.

[crazy^millman]

11 minutes ago, david said:

Over the years running Okuma's our supervisors has needed something for other employees to do and if we needed a parts loader, we would get a worker for a day or so. After the temporary worker loaded the part and forgot to seat it down or didn't clean the chips off the vise, I would have a scrap part. On a good day it was the first operation so not a lot of time was lost. So we started having the probe verify the part was flat before  the tools started cutting. Here is what  probe program for an Okuma.

CALL OO83 (Probe On)
G15 H1
X3 Y0
G56 H60
CALL O9810 PZ=.4 PF=200
CALL OO10 PMOD=3 PEI=0.000
CALL OO20 PHN=1 PZ=0.000

CALL O9810 PX=-3 PY=0 PF=200
CALL OO10 PMOD=3 PEI=0 PEE=.001 (This line was all it took)

CALL O9810 PZ=2 PF=200
CALL OO84 (Probe Off)

Now I realize I'm using a Haas but its still a Renishaw spindle probe. Hopefully its simpler than writing macros. If it isn't, then it is what it is. I like challenges.

Stock Allowance Macro work where you can have up to 6 Points? O9820

 

[david]

Thank you crazy^millman.

[jpatry]

On 10/19/2023 at 12:16 PM, david said:

Recently retired from machining and working with Okuma mills. Now I am working with a Haas vertical machine with a classic control part time. I am familiar with Renishaw probing routines for the Okuma's but am learning the routines for the Haas. I would like to confirm flatness in the Z axis with a tolerance after Z is set.

Example;

G65 P9832 (Probe On)
G65 P9810 X3. Y0. F200. 
G65 P9810 Z1. F50. 
G65 P9811 Z0. Q0.4 S1. (PROB Z)

G65 P9810 X-3. Y0. F200. 

What kind of code is needed here to verify flatness within .001"

G65 P9833(Probe OFF)

 

Thank you for any suggestions.

With the Renishaw macros that are shipped with there is not a dedicated multisample probing macro to do what you want to do.

You would have to take a Z probe sample and dump it out to a separate variable at each location, then perform the math on the sampled values.

It appears that I am wrong, Millman has the solution

[jpatry]

On 10/20/2023 at 10:13 AM, crazy^millman said:

Stock Allowance Macro work where you can have up to 6 Points? O9820

 

Neat, so I could interrogate 195 and 194 to pull an average z position 

[crazy^millman]

On 11/4/2023 at 11:18 AM, jpatry said:

Neat, so I could interrogate 195 and 194 to pull an average z position 

I was the Product Manager at Verisurf for Machine Tool Probing and PCMM/Master3DGage. I released a free complete Renishaw probing logic using drill cycles on the forum years ago. I am always learning so glad to pass on something someone else can learn from.