Haas probe tweak - need help!

metal-ica · Oct 2, 2020

My Z-depths are off between .0005 / .001 of an inch. (yes, it's calibrated)

With my classic control I was able to dial it in by entering this amount into the probes tool offset. In my case tool 21.

This works well.

On my next-gen control if I enter any adjustments into the tool 21 offset the machine will alarm out when probing parts telling me to calibrate my probe. The machine knows what value was entered during calibration and alarms out if there is any deviation. I sorta understand the purpose but it's annoying.

Does anyone know how can I make adjustments to the z value of the probe?

Mike1974 · Oct 2, 2020

metal-ica said:
My Z-depths are off between .0005 / .001 of an inch. (yes, it's calibrated)

With my classic control I was able to dial it in by entering this amount into the probes tool offset. In my case tool 21.

This works well.

On my next-gen control if I enter any adjustments into the tool 21 offset the machine will alarm out when probing parts telling me to calibrate my probe. The machine knows what value was entered during calibration and alarms out if there is any deviation. I sorta understand the purpose but it's annoying.

Does anyone know how can I make adjustments to the z value of the probe?

I don't have an answer to your probe question, but why not just adjust your G54 Z value, or a specific tool offset. IMO, it is pretty common to tweak offsets at the machine vs getting the probe perfect - tool wear, material varying, etc.

metal-ica · Oct 2, 2020

Because I'm probing 30 parts every cycle trying to hold +/- .001 z-depth.

coyoinu · Oct 2, 2020

when you calibrated the spindle probe with the master gage, was the tool probe clean? I ran a test yesterday and the calibration was off .001 if there was coolant residue on the tool probe when i ran the total probe calibration.

snowshooze · Oct 2, 2020

Mike1974 said:
I don't have an answer to your probe question, but why not just adjust your G54 Z value, or a specific tool offset. IMO, it is pretty common to tweak offsets at the machine vs getting the probe perfect - tool wear, material varying, etc.

Well..
I did notice a difference in my calibration of the probe off the tool-setter when I set it automatically the way I do tools as opposed to putting the probe over the tool-setter and touching off manually with the MPG
I was always concerned as both elements are spring loaded.
If you can't figure out how to get the thing to calibrate under MPG ( I don't use the tool-set cycle to get my probe G43 ) try to turn your feeds to dead minimum so the probe trips the tool setter as slowly as possible.

Another thought.. you are in the mill I assume...
Check your backlashes. They are in the parameters.. and if you are running box-ways, make sure your gibs are set correctly.
I check mine periodocally.
And.. a good machine warm-up before you start playing around.
You are getting right in there and anything can blow it.

Mike1974 · Oct 2, 2020

metal-ica said:
Because I'm probing 30 parts every cycle trying to hold +/- .001 z-depth.

Well maybe another work around, can use G52 in the program, or are the Z's moving plus and minus?

Mike1974 · Oct 2, 2020

snowshooze said:
Well..
I did notice a difference in my calibration of the probe off the tool-setter when I set it automatically the way I do tools as opposed to putting the probe over the tool-setter and touching off manually with the MPG
I was always concerned as both elements are spring loaded.
If you can't figure out how to get the thing to calibrate under MPG ( I don't use the tool-set cycle to get my probe G43 ) try to turn your feeds to dead minimum so the probe trips the tool setter as slowly as possible.

I think, depending on vintage of machine, when calibrating (not just using a tool setting cycle) the spindle probe it does take 3 hits or so? First one "fast" then 2 successively slower ones.

metal-ica · Oct 2, 2020

I do think it has something to do with the fact that both the probes are spring loaded. My work around was I changed my program to leave z-stock of .001 and that worked great for last nights run. I'm disappointed this isn't dead nuts out of the box. Machine is less than a year old and I added the probing last week. I will hit up my dealer to see what they say.

snowshooze · Oct 2, 2020

Mike1974 said:
I think, depending on vintage of machine, when calibrating (not just using a tool setting cycle) the spindle probe it does take 3 hits or so? First one "fast" then 2 successively slower ones.

Yes, absolutely correct.
But.. although pretty darned good... it ain't spot on.
Which took me a while to identify, but the MPG creeping in tenths did in fact give me a different value.
Just for fun, manually turn on the tool-setter G65 P9855 , touch off the probe as perfect as possible, and compare your values.
Push reset and the probe will turn off.

Also, who installed the tool-setter?
I did mine, and I used my trusty Starret .0001 test indicator to get the face of the tool setter as close to perfect as I could for flat.
I didn't quit until the needle stopped.
You may better verify that as well.

metal-ica · Oct 2, 2020

HAAS installed the probe. Table probe indicates dead nuts in y and better than .0002 across the face in x.

snowshooze · Oct 2, 2020

metal-ica said:
HAAS installed the probe. Table probe indicates dead nuts in y and better than .0002 across the face in x.

There ya go.
Grab your allen wrenches and have at it.
Don't use a cheater bar to get it right. they are opposed jack and draw screws, but you don't want them stretching or compressing.
Then everything has to be re-calibrated.
And then, check it again, tomorrow... a couple days later.... to be sure it is settled.
I don't trust a field hand to meet my expectations.. they gotta get in, get done, and head off to the next one.
And, I ain't got any service here anyway...
At least one variable will be eliminated.

metal-ica · Oct 2, 2020

snowshooze said:
There ya go.
Grab your allen wrenches and have at it.
Then everything has to be re-calibrated.
And then, check it again, tomorrow... a couple days later.... to be sure it is settled.
I don't trust a field hand to meet my expectations.. they gotta get in, get done, and head off to the next one.
And, I ain't got any service here anyway...
At least one variable will be eliminated.

I really don't think that's the root of the problem here though.

snowshooze · Oct 2, 2020

metal-ica said:
I really don't think that's the root of the problem here though.

Usually, there is a compound problem of different aspects..
Tool holder, backlash, gibs, always orient your spindle and holder...
Sometimes you get lucky.
It's always something simple, the problem is there are so many simple things to dig through.

Oh, and I had a salesman trying to sell me a draw-bar pressure gauge.
He swore I had to have one.
So, spindle, draw-bar, bearing lash..
Hey, who threw this machine together, anyway?

Like I said... you are getting right in there. Sometimes you gotta go to the end of the trail.
Of course, if money ain't a problem, them laser tool setters sure look snazzy.
But I am sure you will get it.

Mike1974 · Oct 2, 2020

metal-ica said:
I really don't think that's the root of the problem here though.

I would agree. .0002" in X is not causing .001 in Z. Also, in theory, the spindle probe is calibrated directly in the middle of the disk, which is where all the auto non-rotating are calibrated, and the larger tools should offset exactly half the value of what you type in, meaning they also calibrate at center.

One thing I noticed here at current job, the OTS disc had some marring/scratchin/dings, almost like an endmill was running forward when doing a touch off? Anyways, I disassembled them and ground the tops in a V block with a diamond wheel, we get much better repeatability now.

Mike1974 · Oct 2, 2020

One other thing, did you use a probe calibration tool in the spindle when you set it up?

CAT40 Tool Probe Calibrator - Made in USA MariTool

Shouldn't affect the variances you are seeing, but nice to have 1 single known diameter/length tool if you have multiple machines.

thesidetalker · Oct 2, 2020

When you get the "probe needs calibration" alarm, the control is just checking the tool length for probe (#2000 var) to #10561

You can bypass this by setting them both to whatever you want. I do this regularly. I use a simple macro to set tool lengths 'as drill' for whatever is in the spindle. Very handy when updating or just setting in general, esp if you use a lot of small tools.

I update my probe that way. Added a statement at the end that if the probe is in spindle, it will also update #10561.

If you are consistently off by the same amount, you could add or subtract some at the end?

This is what I'm using, I picked G200 to use. And in my case, my probes on every machine are T25.

Code:

%
O09013 (PROBE - TOOL LENGTH 4 DRILL) 

G65 P9995 A0. B1. C2. T [ #3026 ] 

(CLEAR CURRENT LOAD)
#[5800+#3026]= 0

(CLEAR TOOL TIMERS)
#[5500+#3026]= 0
#[5400+#3026]= 0
#[5700+#3026]= 0

(UN-EXPIRE TOOL) 
#[ 8000 + #3026 ]= 0 

IF [ #3026 EQ 25. ] THEN #10561= #2025 

#3901= #3901 -1 
#3902= #3902 -1 

M30 
%

If you need to, add something like this at the end to make adjustments... (but change 25 to whatever your probe is.)
#2025= #2025 ± .001
#10561= #2025

snowshooze · Oct 2, 2020

Mike1974 said:
One other thing, did you use a probe calibration tool in the spindle when you set it up?

CAT40 Tool Probe Calibrator - Made in USA MariTool

Shouldn't affect the variances you are seeing, but nice to have 1 single known diameter/length tool if you have multiple machines.

I didn't go quite that far, in my case I just bored a hole in a chunk of steel and measured it. I know I am good to .0002 and when we get under that, we start arguing. Used as gauge right then. At least I was pretty sure my hole was aligned... as good as my spindle.

metal-ica · Oct 2, 2020

One other thing, did you use a probe calibration tool in the spindle when you set it up?

CAT40 Tool Probe Calibrator - Made in USA MariTool

Shouldn't affect the variances you are seeing, but nice to have 1 single known diameter/length tool if you have multiple machines.

No....but I ordered one yesterday wondering if it had anything to so with it. I'll re-calibrate when it comes in. I don't think that's the problem either though.

metal-ica · Oct 2, 2020

When you get the "probe needs calibration" alarm, the control is just checking the tool length for probe (#2000 var) to #10561

You can bypass this by setting them both to whatever you want. I do this regularly. I use a simple macro to set tool lengths 'as drill' for whatever is in the spindle. Very handy when updating or just setting in general, esp if you use a lot of small tools.

I update my probe that way. Added a statement at the end that if the probe is in spindle, it will also update #10561.

If you are consistently off by the same amount, you could add or subtract some at the end?

This is what I'm using, I picked G200 to use. And in my case, my probes on every machine are T25.
Code:
%
O09013 (PROBE - TOOL LENGTH 4 DRILL)

G65 P9995 A0. B1. C2. T [ #3026 ]

(CLEAR CURRENT LOAD)
#[5800+#3026]= 0

(CLEAR TOOL TIMERS)
#[5500+#3026]= 0
#[5400+#3026]= 0
#[5700+#3026]= 0

(UN-EXPIRE TOOL)
#[ 8000 + #3026 ]= 0

IF [ #3026 EQ 25. ] THEN #10561= #2025

#3901= #3901 -1
#3902= #3902 -1

M30
%
If you need to, add something like this at the end to make adjustments... (but change 25 to whatever your probe is.)
#2025= #2025 ± .001
#10561= #2025

this is the ticket right here! I'll do some digging. Thank you!

snowshooze · Oct 3, 2020

I'd sure like to hear how this worked out for you, it is a lot deeper digging than I have done.
Thanks!
Mark

Haas probe tweak - need help!

Cast Iron

Diamond

Cast Iron

Aluminum

Stainless

Diamond

Diamond

Cast Iron

Stainless

Cast Iron

Stainless

Cast Iron

Stainless

Diamond

Diamond

Stainless

Stainless

Cast Iron

Cast Iron

Stainless

Similar threads