584,842 active members*
4,554 visitors online*
Register for free
Login

Thread: Tool Wear

Results 1 to 17 of 17
  1. #1
    Join Date
    Dec 2006
    Posts
    302

    Tool Wear

    I'm trying to like to like PP, really I am. Sure, the interface is ugly and a little counter-intuitive. In time those issues will be long forgotten. My current problem, or question, is how to enter tool wear in the tool setup file.

  2. #2
    Join Date
    Nov 2007
    Posts
    2151

    Re: Tool Wear

    I see this question now and then and struggled to understand what this is and as a new user I would like to know what tool wear is. Is tool wear a measurement of tool diameter, length or both? Is it used during program execution or a fixed value in tool table? If the tool does wear down in diameter or length or both, how much is this value? Would this value be divided by 2 and make it so small that its outside the performance of a tormach ? My brain keeps telling me these numbers are very small, what am I missing here?
    Any information on this subject would be welcome

  3. #3
    Join Date
    Dec 2006
    Posts
    302

    Re: Tool Wear

    Truth is I'm more likely to snap a tool than to wear it down any significant amount. Tool wear can be used to conveniently tweak a cut that's a little off. A real machinist will no doubt shake his head at me, but since I'm not a real machinist, they'll just have to grin and bear it. ;-)

  4. #4
    Join Date
    Nov 2007
    Posts
    2151

    Re: Tool Wear

    Quote Originally Posted by JohnToner View Post
    Truth is I'm more likely to snap a tool than to wear it down any significant amount. Tool wear can be used to conveniently tweak a cut that's a little off. A real machinist will no doubt shake his head at me, but since I'm not a real machinist, they'll just have to grin and bear it. ;-)
    I recently noticed my tools start cutting like crap long before they show wear form what I see anyway. I try to by decent quality tools "yg" mostly and hope they are accurate in size. I have limited quality measuring tools and real ability to measure cutters size to any degree of accuracy.

  5. #5
    Join Date
    Jun 2014
    Posts
    1777

    Re: Tool Wear

    Quote Originally Posted by JohnToner View Post
    Truth is I'm more likely to snap a tool than to wear it down any significant amount. Tool wear can be used to conveniently tweak a cut that's a little off. A real machinist will no doubt shake his head at me, but since I'm not a real machinist, they'll just have to grin and bear it. ;-)
    This is enlightening to me as well.......
    I always wondered how this was used?? I never use the cutters long enough to wear them down any measurable amount, they are broken or chipped or dulled before any wear can take place that I am capable of measuring.
    I use CAM to tweak my tool diameters to adjust the size of bores or slots, profiles etc.
    I mainly use it to change the tool diameter when one is reground or sharpened.

    I too am a rookie cnc machinist, and dont hand code, so I have never used this function. I can see that it could be useful in hand coding though.
    mike sr

  6. #6
    Join Date
    Jun 2006
    Posts
    3063

    Re: Tool Wear

    I could be way off base, but I thought that one of the uses for a tool wear parameter in the controller tool table was to provide a way to account for wear in tools during a production. The operator would check dimensions every few parts - if he finds a square boss is 0.0005" too large in X and Y, he'd adjust the diameter wear field by 0.0005" and the controller would take into account both the entered too diameter and the wear parameter to adjust the tool path by 0.0005". I'd thought that Mach3 could not reliable use the wear parameter in its tool table so there seemed no point to me in trying to use it.

  7. #7
    Join Date
    Aug 2013
    Posts
    980
    Correct me if I am wrong but I thing the cam program does the tool wear comp so the controller never sees it.
    It would make since the controller tool table could be manually adjusted too.


    Quote Originally Posted by MichaelHenry View Post
    I could be way off base, but I thought that one of the uses for a tool wear parameter in the controller tool table was to provide a way to account for wear in tools during a production. The operator would check dimensions every few parts - if he finds a square boss is 0.0005" too large in X and Y, he'd adjust the diameter wear field by 0.0005" and the controller would take into account both the entered too diameter and the wear parameter to adjust the tool path by 0.0005". I'd thought that Mach3 could not reliable use the wear parameter in its tool table so there seemed no point to me in trying to use it.

  8. #8
    Join Date
    Jun 2005
    Posts
    653

    Re: Tool Wear

    The idea is mostly for production use, tools wear, break and get replaced over time. Especially when it was being implemented way back when, endmills can vary a few tenths here or there and resharpened ones even more. The CNC machine operator can't be running back to CAM to correct for variations between tools when they swap one out in the middle of a production run, so they just punch a new value into the tool wear setting and the machine deals with the difference between the 'ideal' tool that was programmed and what's actually in the machine.

  9. #9
    Join Date
    Nov 2007
    Posts
    2151

    Re: Tool Wear

    Thanks for the information, Checking the finished part for variance in size makes sense. I was thinking even tool deflection would in general be greater then wear. Anyway, after asking the above question I did some thinking about tooling and under what conditions it would wear in a predictable "programmable" manner. I concluded I have exposure to a very small selection of tools and the world is full of systems, processes and tools that would benefit and or require some strategy or compensation method. Cnc grinding systems for making end mills comes to mind as one

  10. #10
    Join Date
    Nov 2007
    Posts
    2151

    Re: Tool Wear

    Quote Originally Posted by shred View Post
    The idea is mostly for production use, tools wear, break and get replaced over time. Especially when it was being implemented way back when, endmills can vary a few tenths here or there and resharpened ones even more. The CNC machine operator can't be running back to CAM to correct for variations between tools when they swap one out in the middle of a production run, so they just punch a new value into the tool wear setting and the machine deals with the difference between the 'ideal' tool that was programmed and what's actually in the machine.
    Ahh!
    There you go, Hard to see the big picture. I can run back to cam and rebuild everything at will and takes no time at all. If your on a mile long factory floor this is not going to happen and it takes a meeting with 15 people to change anything.

  11. #11
    Join Date
    Mar 2010
    Posts
    72

    Smile Re: Tool Wear

    Quote Originally Posted by mountaindew View Post
    Ahh!
    There you go, Hard to see the big picture. I can run back to cam and rebuild everything at will and takes no time at all. If your on a mile long factory floor this is not going to happen and it takes a meeting with 15 people to change anything.
    Guys, Seriously, If you are sooo worried about Tool wear and running a mile down the other end of the shop to change the cam. You should probably have a real machine. You know, Mori Seiki, Okuma, Makino, Matsuura, Yasda, JTEKT etc. etc. etc. With a real control . OSP or Fanuc or one of a bunch of others.

    "Tool wear" comes in in a production situation (real manufacturing) where a machine is set up with a primary tool to do a certain function (or functions) and under a set of predefined(predetermined tool load limit) circumstances the machine(thru the operating system) will enact a tool change with a replacement tool to do the same function as the previous tool.
    To have that type of function on a machine it is likely that you will have a tool magazine that could be in the double or even triple figures (maybe 50+ or even 150+ tool magazine).

    Don't sweat Tool wear.
    In the scheme of things it's a minor(read insignificant) detail at the Tormach level.
    While you cannot specifically change "tool wear" you can change the diameter of the tool as listed in the tool list that you created on your PP controlled machine.

    It may start off as a 10.00mm tool when it was programmed by whoever.
    But when you read the tool list and set your tools according to what you have, you can simply enter the size of the tool that you have.
    The machine will compensate for the difference.
    But you will need to apply it through G41 or G42 and at the appropriate time in the NC file.
    In PP it does work, unlike Mach 3 where it never worked for me.
    Don't forget to cancel it out at the appropriate time either, cos it will(read may...depends on the following operation) affect the next tool in some way.
    IF you are wishing to use G41 G42 avoid this thru manual programming.
    If you enter it at the wrong time(in the program) it may not work or not apply correctly.
    So it also goes to say that when you cancel G41 G42 with the G40 command, make sure too, that it is at the right time. The consequences could be interesting.

    When the CAM process is applied to the file, I would expect that your CAM program will ask (in one form or another) if you want to apply G41 or G42.
    If you do not accept it, then your tool diameter (as set in tool offsets) should be ignored.
    If you do accept it then G41 or G42 will be incorporated into the code and of course you will need to have the diameter of the cutter in the "diameter offset".
    Even if you just enter the standard size, say 10.000 (mm) then it will be exactly the same as having not written G41 or G42 into the code.
    You should then notice that your pocket(example) will be undersize, by the difference between the programmed size and the actual size of the cutter.
    It can be very handy if you are after a very accurate size. You can work your way out to it(required size), so to speak.

    REMEMBER too, that not all the error will be because of the difference between the "programmed size", actual "cutter size" and the Diameter entered into the cutter diameter size(in off set).
    The remainder of the error will be in your slideways, Ball screws etc.

    So don't worry about the small stuff(tool wear).
    There are plenty of other things to worry about before tool wear.
    (Don't even get me started on Flex, distortion, spindle temperature and cutter condition).

    If anybody sees tool wear any differently, then I would love to hear your opinions....I'm not an expert, what I have written is purely based on my number of years of experience(some of that may be a bit out of date).

    Regards
    Peter

  12. #12
    Join Date
    Dec 2006
    Posts
    302

    Re: Tool Wear

    Most enlightening.

  13. #13
    Join Date
    Jun 2014
    Posts
    1777

    Re: Tool Wear

    Enlightening here too.

    I never knew why they saw a reason for it as it can be done in cam, I resize cutters often (reground), That mile to the cam guy, or difficulty to get cam changed explains the need for it at the operator level, also they get enough mileage out of their tools to actually need it ha!
    mike sr

  14. #14
    Join Date
    Mar 2010
    Posts
    72

    Re: Tool Wear

    Hi,
    Cutting tool manufacturers rarely (if ever) make tools "on size" they are always undersize.
    Regardless of manufacturer.
    I'm not sure why, but I have never had a tool that is SIZE.
    Everything that is made(manufactured) has a tolerance and in the case of cutting tools it is ALWAYS a negative tolerance. Always.
    I guess the reason being is that on real machines, you can "adjust" your size(for a tool that is undersize) via your tool offsets, but if you have a tool that is oversize, say 10.03mm diameter, how can you generate a 5.00mm radius on the inside of a pocket?
    I would have thought that a programmer, and in fact a machinist would prefer a G02 G03 for a corner move.
    At least that way, when the cutter is undersize the program can compensate for the ARC being generated at the corner.
    In a G01 to G01 move you cannot change the radius in the corner.
    Your controller will stop short of the theoretical centre of the radius point(if the cutter is oversize) and go the required amount further if the cutter is undersize, but neither of those two scenarios will give you the correct radius in the corner.
    In saying that, the radius(of the pocket) may have a different tolerance to the more important tolerance applied to the pocket itself.
    Generally you would have a larger radius(+tolerance) on both an internal pocket AND an external radius.
    As a general rule, if you would not be looking to contact(location) on the corner radius' of the pocket, only the sides.

  15. #15
    Join Date
    Jun 2014
    Posts
    1777

    Re: Tool Wear

    Has anyone figured out how to set "tool wear" in PathPilot?
    I always set actual cutter diameter in CAM to the actual diameter, I am wondering just how to go about it in Pathpilot? The only critical thing I know of in the tool table is length, the diameter setting (tool table), in my limited understanding, is just a figure? Maybe I am missing something, and if so I would like to learn the method of setting it.......
    mike sr

  16. #16
    Join Date
    Jun 2013
    Posts
    1041

    Re: Tool Wear

    Tool wear comp and diameter comp are basically the same thing. There not just for production. There for accurately cutting parts without reposting every time. They are both implemented through g41 and g42. Wear comp is when your cam program adjusts like always for your tool size selected. It also outputs in g41/42 the pre comped path. Then if you cut a bearing seat or some other critical dimension instead of reposting your code you just input the amount your feature is off in the wear field and run the program again. For diameter comp the cam program does not adjust for g41/42 it just outputs the actual geometry with g41/42. The control take the tool diameter in the diameter column and adjusts the toolpath accordingly. If the part is off you just adjust the tool diameter in the control what is needed to bring the part to the correct size and rerun the program. Good cam programs will allow you to do it either way and there is no need to worry about turning comp on and off. The cam will turn on comp at the beginning of each cut and turn it off at the end of the cut. With wear comp if your part is off by -.002 you would put that in the wear column. With diameter comp if your part is off by -.002 or +.002 depending on inside or outside measurement you would make the diameter of the tool .002 less then what it was before. Sorry if I'm confusing. Either way if your cam has the ability and your control supports it you can save time on any part needing high accuracy production or not. It also allows you to creep up on a critical dimension which can be a life saver on expensive parts.

    Ben

  17. #17
    Join Date
    Jun 2014
    Posts
    1777

    Re: Tool Wear

    Quote Originally Posted by bhurts View Post
    Tool wear comp and diameter comp are basically the same thing. There not just for production. There for accurately cutting parts without reposting every time. They are both implemented through g41 and g42. Wear comp is when your cam program adjusts like always for your tool size selected. It also outputs in g41/42 the pre comped path. Then if you cut a bearing seat or some other critical dimension instead of reposting your code you just input the amount your feature is off in the wear field and run the program again. For diameter comp the cam program does not adjust for g41/42 it just outputs the actual geometry with g41/42. The control take the tool diameter in the diameter column and adjusts the toolpath accordingly. If the part is off you just adjust the tool diameter in the control what is needed to bring the part to the correct size and rerun the program. Good cam programs will allow you to do it either way and there is no need to worry about turning comp on and off. The cam will turn on comp at the beginning of each cut and turn it off at the end of the cut. With wear comp if your part is off by -.002 you would put that in the wear column. With diameter comp if your part is off by -.002 or +.002 depending on inside or outside measurement you would make the diameter of the tool .002 less then what it was before. Sorry if I'm confusing. Either way if your cam has the ability and your control supports it you can save time on any part needing high accuracy production or not. It also allows you to creep up on a critical dimension which can be a life saver on expensive parts.

    Ben
    Thanks Ben,

    My cam does this (sprutcam 7) and thats where I set the tool diameter. I was just wondering how its set in the machine controller (Pathpilot) for touching up without having to change cam, just curious.
    mike sr

Similar Threads

  1. Tool Wear
    By rckdef in forum Haas Mills
    Replies: 9
    Last Post: 08-09-2014, 01:32 PM
  2. Replies: 2
    Last Post: 02-11-2014, 01:17 PM
  3. Replies: 7
    Last Post: 01-23-2013, 05:46 PM
  4. Dealing with tool wear
    By JTulley in forum Tormach Personal CNC Mill
    Replies: 11
    Last Post: 11-17-2008, 07:48 PM
  5. tool wear indicater
    By Vern Smith in forum Haas Mills
    Replies: 13
    Last Post: 03-20-2007, 07:09 PM

Tags for this Thread

Posting Permissions

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