562,272 active members*
2,589 visitors online*
Register for free
Login
Page 1 of 5 123
Results 1 to 20 of 83
  1. #1
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Work offset misbehaving.

    OK, so I have a weird problem.

    I'm making a mill part that I have made thousands of. (VF2SS)
    I use 3 work offsets on it, G54, 55, and 56.
    Different features have different Datums, and G56 is simply used to center some engraving on the part.

    I set the job up today, and when I run the first part, I always start with all three offsets the same in X, Y, and Z.
    So, I run it, and none of the G56 engravings are cut!

    I try again, and see that it is cutting air.
    Z is off by .750 -1"
    WTF?

    I check the offsets, they all match.
    Re probe the engraving tools.
    Try again.
    No love, still off.

    So I re calibrate everything, tool probe and work probe.
    Probe the tools, and the part, try again.
    Still no good.
    Cutting air.

    So, I figure what the hell, and change the offset from G56 to G54 and give it a go.
    Cuts fine!

    Some how, some way, when it calls up G56, it is adding a number to the Z offset for G56.
    But only G56.

    Anybody have any ideas?

  2. #2
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    I just nuked the whole work offset table, and started over.
    It's behaving now, but I'm still curious WTF...

  3. #3
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    I just nuked the whole work offset table, and started over.
    It's behaving now, but I'm still curious WTF...
    In the G56Z 0ffset you must have had a different number set from what the G54 was using
    Mactec54

  4. #4
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    No sir.
    All 3 offsets were the same.
    In x, y, and z!
    I wouldn’t have posted here if it was behaving as one would expect it to behave!

  5. #5
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    No sir.
    All 3 offsets were the same.
    In x, y, and z!
    I wouldn’t have posted here if it was behaving as one would expect it to behave!
    It is obvious that (1) of the offsets was incorrect some were, either in the Tool Table or the work 0ffset Table, clearing them out and resetting them solved the problem so (1) must have been incorrectly set

    The machine will do what you tell it to do, it's easy to make a mistake, find where you went wrong as it will happen again, you were lucky it was cutting air, as it could have been the other way and crashed the machine spindle / tool into the job
    Mactec54

  6. #6
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    I am lucky, yes.
    But no, all of the offsets were correct.
    Haas was stumped by this as well.
    Nobody could figure out what was going on.
    They kept saying 'well, obviously one of the offsets is different'
    But they weren't.
    So, I sent pics and video of the offsets, and the behavior...
    I have no reason to lie here bud.
    I was just looking to see if anyone else had encountered such an issue...
    My dumb robot was NOT doing what it was told...
    Here's the offset picture I sent to Haas.
    There clearly was a glitch in the offset table, but not anywhere visible to us.
    Everything was probed, and re probed.
    Probes were calibrated and everything was probed again...
    Running the tool @ G54 cut metal, changing nothing but the G54 to G56 in the program, and it cut air. (G55 cut correctly too, I tried it)
    Close to 1" off.
    54 and 56 were the same in the offset table.
    Attachment 486082

  7. #7
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    I am lucky, yes.
    But no, all of the offsets were correct.
    Haas was stumped by this as well.
    Nobody could figure out what was going on.
    They kept saying 'well, obviously one of the offsets is different'
    But they weren't.
    So, I sent pics and video of the offsets, and the behavior...
    I have no reason to lie here bud.
    I was just looking to see if anyone else had encountered such an issue...
    My dumb robot was NOT doing what it was told...
    Here's the offset picture I sent to Haas.
    There clearly was a glitch in the offset table, but not anywhere visible to us.
    Everything was probed, and re probed.
    Probes were calibrated and everything was probed again...
    Running the tool @ G54 cut metal, changing nothing but the G54 to G56 in the program, and it cut air. (G55 cut correctly too, I tried it)
    Close to 1" off.
    54 and 56 were the same in the offset table.
    Attachment 486082
    Something must have happened with the Tool 0ffset then, by changing it to G54 changed something to how it needed to work.

    Post the original Program there may be something that through it off, before the G56. (Just cut and paste it here)
    Mactec54

  8. #8
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    It's a rather long program, but I'll go copy the important bits.
    FWIW, the program is out there running right now.
    Never changed it.
    Just cleared the offset table, and re probed.
    Set the program back to G56, and got after it. (only change to the program was moving between G56 and 54/55)
    Electronics glitch sometimes...

  9. #9
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    Here's the end of the previous tool, and the beginning of the next tool, at G56.

    G1 X-4.0101
    X-4.0131
    G3 X-4.0158 Y.0119 I0. J-.0106
    G1 G40 X-4.0145 Y.0068
    G0 Z.5
    M89
    M5
    G53 G0 G90 Z0.
    M01

    ( CUT NAME )
    T14 M6 ( .030 BULL ENDMILL )
    M88
    T12
    G0 G90 G17 G56 X-3.5562 Y0. A79.39 S15000 M42
    M3
    G43 H14 Z.716
    Z.257
    G1 Z.217 F9.
    Z.2139 A63.474
    X-3.5914 Z.212
    X-3.5663 Z.2107
    X-3.5562
    A79.39
    A63.474
    X-3.5914
    G0 Z.257
    X-3.5562 A71.432
    G1 Z.217
    X-3.5836 Z.2156
    X-3.5562 Z.2141
    X-3.5836 Z.2127
    X-3.5562 Z.2112
    X-3.5665 Z.2107
    X-3.5836
    X-3.5562
    G0 Z.257
    X-3.664 A79.39
    G1 Z.217
    X-3.6289 Z.2152
    Z.212 A63.474
    X-3.6539 Z.2107
    X-3.664
    X-3.6289
    A79.39
    X-3.664
    G0 Z.257

  10. #10
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    Here's the end of the previous tool, and the beginning of the next tool, at G56.

    G1 X-4.0101
    X-4.0131
    G3 X-4.0158 Y.0119 I0. J-.0106
    G1 G40 X-4.0145 Y.0068
    G0 Z.5
    M89
    M5
    G53 G0 G90 Z0.
    M01

    ( CUT NAME )
    T14 M6 ( .030 BULL ENDMILL )
    M88
    T12
    G0 G90 G17 G56 X-3.5562 Y0. A79.39 S15000 M42
    M3
    G43 H14 Z.716
    Z.257
    G1 Z.217 F9.
    Z.2139 A63.474
    X-3.5914 Z.212
    X-3.5663 Z.2107
    X-3.5562
    A79.39
    A63.474
    X-3.5914
    G0 Z.257
    X-3.5562 A71.432
    G1 Z.217
    X-3.5836 Z.2156
    X-3.5562 Z.2141
    X-3.5836 Z.2127
    X-3.5562 Z.2112
    X-3.5665 Z.2107
    X-3.5836
    X-3.5562
    G0 Z.257
    X-3.664 A79.39
    G1 Z.217
    X-3.6289 Z.2152
    Z.212 A63.474
    X-3.6539 Z.2107
    X-3.664
    X-3.6289
    A79.39
    X-3.664
    G0 Z.257
    Thats pretty messed up format for a Haas machine, where was the G56 placed
    Mactec54

  11. #11
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    What’s messed up about it?
    Tool change.
    Through spindle coolant
    Stage the next tool
    Move to position (the g56 is there) set rpm, etc.
    Fire up the spindle.
    Move to clearance plane
    Move to retract plane
    Start cutting.
    Seems pretty standard.
    It could be done a little differently I suppose, but the post spits it out this way, and it’s easy to edit.

  12. #12
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    What’s messed up about it?
    Tool change.
    Through spindle coolant
    Stage the next tool
    Move to position (the g56 is there) set rpm, etc.
    Fire up the spindle.
    Move to clearance plane
    Move to retract plane
    Start cutting.
    Seems pretty standard.
    It could be done a little differently I suppose, but the post spits it out this way, and it’s easy to edit.


    Then you need to have the post changed, or change it your self

    G56 Should be on a line by itself can't be used in a string like that, it can be used combined with some codes but not like you have it, so it is always best to have any 0FFSET change on its own line


    G53 G0 G90 Z0. What is this for the tool change call T14M6 takes it to this position.
    M01

    G0 G90 G17 G56 X-3.5562 Y0. A79.39 S15000 M42 This line is very messed up the G90 and G17 is most likely not needed unless it was on a different plane from the previous Tool being run, these are default codes that the control already has, look at your control and see what codes are on the screen to the right go through them this is where you can see if your 0FFSET is working, it will show the change from G54 (Default) to the G56 if this change does not take place then it has not seen the programed 0FFSET you want to use which is what happened in your case

    If your through coolant is the only coolant being controlled, that to may be controlled by the M6 and it may not need to be in the program just look at the control to see if it is in the default codes

    G0 G90 G17 G56 X-3.5562 Y0. A79.39 S15000 M42, the control would not read the G56 in this line I'm surprised Haas did not pick this coding problem, this is not normal to program the G56 in a string like this.

    (M3) M3 on a different line to the spindle speed call is nuts

    This will work the G56 can be in combination with other codes but not preprogramed like you have it

    G56
    M42M3S15000
    G0 G90 G17 G56 X-3.5562 Y0 A79.39. (The G17 and G90 is most likely redundant)
    Mactec54

  13. #13
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    I could see putting the work offset in a line by itself, but all the machines have run like this for years! They absolutely read that line.

    G53 G0 G90 Z0. is a safety line. Why not? I don't pay by the line of code. Z, go home... If I am running in optional stop mode, I want the z away from the part.

    G90 and G17 absolutely aren't necessary repeatedly in the program. But again, why not build in redundancies?

    And no, that is NOT what happened in my case. My case was a machine glitch. The machine did in fact say it was at G56. Even if it hadn't and it thought it was at G54, 54 and 56 were the same.

    I like controlling my coolant myself. And often, especially on these engraving cutters, I turn on both M88 and M8. I get a pretty large bump in tool life cutting Titanium that way.

    I have two Haas mills, a 2012 and an NGC, both of them read the work offset changes in the G0 line, and have for years.
    I see the logic in moving it to its own line, earlier though.

    I think the M3 moved to a different line some years ago when I had the post fixed so that the spindle didn't come on at the toolchange for tapping.
    The spindle would come on after the toolchange, then position itself, then turn off, clock itself and tap.
    It was faster to only have it turn on to actually tap.
    I never paid attention to the M3 being on a different line that the RPM, because it works fine.

    I'll look at the post when I have a little time, and streamline some stuff.

    But here, for your perusal, are a couple of pics of my other machine, not the next gen control.
    Very similar startup line, G55 is on the line with the move, AND the spindle on command!
    You will notice that it does indeed pick up the G55. It started at G54...
    Attachment 486100
    Click image for larger version. 

Name:	after.jpg 
Views:	3 
Size:	147.3 KB 
ID:	486102

  14. #14
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    Cleaned up my post for the old mill a bit...

    Was
    %
    O1111 ( BACKSPACERS STEP 2 )
    (DATE - 11-12-22-13:00)
    (MASTERCAM - HAAS VMC)

    (T1 3/8 FLAT ENDMILL, .375 DIA)
    (T4 1/8 X .040" CHAMFER TOOL, .125 DIA)

    G00 G17 G20 G40 G80 G90
    G53 G0 G90 Z0.
    T1 M6 ( 3/8 FLAT ENDMILL )
    G00 G90 G54 X-.2847 Y-.7289 S6000 M3
    M8
    G43 H1 Z1.
    G94
    Z.1
    G01 Z-.05 F60.
    X-.2689 Y-.4794 F48.

    Is now
    %
    O1111 ( BACKSPACERS STEP 2 )
    (DATE - 11-12-22-13:01)
    (MASTERCAM - HAAS VMC)

    (T1 3/8 FLAT ENDMILL, .375 DIA)
    (T4 1/8 X .040" CHAMFER TOOL, .125 DIA)

    G00 G17 G20 G40 G80 G90
    G53 G0 G90 Z0.
    T1 M6 ( 3/8 FLAT ENDMILL )
    G54
    G00 X-.2847 Y-.7289
    S6000 M3
    M8
    G43 H1 Z1.
    G94
    Z.1
    G01 Z-.05 F60.
    X-.2689 Y-.4794 F48.

    Still a redundant G90 in there, but I like that Z safety line, I'm gonna keep it.

  15. #15
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    I could see putting the work offset in a line by itself, but all the machines have run like this for years! They absolutely read that line.

    G53 G0 G90 Z0. is a safety line. Why not? I don't pay by the line of code. Z, go home... If I am running in optional stop mode, I want the z away from the part.

    G90 and G17 absolutely aren't necessary repeatedly in the program. But again, why not build in redundancies?

    And no, that is NOT what happened in my case. My case was a machine glitch. The machine did in fact say it was at G56. Even if it hadn't and it thought it was at G54, 54 and 56 were the same.

    I like controlling my coolant myself. And often, especially on these engraving cutters, I turn on both M88 and M8. I get a pretty large bump in tool life cutting Titanium that way.

    I have two Haas mills, a 2012 and an NGC, both of them read the work offset changes in the G0 line, and have for years.
    I see the logic in moving it to its own line, earlier though.

    I think the M3 moved to a different line some years ago when I had the post fixed so that the spindle didn't come on at the toolchange for tapping.
    The spindle would come on after the toolchange, then position itself, then turn off, clock itself and tap.
    It was faster to only have it turn on to actually tap.
    I never paid attention to the M3 being on a different line that the RPM, because it works fine.

    I'll look at the post when I have a little time, and streamline some stuff.

    But here, for your perusal, are a couple of pics of my other machine, not the next gen control.
    Very similar startup line, G55 is on the line with the move, AND the spindle on command!
    You will notice that it does indeed pick up the G55. It started at G54...
    Attachment 486100
    Click image for larger version. 

Name:	after.jpg 
Views:	3 
Size:	147.3 KB 
ID:	486102
    The M6 will turn the spindle on with your Haas control so it does not matter where the M3 is or placed as it is redundant

    Most program this by habit and don't have a good understanding of how a control works most of the time poorly formatted code works so nobody changes anything until it does not work.

    What is a G0 for, a Rapid move so it should be used correctly with an X Y Z Etc. move

    A Work 0FFSET should be the first in the line if used with other codes and in this order, you have to think how the control works

    G56G90 G0X----- this is correct way to use it if doing it like you are
    G54G1Y-----X------F20.

    Your redundant code is just a programing habit, and the safety line is ridiculous

    G53 Non-Modal Machine Coordinate Selection (Group 00)
    This code temporarily cancels work coordinate offsets and uses the machine coordinate system. This code will also ignore tool offsets. In the machine coordinate system, the zero point for each axis is the position where the machine goes when a Zero Return is performed. G53 will revert to this system for the block in which it is commanded.

    So, you should use a G53 at the end of a program not before a Tool Change

    Then came the M01 so the coordinate would have still been canceled at this point

    So, when you pressed start, the first code it saw was G0 moves,
    Mactec54

  16. #16
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    M6 doesn't turn on the spindle in any machine that I own.
    And I am happy about that.
    I see no reason I would even desire that.

    I can't see why a Z safety line is ridiculous either.
    I insist on my machine being at Z home before any XY motion happens.
    If T1 was called out, and T1 was already in the machine, it would just start moving in XY.
    If the machine wasn't parked in a safe position, this could be catastrophic.
    So, I have it in the header...
    It is also at the end of every operation so that the tool clears the part when running in optional stop mode.
    Hell, I'm tempted to also add it after the toolchange.
    I don't have good help, so why not program around that?
    There's no fee for extra lines of code.

    An M1 without a Z home move first makes no sense to me.
    I often re-run the same tool, especially when setting up a new part.
    Do people really use M1 without a Z homing move first?
    The the machine just stops with the tool down?
    Why would that be desirable?

    I used to use G28 to clear Z, but I don't like ever being in incremental mode, so I got rid of it, and went to G53.

  17. #17
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    M6 doesn't turn on the spindle in any machine that I own.
    And I am happy about that.
    I see no reason I would even desire that.

    I can't see why a Z safety line is ridiculous either.
    I insist on my machine being at Z home before any XY motion happens.
    If T1 was called out, and T1 was already in the machine, it would just start moving in XY.
    If the machine wasn't parked in a safe position, this could be catastrophic.
    So, I have it in the header...
    It is also at the end of every operation so that the tool clears the part when running in optional stop mode.
    Hell, I'm tempted to also add it after the toolchange.
    I don't have good help, so why not program around that?
    There's no fee for extra lines of code.

    An M1 without a Z home move first makes no sense to me.
    I often re-run the same tool, especially when setting up a new part.
    Do people really use M1 without a Z homing move first?
    The the machine just stops with the tool down?
    Why would that be desirable?

    I used to use G28 to clear Z, but I don't like ever being in incremental mode, so I got rid of it, and went to G53.
    Yes, agree G28 G91 can be a disaster that's why most never use it

    So, you don't need that safety line, the last Z move in your previous program should be used to give you the safe clearance you need for any X Y axis movement, if using the same tool

    G0 Z.5 (From your posted program, this can be the safe Z axis move G0Z3. or whatever number you want to clear your work) No G53 line needed

    G0 Z.5 (Z axis clearance move here, and you don't need the G53 Line)
    M89
    M5
    G53 G0 G90 Z0.
    M01


    So, if you were to want to use the G53 after you have already done a G0 Z--- move like in your program, you would write it like this

    G53Z0. nothing more needed no G0 or G90 required why because you are already using absolute G90, and you used a G0 call just before the G53 call so both codes are Modal so are active until changed

    M01 is in your program you posted which is ok if you wanted to stop the machine to check something
    Mactec54

  18. #18
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    Ahh, I see where you are coming from.
    Ideal world!
    I don't live in ideal world!
    I have dumb oafs working for me.
    Myself included.
    I trust no modal commands if there is not a compelling reason to trust them.
    i haven't been presented any compelling reasons yet.

    I can't presume that whatever the machine was doing last left in in absolute, or G0.
    Could have been something run real quick in another vise in MDI.
    Then starting mid program on the programmed part.
    Unless there is a demonstrable reason why having G0 and G90 in the G53 Z0. is bad, I don't see the harm.

    And I want Z home before any XY motion. There's often 2 parts, and a 4th axis in my machine.
    Z home clears them all, always.
    So, on my machines, z goes home.

    Hand programming, I do things differently.
    But 99% of my programming comes out of Mastercam.
    It's no skin off my nose for it to post extra, redundant lines.
    I'm still tempted to add it after the Toolchange! I see opportunity for an accident without it. (tool on the wrong side of a different part/4th axis/etc... and starts mid program with the called tool already in the spindle.)

    If it was there, it would just be a line that did nothing 99.999% of the time... And that's OK. That one time it stops a crash would make a lot of redundancies worth it.

    My rudimentary post editing skills make it a lot easier to have a "generic" line that gets dropped in places.
    With more post coding skill I'm sure it's possible to have it do more specific tasks at different times
    But, I don't have those skills, nor do I have an issue with there being redundancies in my programs..

  19. #19
    Member
    Join Date
    Jan 2005
    Posts
    14718

    Re: Work offset misbehaving.

    Quote Originally Posted by HayreAss View Post
    Ahh, I see where you are coming from.
    Ideal world!
    I don't live in ideal world!
    I have dumb oafs working for me.
    Myself included.
    I trust no modal commands if there is not a compelling reason to trust them.
    i haven't been presented any compelling reasons yet.

    I can't presume that whatever the machine was doing last left in in absolute, or G0.
    Could have been something run real quick in another vise in MDI.
    Then starting mid program on the programmed part.
    Unless there is a demonstrable reason why having G0 and G90 in the G53 Z0. is bad, I don't see the harm.

    And I want Z home before any XY motion. There's often 2 parts, and a 4th axis in my machine.
    Z home clears them all, always.
    So, on my machines, z goes home.

    Hand programming, I do things differently.
    But 99% of my programming comes out of Mastercam.
    It's no skin off my nose for it to post extra, redundant lines.
    I'm still tempted to add it after the Toolchange! I see opportunity for an accident without it. (tool on the wrong side of a different part/4th axis/etc... and starts mid program with the called tool already in the spindle.)

    If it was there, it would just be a line that did nothing 99.999% of the time... And that's OK. That one time it stops a crash would make a lot of redundancies worth it.

    My rudimentary post editing skills make it a lot easier to have a "generic" line that gets dropped in places.
    With more post coding skill I'm sure it's possible to have it do more specific tasks at different times
    But, I don't have those skills, nor do I have an issue with there being redundancies in my programs..
    I can see where you are coming from, but you can't get away from the fact that when you are using your cam software, you write this number in there G0Z.5 this can be the safety line, I use it all the time after an operation you can set that in your created program to any number you want to clear a potential Tool Crash, this you have full control of.

    G53G90G0Z0. (Note the correct format for its use)
    There is nothing wrong with using the full code string, I was showing how it can be used,

    I use it like this G53Y0. on most operations it can of cause have a X in there, if you need the table to line up to get the parts out easy, it can be used like this also

    G53G90G0Z0. this can always be set to any number you want within the Z axis travel range
    G53Y0.X5.

    G0Z3. (This does the same thing as above which you have full control of in your cam program, and can be at the end of any operation
    M9
    M5
    G53Y0.
    M30
    Mactec54

  20. #20
    Registered
    Join Date
    Jun 2006
    Posts
    102

    Re: Work offset misbehaving.

    In Mastercam, that Z.5 is my clearance plane.
    I use it for several things.
    A visual check for my guys to run an operation in single step mode and see that they set everything correctly. It's usually 1" above zero.
    Clearance for getting around clamps when I have parts clamped to a plate.
    And on some parts, where the depth is critical, we actually run the program to that point and stop it. Set the Operator Z zero there, and check it with a gage pin. We can then jog the tool up or down until it's perfect, see where we arand adjust the tool offset.
    It already serves a purpose in my world.

    I did change the post yesterday to format the line as G53 G90 G0 Z0. Because I am a fan of things being in a sensible order, even if it doesn't make a difference.

    The end of my programs send the table to yet a different zero. One that we set to be easy to swap out whatever part we are running.

    G01 X-.0216
    G03 X.7126 Y.3309 I0. J1.9885
    G03 X.7411 Y.3468 I-.0461 J.1161
    G01 G40 X.7652 Y.3647
    G00 Z1.
    M83
    M9
    M5
    G53 G90 G0 Z0.
    G00 G129 X0. Y0.
    M30
    (PUT ANOTHER PART IN THE MACHINE RIGHT NOW, JERK)
    %

    I wired a buzzer in to the machine at the M83 solenoid.
    I didn't like the way Haas changed there beep some years ago, so I figured out my own.
    Works great.

Page 1 of 5 123

Similar Threads

  1. Replies: 11
    Last Post: 12-17-2016, 04:59 AM
  2. Replies: 1
    Last Post: 05-22-2016, 10:59 PM
  3. Replies: 8
    Last Post: 09-17-2015, 04:14 AM
  4. Tool offset with work offset
    By botha.y in forum SIEMENS Sinumerik CNC controls
    Replies: 7
    Last Post: 06-04-2012, 06:31 PM
  5. Tool offset with work offset
    By botha.y in forum SIEMENS Sinumerik CNC controls
    Replies: 0
    Last Post: 05-28-2012, 09:48 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
  •