Haas OTS Probe Tool Diameter off?
Close
Login to Your Account
Results 1 to 10 of 10
  1. #1
    Join Date
    Jul 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    312
    Post Thanks / Like
    Likes (Given)
    118
    Likes (Received)
    30

    Default Haas OTS Probe Tool Diameter off?

    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?

  2. #2
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,501
    Post Thanks / Like
    Likes (Given)
    2190
    Likes (Received)
    2716

    Default

    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....

  3. #3
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    601
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    211

    Default

    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)

  4. Likes Mike1974, Djstorm100, Fancuku, Chris59 liked this post
  5. #4
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,501
    Post Thanks / Like
    Likes (Given)
    2190
    Likes (Received)
    2716

    Default

    Quote Originally Posted by 13engines View Post
    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...?

  6. Likes snowshooze, Djstorm100 liked this post
  7. #5
    Join Date
    Sep 2010
    Location
    Anchorage, Alaska, USA
    Posts
    716
    Post Thanks / Like
    Likes (Given)
    307
    Likes (Received)
    142

    Default

    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

  8. Likes Djstorm100 liked this post
  9. #6
    Join Date
    Jul 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    312
    Post Thanks / Like
    Likes (Given)
    118
    Likes (Received)
    30

    Default

    Quote Originally Posted by Mike1974 View Post
    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.

    Quote Originally Posted by 13engines View Post
    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.

  10. #7
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    624
    Post Thanks / Like
    Likes (Given)
    91
    Likes (Received)
    158

    Default

    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.

  11. Likes Djstorm100 liked this post
  12. #8
    Join Date
    Sep 2020
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    it only puts absolute measured diameter of the tool into D- diameter offset and makes wear offset=0

    But if your programming is done with the center of the cutter, then you actually only need the difference between actual and programmed diameters of the tool. for more information read this article Ratcheting Wrenches: Types and Options - Ratchet Wrench

  13. #9
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    601
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    211

    Default

    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...

  14. #10
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    624
    Post Thanks / Like
    Likes (Given)
    91
    Likes (Received)
    158

    Default

    Quote Originally Posted by 13engines View Post
    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.

  15. Likes 13engines liked this post

Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •