Z work offset and/or tool length offset in vmc??
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,271
    Post Thanks / Like
    Likes (Given)
    915
    Likes (Received)
    512

    Default Z work offset and/or tool length offset in vmc??

    Hi Everybody!

    I was flipping through Smid's CNC Programming Handbook because I enjoy going "back to the basics" from time to time and he really preaches the use of Z0 in work offsets and then compensating entirely via the tool length offset:

    ...The Z0 offset entry is very important in the machine control. Specified Z0 means that the coordinate setting for the Z amount does not change from one part to another...The only time there is a need to consider Z-axis within the work offset setting is in those cases where the height of each part in the setup is different...

    I can dig it...and that is what we do on machines that don't have probes (leave Z0, touch the tools off to the top of the part, tool offset measure, Bob's your uncle! (so our tool length offsets end up being like -15.123.) But on machines with probes I enjoy setting the Z0 offset to a number that represents the distance from the gage line to the top of the work (on our Haas's) or the distance from the table top to the top of the work (on our Brother's) and then having the tool length offset represent that actual length of the tool!

    I imagine this is just one of those, "more than one way to skin a cat" scenarios but I am inquisitive by nature and tend to suffer from tunnel vision so I wanted to ask if there IS a generally-accepted way of setting top of stock and tool length out there or if it is more of a, "one guy tells you thing and one guy tells you another" deal.

    Thank you!

  2. #2
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    59
    Likes (Received)
    8

    Default

    This is one of those what ever works best for you things.
    Also could of just opened a can of worms

  3. #3
    Join Date
    Jun 2012
    Location
    Chicago, USA
    Posts
    1,762
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    137

    Default

    I'm still wrapping my head around this, and forgive me if it's a dumb question:

    If you leave the WCS Z value as 0, and touch off on the part to set your tool offset instead, doesn't that mean you have to re-touch off every tool, every time you run a different part? That seems like a hassle compared to leaving the tool offsets untouched and just changing to WCS z-offset value.

    I suppose it makes sense if you're setting up for a production run, but for prototyping or small numbers of parts it seems like the other way makes more sense.

    There's probably something I'm missing here - it's been known to happen

    Lee

    Sent from my SM-N960U using Tapatalk

  4. #4
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,803
    Post Thanks / Like
    Likes (Given)
    1189
    Likes (Received)
    1941

    Default

    I prefer the gage line method. It makes more sense for my use. Plus it's a quick visual check on the tool length.

  5. Likes Nerdlinger liked this post
  6. #5
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,803
    Post Thanks / Like
    Likes (Given)
    1189
    Likes (Received)
    1941

    Default

    Quote Originally Posted by leeko View Post
    If you leave the WCS Z value as 0, and touch off on the part to set your tool offset instead, doesn't that mean you have to re-touch off every tool, every time you run a different part? That seems like a hassle compared to leaving the tool offsets untouched and just changing to WCS z-offset value.



    There's probably something I'm missing here - it's been known to happen

    Lee

    Sent from my SM-N960U using Tapatalk
    Yes you would re-touch off for each new set-up. So instead, what seems to be common is to touch off a standard place, like say a 1-2-3 block on the table. Now you measure from the 1-2-3 block to the top of the work and put that in G54 Z value. It's sort of a hybrid of the two.

  7. #6
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    418
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    104

    Default

    So whenever you setup a new part, you have to set every tool you are going to use? Even if they are always in the magazine?

    Very productive.

  8. #7
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,803
    Post Thanks / Like
    Likes (Given)
    1189
    Likes (Received)
    1941

    Default

    ^^ Not if you use the gage line method or the hybrid method.

  9. #8
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,615
    Post Thanks / Like
    Likes (Given)
    1687
    Likes (Received)
    2181

    Default

    If you're running a cnc mill and are not using at least a dial type height setter and a haimer, then you are wasting huge amounts of time.

    And yes, not using the Z work offset is ridiculous.

  10. Likes mhajicek, Nerdlinger, Fancuku liked this post
  11. #9
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,130
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1749

    Default

    Hello Nerdlinger,
    Yes, there are many ways to set the tools and coordinate system for the part. However, where the Z Workshift is always left at Zero, requires the tool length offset to be set for all tools used in the program for each new job. Not all that inconvenient where only few tools are used, but rather time wasting where many tools are involved. Further, unless the routine is to set all tools in the magazine, whether they're used in the particular job or not, this system can result in tools in the magazine with length offsets that suits nothing and the potential for a crash should any of these tools be introduced to the program later and inadvertently not have their tool length offset set.

    With systems that use the Z Workshift to set the workpiece coordinate system, the tool length offsets of all tools in the magazine should suit the current workpiece Z Zero by setting the Z Workshift with any tool in the magazine. I have my clients develop the habit of always setting the Tool Length Offset of any new tool introduced to the machine, as soon as its put into the machine.

    The method of setting the Tool Length Offset of each tool and not using a Z Workshift Offset, also precludes being able to pre set the Offsets away from the machine unless an accurate dimension for where Z Zero of the workpiece involved is within the machine space.

    Overall, the Zero Z Workshift methods provides a few more opportunities to stack the machine.

    Regards,

    Bill

  12. Likes Nerdlinger liked this post
  13. #10
    Join Date
    Jan 2003
    Location
    Posts
    611
    Post Thanks / Like
    Likes (Given)
    134
    Likes (Received)
    197

    Default

    Quote Originally Posted by Nerdlinger View Post
    I was flipping through Smid's CNC Programming Handbook because I enjoy going "back to the basics" from time to time and he really preaches the use of Z0 in work offsets and then compensating entirely via the tool length offset
    Sounds like Mr. Smid has spent more time writing books then running machines.

  14. #11
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,886
    Post Thanks / Like
    Likes (Given)
    2520
    Likes (Received)
    1289

    Default

    Yeah, no.

    As said above, if you touch off the tool on the work you need to repeat that for every setup, even if using the same tools. If your typical job has three tools, maybe not a big deal. Mine often have over 20 per job, and I group jobs that reuse many of the same cutters to save setup time.

    Also think about what happens when you break or wear out a tool. If you're touching on the top of stock, when you set your replacement tool it will be on another piece of stock, which may be a little thicker or thinner, so if you replace one tool you have to touch them all. If you're doing short runs in aluminum, again, maybe not a big deal. Longer runs in steels, Ti, etc., big headache. And how do you save the part that was running when the tool failed? You can't touch off with a part in place. Gotta pull it, put in fresh stock, touch off all your tools again, then put the part back and hope it's in the same place. If it's a $10 piece of stock, no big. Hundreds or thousands, or for some people tens of thousands of dollars per piece of stock, that's a problem.

  15. Likes Nerdlinger liked this post
  16. #12
    Join Date
    Aug 2005
    Location
    CT
    Posts
    8,366
    Post Thanks / Like
    Likes (Given)
    457
    Likes (Received)
    2230

    Default

    Quote Originally Posted by Nerdlinger View Post
    (leave Z0, touch the tools off to the top of the part, tool offset measure, Bob's your uncle! (so our tool length offsets end up being like -15.123.) But on machines with probes I enjoy setting the Z0 offset to a number that represents the distance from the gage line to the top of the work (on our Haas's) or the distance from the table top to the top of the work (on our Brother's) and then having the tool length offset represent that actual length of the tool!

    Not sure how Haas is working nowadays, but 10 years ago there was a definite different procedure in picking up tools between a lathe with toolsettter and without.
    (If I had my guess, their mills were the same.)
    All of that is a bunch of bullsihite because the Haas programmers couldn't figure out how to apply a different logic!

    There SHOULD BE NO DIFFERENCE in work and tool pickup procedure between probe or no-probe!
    In fact, that is the PRIMARY reason I don't have a probe on my Haas VMC-s!

    MORI figured it out on the lathes, so should the idiot "programmers" at Haas.

    But to answer your question, your Work Z offset ( Z-workshift) should NEVER be 0! ( If it is, you're either doing it wrong or should run and get a lotto ticket)

  17. #13
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,271
    Post Thanks / Like
    Likes (Given)
    915
    Likes (Received)
    512

    Default

    Thanks, everyone! It sounds like we are all on the same page...I just got spooked a bit when I read what I read in that book . Yes - on the two machines we have that do not have probes we touch off every tool to the top of the work on every set up. It's not that big of deal because most jobs run for at least a week, but I understand that loss of efficiency compared to what I consider to be the "proper" gage line method we use on all the other machines. Thanks, again!

  18. #14
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,615
    Post Thanks / Like
    Likes (Given)
    1687
    Likes (Received)
    2181

    Default

    Quote Originally Posted by Nerdlinger View Post
    I just got spooked a bit when I read what I read in that book
    I wouldn't pay much attention to that book. Years ago I bought a copy, because the word was that it was the book to read if you wanted to get good. I probably opened my copy three or four times. I haven't seen it for years, and I don't really care where it went. I have a similar opinion of that book to the machinery's handbook. A huge expensive tome, filled with not very useful information.

    My indifference to the CNC Programming Handbook is the reason I bought Sinha's book instead of Smid's when I wanted to learn more about macro programming. In retrospect I think that was a very good choice.

  19. Likes Nerdlinger liked this post
  20. #15
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    220
    Post Thanks / Like
    Likes (Given)
    558
    Likes (Received)
    57

    Default

    Smid sounds like one of those guys who learned programming but never actually touched a machine.
    Setting the work offset to zero and touching off tools on every new job even if you never moved them is insanity.

  21. #16
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,901
    Post Thanks / Like
    Likes (Given)
    604
    Likes (Received)
    346

    Default

    Quote Originally Posted by Fancuku View Post
    Smid sounds like one of those guys who learned programming but never actually touched a machine.
    Setting the work offset to zero and touching off tools on every new job even if you never moved them is insanity.
    Absolutely.

    Set tool length offsets as a positive distance from spindle gauge line to tool tip and the offsets will remain usable for any number of programs.

    There are several methods of accomplishing this (including mine)so I'm not going to wade through them again.

  22. #17
    Join Date
    Dec 2012
    Location
    Se Ma USA
    Posts
    2,238
    Post Thanks / Like
    Likes (Given)
    180
    Likes (Received)
    1218

    Default

    And if you use Mazatrol you measure a tool and done. Break it and measure the replacement. Go back to work on any part.
    I know, sorry, I'll let myself out...........

  23. #18
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,581
    Post Thanks / Like
    Likes (Given)
    853
    Likes (Received)
    692

    Default

    Quote Originally Posted by Nerdlinger View Post

    I imagine this is just one of those, "more than one way to skin a cat" scenarios but I am inquisitive by nature and tend to suffer from tunnel vision so I wanted to ask if there IS a generally-accepted way of setting top of stock and tool length out there or if it is more of a, "one guy tells you thing and one guy tells you another" deal.

    Thank you!
    Smid isn't wrong, and in fact, it's how I set up mills for years. However I learned a pretty good trick when I worked for a MTB. On mills that didn't have probes, you would set all the tools off a 1-2-3 block on the table. Then, measure from the top of the workpiece to the block and input that into the work coordinate "Z". Now, when you have a different job and say, the tools were the same, you just measure the height to the block and the machine is set rather than touching off tools individually again. Kinda like a lathe setup in a mill. Seems to work OK.

    Spindle and tool probes however, are largely making this obsolete, excepting on older machines.

  24. Likes mhajicek liked this post
  25. #19
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,615
    Post Thanks / Like
    Likes (Given)
    1687
    Likes (Received)
    2181

    Default

    Quote Originally Posted by DouglasJRizzo View Post
    Smid isn't wrong, and in fact, it's how I set up mills for years. However I learned a pretty good trick when I worked for a MTB. On mills that didn't have probes, you would set all the tools off a 1-2-3 block on the table. Then, measure from the top of the workpiece to the block and input that into the work coordinate "Z". Now, when you have a different job and say, the tools were the same, you just measure the height to the block and the machine is set rather than touching off tools individually again. Kinda like a lathe setup in a mill. Seems to work OK.

    Spindle and tool probes however, are largely making this obsolete, excepting on older machines.
    This is effectively what you're doing when you use a height setter and a haimer, except the height setter + haimer is easier, quicker, and more accurate.

  26. Likes mhajicek, DouglasJRizzo liked this post
  27. #20
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,649
    Post Thanks / Like
    Likes (Given)
    1008
    Likes (Received)
    3191

    Default

    In the very early 80s when I first stood in front of a VMC, the guy doing the training taught the “touch each tool to the part” method and always leave the fixture offset for Z at 0. Not knowing any better at the time I blindly followed what was taught. This was on a machine with an indexer so I was setting different tool offsets for each face! Thankfully it only held 20 tools and there were 99 offsets.

    After a while I got to thinking it was a waste of time so started trying different things. First thing I did was touch just one tool to the new workpiece and note the difference and then just incrementally adjust the offsets for the remaining tools. Was noticeably faster than touching all the tools.

    Then I started wondering why the control had a Z fixture offset when I was told to always leave it 0. Started playing around with small numbers in there to see what happened and man did the lights come on. Started setting tools to a set block and setting the fixture offset as the difference between the set block and the 0 face of the part.

    Thought I was a genius and had sussed out a great secret in how to improve CNC operations. Then a few years later, discovered that other shops were doing the same thing. My balloon was quickly popped.


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
  •