What's new
What's new

Haas OTS Probe Tool Diameter off?

Djstorm100

Cast Iron
Joined
Jul 26, 2014
Location
Richmond
Hey everyone, I notice my Haas OTS is not calculating the right diameter at least it doesn't seem like it. Endmills tested were helical in Maritool holders. I've got some tight tolerance features I'm gonna have to walk in and why I was measuring the tool diameter.

Example
1/4" end mill in a endmill holder measures 0.2519

**However run out toward the bottom of the end mill is only 0.0003-4***

Tired 1/8" endmill in a ER16 run out is 0.0001-2 toward the bottom of the end mill. The diameter on it came out to be 0.1241

I wanted to test this more on some other tooling, however I didn't have enough time to do so.

Has anyone deal with this?

Other things to check out?
 
It seems you're assuming that the end mills are dead on size which is almost never the case. It really doesn't matter what your tools measure, whether chasing tight tolerance part features are not. Creating the part features includes the tool and machine flex which is not measured at the tool probe.

Make sure the probes location is precisely known and calibrate it for side tool touch off using a pin of exacting diameter, positioned with the touching side set at the mid point of runout it has in the holder used. (Or whatever method Haas/Renishaw suggest)

Use comp on all finish passes so you can dial in your sizes. Eliminating runout of your tools is not a bad idea, but counting on probe measured offset/diameter numbers to translate perfectly into exactly sized parts is.

Honestly, I almost never measure my tool diameters. I just use nominal or nominal plus comps to start. Again it's the size that happens at the cut that matters.

As you said... walk it in. (with comp)
 
It seems you're assuming that the end mills are dead on size which is almost never the case. It really doesn't matter what your tools measure, whether chasing tight tolerance part features are not. Creating the part features includes the tool and machine flex which is not measured at the tool probe.

Make sure the probes location is precisely known and calibrate it for side tool touch off using a pin of exacting diameter, positioned with the touching side set at the mid point of runout it has in the holder used. (Or whatever method Haas/Renishaw suggest)

Use comp on all finish passes so you can dial in your sizes. Eliminating runout of your tools is not a bad idea, but counting on probe measured offset/diameter numbers to translate perfectly into exactly sized parts is.

Honestly, I almost never measure my tool diameters. I just use nominal or nominal plus comps to start. Again it's the size that happens at the cut that matters.

As you said... walk it in. (with comp)

As he said, doesn't really matter if it checks .126 or .124, the finished part is what matters. That is what wear comp (or probing for dim's) is for. Can't find it now, but I remember some MSC tools had a +0.0/-.005" tolerance on cutting diameter so...?
 
Well,
I went through this.
To overcome it, I took a 1" cat 40 holder and put a chunk of 12L14 CF bar in it as a tool.
Put a brazed tool in the vise and turned the bar stock just as if I were in a lathe. ( Cut a good finish you can get a solid measurment from )

After that, I ran the tool setter and adjusted it's parameters until they matched up. Having all runnout eliminated narrows everything down.
I have had no issues since. It the tool setter says that .5 inch endmill is cutting at .5016 in that holder, I use that in either the tool table in the software, or the tool diameter offset in the case of programming to nominal.
Worked for me.
Mark
 
Did you calibrate with a calibration tool like this?

CAT40 Tool Probe Calibrator - Made in USA MariTool

We don't use the diameter so I don't know what else I would check....

Yes sir, I have that exact tool.

It seems you're assuming that the end mills are dead on size which is almost never the case. It really doesn't matter what your tools measure, whether chasing tight tolerance part features are not. Creating the part features includes the tool and machine flex which is not measured at the tool probe.

Make sure the probes location is precisely known and calibrate it for side tool touch off using a pin of exacting diameter, positioned with the touching side set at the mid point of runout it has in the holder used. (Or whatever method Haas/Renishaw suggest)

Use comp on all finish passes so you can dial in your sizes. Eliminating runout of your tools is not a bad idea, but counting on probe measured offset/diameter numbers to translate perfectly into exactly sized parts is.

Honestly, I almost never measure my tool diameters. I just use nominal or nominal plus comps to start. Again it's the size that happens at the cut that matters.

As you said... walk it in. (with comp)


It's common for endmills to come in undersized, yes sir. Call me surprised when I found my 1/4" endmill was reading larger than it should, when runout is min. Don't understand how that can be. Unless the tool is oversize it self but have no total accurate way to measure it.

I remember a user having the same issue and changing parameters of the OTS pad diameter.
 
Machine mounted tool setters are great and accurate for tool length setting. The runout of both, calibration tool used for setup of the tool setter and of the measured tool, causes inaccuracies and lack of correlation between them. The exact effective diameter of the rotating cutting tool can be established only by taking a cut in the material and measuring the width of the slot (either manually or using the spindle probe). Then the diameter offset value can be updated.
 
I'm not positive about how an OTS Tool Probe gets its diameter/radius measurement, but I have to imagine it's a combination of all these things, which from the get-go looks like room for small, stacked errors.

*1) The precise location of the measuring pad has to be known. Preferably located with a dial test indicator with a light touch so as not to move the pad or unseat an OTS contact.

2) The precise diameter of the measuring pad. Measured with your best use of a micrometer.

3) The lag in the Skip or High Speed Skip Signal. This is where the calibration routines take over?

4) Tool runout. I imagine it has an enlarging influence on true diameter. Snowshooze #5 had a pretty good idea about handling this.

* One could probably eliminate the need or effects of number 1 by measuring the tool on opposite sides of the OTS pad and taking the average. A cake walk I'm sure for any Macro heads.

As I said earlier, I still think why bother? This stuff here is nothing more then an expansion of what Probe #7 said, and me just thinking through what's needed or what happens in a tool diameter measurement.

On another note: Not sure what "Ratcheting Wrenches" (not following that link) has to do with the somewhat common practice of running an offset tool path with tiny comps. (Which BTW can be entered at the one-in-the-same_D or D-Wear address.) Also less we forget, the "D" in the tool tables is sweet in that it reminds us of "Diameter," which was on purpose, but it is in fact an "Address" in the computer where one normally inputs a Radius in the "D" column. At least on the Fanucs I'm familiar with. Just sayin...
 
I'm not positive about how an OTS Tool Probe gets its diameter/radius measurement, but I have to imagine it's a combination of all these things, which from the get-go looks like room for small, stacked errors.
In order to prevent these errors the calibration routine of TS center and diameter is normally supplied as a part of setter macro programs.
Here is my prescription for proper procedure:
1. Choose your calibration tool. Do not waist hundreds of dollars on dedicated instrument. Use your own tool holder which fits the machine spindle, clamp in it pin (0.5 inch dia. end mill opposite side clamped in holder is just fine).
2. Using micrometer measure the diameter of your calibration tool.
3. Place the tool above the setter, roughly in its center.
4. Run the dedicated macro. The suggested progression of tasks in such macro:
4.1. While the calibration tool ROTATES, touch the setter stylus on both sides in X and Y, and calculate its EFFECTIVE center. Pay attention, it does not correlates with setter's GEOMETRICAL center.
4.2. Place the probe over just found tool setter's center, and repeat the procedure while the tool DOES NOT ROTATE.
Based on measured calibrating tool diameter, calculate the EFFECTIVE diameter of the setter's stylus. Once more, it differs from the NOMINAL diameter given by producer.
That's all, the only thing you have to measure while executing this procedure is your tool diameter. If you choose to use calibration pin of known diameter, even this action can be spared.
 
yes, I have dealt with this problem for over a year on new machine

Hey everyone, I notice my Haas OTS is not calculating the right diameter at least it doesn't seem like it. Endmills tested were helical in Maritool holders. I've got some tight tolerance features I'm gonna have to walk in and why I was measuring the tool diameter.

Example
1/4" end mill in a endmill holder measures 0.2519

**However run out toward the bottom of the end mill is only 0.0003-4***

Tired 1/8" endmill in a ER16 run out is 0.0001-2 toward the bottom of the end mill. The diameter on it came out to be 0.1241

I wanted to test this more on some other tooling, however I didn't have enough time to do so.

Has anyone deal with this?

Other things to check out?

I have a HAAS TM-3P New next Gen. mill now for over 1 year. The Wireless Renishaw Probe (accurate to a couple of tenths) I have is an OMP-40 Work probe and an OTS Tool Probe. Both dialed in using a Maritool Master and Mitutoyo .9998 ring gage. None of the tools measured by the $6,000.00 plus OTS probe were within .001" of the actual cut diameter. Also, the errors are different from tool to tool. HAAS/Phillips has been out numerous times and has verified the problem. Their answer was to change the values etched on the Cal. Master to compensate during the Cal. program. This is not a ix. It is a work around. It also only helps with that one tool.

My issue is not how to trick the machine to make the proper cut. My issue is the $6,000.00 plus I spent on the Probing system. The measured diameter of even the Cal. Master is off by more than .001"!

Please email me if anyone else is having this probing problem. I will be suing HAAS/Phillips/Renishaw to get this right. If there are enough responses, we may be able to gain status of a "class action". Renishaw has emailed me that the actual cut should not be more than a couple of tenths off.
 
I have a HAAS TM-3P New next Gen. mill now for over 1 year. The Wireless Renishaw Probe (accurate to a couple of tenths) I have is an OMP-40 Work probe and an OTS Tool Probe. Both dialed in using a Maritool Master and Mitutoyo .9998 ring gage. None of the tools measured by the $6,000.00 plus OTS probe were within .001" of the actual cut diameter. Also, the errors are different from tool to tool. HAAS/Phillips has been out numerous times and has verified the problem. Their answer was to change the values etched on the Cal. Master to compensate during the Cal. program. This is not a ix. It is a work around. It also only helps with that one tool.

My issue is not how to trick the machine to make the proper cut. My issue is the $6,000.00 plus I spent on the Probing system. The measured diameter of even the Cal. Master is off by more than .001"!

Please email me if anyone else is having this probing problem. I will be suing HAAS/Phillips/Renishaw to get this right. If there are enough responses, we may be able to gain status of a "class action". Renishaw has emailed me that the actual cut should not be more than a couple of tenths off.

Have you verified the tool setter probe stylus was properly squared? There is a relatively simple indicator procedure for this. It will produce errors as you describe if it is not perfectly aligned. I agree with comments about the calibration tool and using a carbide shank instead. I have a fancy Haas calibration tool that will not run true with less than 0.0005 runout no matter what I do. It is garbage.
 
HAAS Probing Problems

Have you verified the tool setter probe stylus was properly squared? There is a relatively simple indicator procedure for this. It will produce errors as you describe if it is not perfectly aligned. I agree with comments about the calibration tool and using a carbide shank instead. I have a fancy Haas calibration tool that will not run true with less than 0.0005 runout no matter what I do. It is garbage.

I have adjusted the OTS Probe surface to less than one tenth in X and Y.

What did you do with the HAAS Calibration tool?
 
I have adjusted the OTS Probe surface to less than one tenth in X and Y.

What did you do with the HAAS Calibration tool?

It is in a box somewhere under my Q/A table.

About a year after we bought the mill, we had a problem where the machine smashed the tool probe. We had gotten to where we used it all the time and had no issues before. This time, it simply fed at moderate speed down onto the probe. It would have had a hard crash if I was not there to e-stop it. We were told the probe battery probably failed. I changed and the issue did not go away. After investigating, we found there was an issue in the probing routine. Looking closer, we found many bugs in the VPS routines. Things like bolt circle routines that made fantasy patterns regardless of the input data. Some of the other canned routines did crazy stuff.

Haas had reloaded the code in the machine on a service visit just before all this happened. We know a local Haas tech who came over and reloaded the code with a version he said he was confident in. It fixed the VPS issues and it also changed the probe code. It worked fine since. The code we now have looks for the communication with the probe before it moves (I do not know about the old code). Given this, the battery advice was just bullshit.

We replaced the tool probe with the Renishaw replacement program. All in, we were out about $1500. Haas just waived their hands and said "software". I did not push it because their tech did us a favor.
 








 
Back
Top