Fanuc G43.4 expected behavior.
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Oct 2018
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    5

    Default Fanuc G43.4 expected behavior.

    Hey guys. I've lurked for a while and gotten a lot of good information from here. Today the search function is failing me(or I am failing it) so I'm hoping I can get some help.

    I've been tasked with a problem to solve and I'm having trouble narrowing down my options due to some question of how tool center point control behaves on a Fanuc 31i. The machine is a Matsuura MAM72. I spent some time on the phone with applications at Matsuura, but our connection was crappy so I don't think he quite understood what I was trying to ask. I'll try to keep this simple.

    Currently we program our parts from centerline of rotation of the C axis. Those offsets are set in the common, and G54 is set to all zeroes. You will see why this is important in a minute.

    The problem:
    We're machining castings with compound curves on a 5 axis table/table machine. We're trying to machine as close to the casting floor as possible without gouging it. We have a +.05"/-.00" tolerance where the floor meets the wall.

    Casting variance is such that batch and queue doesn't make sense, nor can we really just pick a height and run. The parts are consistent to themselves, but not to each other, if that makes sense. These are production run parts, so it makes sense to invest the time into automating as much as possible.

    My solution:
    I wrote a probe routine that probes X amount of points along the surface that can't be touched with a cutter and dump the difference between nominal and actual into macro variables. I then found the average of that deviation from nominal and added .020". I dumped that number into G54 "Z".

    Now my plan is to take that average variation +.020, insert it before the tool path starts, run the tool path, and then take the variation out so I don't affect any other geometry. I can control this all inside NX so that is not a problem. There will be no hand editing.

    The probe routine does what is expected, the code to do all the offset shifts works great. Where there is some question is what is going to happen if I raise G54 Z when G43.4 is active.

    I expect that it will just run the same exact 3D tool path a little higher or lower. Which, if I am not mistaken, was what I saw on the Mazak table/table machines I used to program and run. They all used G43.4 and G68.2. I've never had to do what I'm being asked to do now though.

    My co-worker disagrees. He is using probe routines that probe the part, and choose a program to run based on material condition(deviation from nominal). While this is a great solution to a very challenging problem, he is leaving the company and I'd like to simplify it if possible. I am not as good of a programmer as he is, and I was having a little trouble following his logic.

    The other issue with his solution is that you only have as many options to handle casting variance as he's programmed. With mine you would have infinite options.

    I'm trying to get some machine time to do some R&D, but in the meantime I thought I'd bounce it off the collective knowledge of this forum and see what I come up with.

    Thanks in advance!

  2. #2
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    184
    Likes (Received)
    109

    Default

    So I'm not 100% clear on what you're exactly asking for help on, but I'll make an attempt.

    Sounds like your concerned about shifting the Z with G43.4 and having the part position properly afterwards. That will mostly depend on which variation of tool center point control (G43.4) you're using. I teach this for Mazaks but it should be identical on a Fanuc. There are 2 variants, workpiece coordinates and table coordinates. In workpiece coordinates definition, XYZ don't rotate as the table rotates in C. This means you most know the exact location of the part relative to the rotary centerlines to have it track properly. This is how most people program 5 axis machines, but it is not ideal for the exact type of situation you are facing.

    What I use/preach instead on most machines is the table coordinates system. In this definition, as you rotate the C axis XYZ will rotate along with it. Why is this beneficial? Because it means the machine automatically tracks where the part is in space, WITHOUT the part having to be on centerline. A lot of people will accomplish this with Dynamic work offsets (G54.2) or Workpiece setup error correction (G54.4), but the nature of the table coordinates system for G43.4 means it does all that automatically.

    So when I setup a trunnion machine I don't need to tram it to the center of the table or worry about where the center of my tilt is. The part can be offset a couple inches from center at any height, I let the machine figure it out. So I just probe G54 or whatever offset I want and go. As long as you have clearance you don't have to worry about it.

    It should also be mentioned that tilted working plane (G68.2) does the exact same internal calculations for 3+2 work. So again, you don't have to worry where the part is EXACTLY in the machine when you program it. You pick up your offset just like a 3 axis VMC and go. The machine will do the work of figuring out where to move.

    So back to your problem, step one would be figuring out what your machine has for 5 axis options, what they the parameters are set for, and how your CAM software is set. All 3 need to be in alignment. If the machining environment is already set for table coordinates G43.4 you can just probe your casting and shift the Z however you like. If it's not you'll need to do a little extra work, but you are on the right track.

  3. Likes LockNut liked this post
  4. #3
    Join Date
    Oct 2018
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    5

    Default

    I think you're leading me down the right track. I appreciate your response. I'm headed out to the machine to check parameters.

    I'm new at the company and there's not a whole lot of documentation on these things. How would it affect previously proven programs if I have to switch from workpiece to table coordinates?

  5. #4
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    184
    Likes (Received)
    109

    Default

    Quote Originally Posted by cellis8200 View Post
    I think you're leading me down the right track. I appreciate your response. I'm headed out to the machine to check parameters.

    I'm new at the company and there's not a whole lot of documentation on these things. How would it affect previously proven programs if I have to switch from workpiece to table coordinates?
    Previously proven programs will no longer be proven

    The actual G code output between the 2 methods is different. That's why you have to make sure the CAM system post processor, program itself AND the machine are set the same way. If they aren't it's gonna break stuff. That's always step one for me in a new system/machine.

    NX posts processors (in my experience at least) usually have a "switch" in the header code to go between workpiece and table coordinates for output.

    I would definitely try to get back in touch with Matsuura apps support again. I'm an AE myself and we do this stuff all the time, so we can guide you down the right path. Now you know some more terminology so that should help the conversation quite a bit. I imagine given Matsuura's product line most/all of their AE's will be pretty well versed in 5X programming particulars.

    Also here is a good video illustrating this stuff, in NX no less:
    YouTube

  6. #5
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    527
    Likes (Received)
    505

    Default

    CNC Hacker is correct and his explanation is one of the best I have heard. This is how I also do it and makes programming and running so much easier. Parameter #19696.5 will switch the machine to table coordinates. Of course, your machine kinematics need to be accurate also.

    Paul

  7. Likes CNC Hacker liked this post
  8. #6
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    184
    Likes (Received)
    109

    Default

    Quote Originally Posted by LockNut View Post
    CNC Hacker is correct and his explanation is one of the best I have heard. This is how I also do it and makes programming and running so much easier. Parameter #19696.5 will switch the machine to table coordinates. Of course, your machine kinematics need to be accurate also.

    Paul
    Can you tell this isn't the first time I've had this conversation with people?

  9. #7
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    527
    Likes (Received)
    505

    Default

    Quote Originally Posted by CNC Hacker View Post
    Can you tell this isn't the first time I've had this conversation with people?
    Of course, same here. I'm an applications engineer too and the hardest part is with people buying their first 5 axis machine. Most of it goes in one ear and out the other because they have heard all these wonderful things that a 5 axis can do from sales people.

    It sounds as if you might work for Mazak or a reseller for them.


    Paul

  10. #8
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    184
    Likes (Received)
    109

    Default

    Quote Originally Posted by LockNut View Post
    Of course, same here. I'm an applications engineer too and the hardest part is with people buying their first 5 axis machine. Most of it goes in one ear and out the other because they have heard all these wonderful things that a 5 axis can do from sales people.

    It sounds as if you might work for Mazak or a reseller for them.


    Paul
    That's correct. I preach the gospel of TCP/TWP all the time. Sadly it usually falls on deaf ears and people still want to run everything from the pivot point in inverse time.

    I'm lazy, my motto is make the machine do the hard work!

  11. Likes macds, barbter liked this post
  12. #9
    Join Date
    Jul 2008
    Location
    Milverton, Ontario, Canada
    Posts
    702
    Post Thanks / Like
    Likes (Given)
    207
    Likes (Received)
    310

    Default

    Quote Originally Posted by CNC Hacker View Post
    That's correct. I preach the gospel of TCP/TWP all the time. Sadly it usually falls on deaf ears and people still want to run everything from the pivot point in inverse time.

    I'm lazy, my motto is make the machine do the hard work!
    Bingo!

    Let the machine worry about where the bloody part is. That way 1 program covers it all, and no pissing around for the operator. THATS when mistakes happen.

  13. Likes barbter liked this post
  14. #10
    Join Date
    Oct 2018
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    5

    Default

    You guys are the best. TCP/TWP is how the mazaks were setup at my previous employer. This is the direction I'd like to take us since I'm the one handling the post.

  15. #11
    Join Date
    Jul 2008
    Location
    Milverton, Ontario, Canada
    Posts
    702
    Post Thanks / Like
    Likes (Given)
    207
    Likes (Received)
    310

    Default

    Its amazing how many people in "high end" shops dont understand the significance of fully utilizing tcp and twp modes.
    Shocking, actually.

    When we got the a51nx optioned with intention of adding a koma 5th down the road, I pushed HARD for tcp\twp. And got it.

    Then nobody ever used it, didnt want to understand it.... instead loading offsets into the cam software to ensure things were machined properly.

  16. #12
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Hello, in the code below we are experiencing a crash into the part on our
    Mazak Variaxis i700 trunnion that does not show up in our Powermill or Vericut simulation. It seems like it may have something to do with the G68.2 bieng used along with the G43.4 but I am not sure. Does anyone have any suggestions on what this could be? We have already sent in a support file to Autodesk and to Mazak to see what they come back with but I found this thread in a search and figured I would post it here too.

    Thanks, Mike

    ( TOOLPATH START)
    ( )
    G00 G53 Z0.0
    G00 G53 X0.0 Y0.0
    G00 A0.0 C0.0
    G01 A17.52288 C7.15583 F1500.0
    G68.2 X2.29008 Y1.17229 Z13.87545 I7.15583 J17.52288 K0.0
    G53.1
    X0.0 Y0.0 F1500.0
    G69
    G90 X2.29008 Y1.17229
    G43.4 Z13.87545 H11
    X2.29008 Y1.17229 Z13.87545
    M828( FINISHING)
    G61.1
    M43
    M46
    M08
    Z13.37545 F1500.0
    Z8.29547 F80.0
    X2.27133 Y1.32166 Z7.81867
    X2.27177 Y1.32302 Z7.81081
    X2.27232 Y1.323 Z7.8026
    X2.27298 Y1.32152 Z7.7944
    X2.2737 Y1.3186 Z7.78659
    X2.27446 Y1.31442 Z7.77954
    X2.27522 Y1.30925 Z7.77351
    X2.27594 Y1.30388 Z7.76823 A17.47183 C7.15468
    X2.27683 Y1.296 Z7.76111 A17.39855 C7.15713
    X2.27842 Y1.28126 Z7.74894 A17.26435 C7.16356

  17. #13
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    184
    Likes (Received)
    109

    Default

    Check 2 parameters first.

    F86 bit 6 = 1
    Selection of rotary axis reference position for tool tip point control
    0: Position during the start of tool tip point control
    1: Position with the rotary axis at 0 degrees


    F144 bit 1 = 1
    Selection of table rotary axis reference position for inclined-surface machining
    0: Table rotary axis start position as the reference
    1: Table rotary axis 0-degree position as the reference

    If these are set to 0,the C zero is taken from the incremental staring position NOT your actual C zero in the work offset. So like in your case were you have the C at 7-ish degrees when it invokes G68.2, it may rotate it again. First thing I would check.

    Next is F85 bit 2:
    Sets the type of coordinate system for controlling the tool tip point.
    0: The table coordinate system that rotates according to the particular
    rotation of the C-axis is defined as the programming coordinate
    system.
    1: The work coordinate system is defined as the programming coordinate
    system.

    Make sure the machine is set to match powermill and to match vericut. If the 3 are not in agreement you will cause weird things to happen.

  18. #14
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    We looked into the parameters and the settings are as follows

    F86 bit 6= 1

    F144 bit 1 = 0

    F85 bit 2 = 0


    Would you happen to know where in the post processor and the vericut control that I can look to check these settings or do I need to contact each of them?

    Thanks for the information on this,
    Mike B

  19. #15
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    184
    Likes (Received)
    109

    Default

    I do not, but I would set F144 bit 1 to a 1 and try it again. Good chance it solves it.

  20. #16
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Ok, thanks again for your help on this. We are going to try this in the morning when the current part is finished.

    Mike B

  21. #17
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    527
    Likes (Received)
    505

    Default

    Quote Originally Posted by mikeb80 View Post
    Hello, in the code below we are experiencing a crash into the part on our
    Mazak Variaxis i700 trunnion that does not show up in our Powermill or Vericut simulation. It seems like it may have something to do with the G68.2 bieng used along with the G43.4 but I am not sure. Does anyone have any suggestions on what this could be? We have already sent in a support file to Autodesk and to Mazak to see what they come back with but I found this thread in a search and figured I would post it here too.

    Thanks, Mike

    ( TOOLPATH START)
    ( )
    G00 G53 Z0.0
    G00 G53 X0.0 Y0.0
    G00 A0.0 C0.0
    G01 A17.52288 C7.15583 F1500.0
    G68.2 X2.29008 Y1.17229 Z13.87545 I7.15583 J17.52288 K0.0
    G53.1
    X0.0 Y0.0 F1500.0
    G69
    G90 X2.29008 Y1.17229
    G43.4 Z13.87545 H11
    X2.29008 Y1.17229 Z13.87545
    M828( FINISHING)
    G61.1
    M43
    M46
    M08
    Z13.37545 F1500.0
    Z8.29547 F80.0
    X2.27133 Y1.32166 Z7.81867
    X2.27177 Y1.32302 Z7.81081
    X2.27232 Y1.323 Z7.8026
    X2.27298 Y1.32152 Z7.7944
    X2.2737 Y1.3186 Z7.78659
    X2.27446 Y1.31442 Z7.77954
    X2.27522 Y1.30925 Z7.77351
    X2.27594 Y1.30388 Z7.76823 A17.47183 C7.15468
    X2.27683 Y1.296 Z7.76111 A17.39855 C7.15713
    X2.27842 Y1.28126 Z7.74894 A17.26435 C7.16356
    First, TWP is turned off before TCP is turned on. Totally legal and this is my preferred way of starting a 5 axis toolpath. TWP before TCP is considered a safety move. It gets the tool safely out over the part after rotation and is then turned off. All of my posts do this. This avoids ramping the tool down towards the part with TCP turned on and avoids unpredictable approaches. Another thing, simulating in your CAM system is no guarantee of safe approaches and retracts once the code is in the machine.

    Paul

  22. Likes CNC Hacker, cameraman liked this post
  23. #18
    Join Date
    Oct 2007
    Location
    Norway
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    5

    Default

    Sorry to hijack the thread, but I see that there are some knowledgeable peeps in 5-axis machining here

    We use G43.4 TCP (table coordinate system) for 4/5-axis simultaneous machining and a master/slave work offset macro for 3+2 machining on a 5-axis table-table VMC. (Master work offset is set in a fixed position of B- and C-axis (usually B0 C0) and a slave work offset is calculated for any orientation other than this.

    The machine runs production series of parts with tight true position tolerances.

    One problem we run into is that as the machine axes drift from temperature changes, the machine kinematics stored in parameters #19700-#19705 are no longer accurate. The Y-axis in the machine grows about 0.02 mm (0,000787 in) over 12-hours of machining, and the stored kinematics are only accurate while the machine temperature is the same as when kinematics were measured. 0.02 mm may not be a lot, but when you are trying to hold 0.1 mm true position this eats up much of the tolerance in Y-axis drift alone.

    I am curious about how other shops that does 5-axis machining deal with this? We are able to hold closer tolerances when we don't use functions like TCP/TWP because of this.

    The machine is a Mori Seiki NMV with a Fanuc F31iA5 control.

  24. Likes cameraman liked this post
  25. #19
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    527
    Likes (Received)
    505

    Default

    Quote Originally Posted by Denim View Post
    Sorry to hijack the thread, but I see that there are some knowledgeable peeps in 5-axis machining here

    We use G43.4 TCP (table coordinate system) for 4/5-axis simultaneous machining and a master/slave work offset macro for 3+2 machining on a 5-axis table-table VMC. (Master work offset is set in a fixed position of B- and C-axis (usually B0 C0) and a slave work offset is calculated for any orientation other than this.

    The machine runs production series of parts with tight true position tolerances.

    One problem we run into is that as the machine axes drift from temperature changes, the machine kinematics stored in parameters #19700-#19705 are no longer accurate. The Y-axis in the machine grows about 0.02 mm (0,000787 in) over 12-hours of machining, and the stored kinematics are only accurate while the machine temperature is the same as when kinematics were measured. 0.02 mm may not be a lot, but when you are trying to hold 0.1 mm true position this eats up much of the tolerance in Y-axis drift alone.

    I am curious about how other shops that does 5-axis machining deal with this? We are able to hold closer tolerances when we don't use functions like TCP/TWP because of this.

    The machine is a Mori Seiki NMV with a Fanuc F31iA5 control.
    What I see a lot of shops do is to do a kinematics check periodically throughout the day or after certain operations like roughing. As the machine warms up, yes, the kinematics are no longer totally valid. Depends on your part tolerances, height of part from center of rotation and a host of other factors. I tell people that kinematics maintenance is part of every day machine maintenance. Most don't listen. 5 axis is a whole new ball game and nothing close to 3 axis milling. Order of magnitude harder to keep tabs on everything. All of this should become part of periodic maintenance or in process maintenance.
    Mori should have a routine in the machine for running a kinematics check and to update the parameters after. Our machines do and I know the newer Moir's do also. If you haven't learned about that, I suggest you ask about it.


    Paul

  26. Likes Denim liked this post
  27. #20
    Join Date
    Oct 2007
    Location
    Norway
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    5

    Default

    Quote Originally Posted by LockNut View Post
    What I see a lot of shops do is to do a kinematics check periodically throughout the day or after certain operations like roughing. As the machine warms up, yes, the kinematics are no longer totally valid. Depends on your part tolerances, height of part from center of rotation and a host of other factors. I tell people that kinematics maintenance is part of every day machine maintenance. Most don't listen. 5 axis is a whole new ball game and nothing close to 3 axis milling. Order of magnitude harder to keep tabs on everything. All of this should become part of periodic maintenance or in process maintenance.
    Mori should have a routine in the machine for running a kinematics check and to update the parameters after. Our machines do and I know the newer Moir's do also. If you haven't learned about that, I suggest you ask about it.


    Paul
    Thanks for your reply, great info. The machine has two routines for measuring the kinematics actually, Mori Seikis own and Renishaw Axi-Set. We measure the kinematics once in a while, but have never done it periodically through the day. Maybe we have to dedicate one of the pallets to the measuring ball used in the kinematic measurement so the operators can run it easily by themselves.

    Are other controls (Heidenhain, Siemens etc.) better at this than Fanuc? I have been told that these have better volumetric 3D thermal compensation features which should make them more accurate at different machine temperatures.


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
  •