CNC lathe tool and work offsets


Results 1 to 20 of 20

Thread: CNC lathe tool and work offsets

  1. #1
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default CNC lathe tool and work offsets

    I could use some help setting up my cnc lathe. I've worked with Machining centers for a long time, but am new to lathes. What I am having trouble with is - how do you set x,z zero for the work offset (i.e. G54) ? I have heard some comments about using a reference tool, but do not understand it completely. Just about everytime I have programmed a mill, I set the x,y zero to the part zero then touch off all the tools in Z and ready to go. Lathes aren't the same, obviously. The machine we have is a Daewoo Puma 6-HS with the Fanuc 10T. Any help and insight will be appreciated.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Jun 2005
    Location
    USA
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default

    This is the method I use to touch off tools, hope it helps. At home or reference position origin all. Look at the incremenal position numbers, they should be zero. Move the tool to the part and position tool at z 0.0 on the part write down that number. take a cut on the diameter write down that number, measure the part and add to the x number. Use theses numbers in a g50 line at the beginning of your program. Your tool offsets will be zero to start and you can make small adjustments from there.



  3. #3
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default cont.....

    That is sort of the same way I go about starting out on mach. centers. First I home the machine and then set the absolute position for x,y to zero. I usually do this by setting the offset in G54 to zero and then MDI input the G54 X0 Y0. With no move commanded, this just changes the displays for x,y to zeros. Then I go find part zero (edge finder, indicator, etc) and whatever the display reads is what goes in the G54 offset. I would like to do the same thing with this lathe, but after homing I MDI input the G54 X0 Y0 with no G1 or G0 and the machine started moving - much to my surprise. After hitting feed hold and reset, I went and checked the G54 offset and X, Z were both set to zero. Can anyone explain, first off why the axis movement with no G0 or G1 commanded? Secondly, I understand the concept of touching off the tool in Z, but I need more clarification of the X after taking skim cut. The measurement of dia. after cut - does this number go in the G54? Also, I am assuming the tool to use is the first tool - which would then be sort of the reference tool ?? Are the rest of the tool offsets then set from this reference ?? I will be setting this lathe to run 4 different parts and would like to use the G54, 55, etc. for each part. Maybe I shouldn't be stuck in this mode of thinking but I like to keep things consistant.



  4. #4
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    The way I've got it figured, every machine establishes its home position after doing the reference point return, which is normally executed shortly after powering up the control. The home position is based in G53, which is called the "machine coordinate system".

    You can change coordinate systems by calling them by their name, G54, for instance. An X, Y or Z value with the G54 will do nothing, unless the machine is already in G01 or G00 mode from a previous command. True, it does "reset the displays to zero", as you said, but no motion occurs on your mill, because you have simultaneously called the G54 coordinate system, and then commanded a zero move within it.

    Certain lathe controls may invoke either G01 or G00 mode automatically, from a parameter setting which is read at startup.

    Now, on a mill, the Z axis G53 home position is typically "up" somewhere near the top of the stroke, and it will have an assigned value of Z0. On a lathe, the G53Z0 might logically be placed somewhere near the face of the chuck. G53X0 would logically be placed along the spindle centerline.

    So, when you command the lathe to G54 X0 Z0 (with only zeros in the G54 table), it sees that there is no difference between the G53 and G54 coordinate systems, that is, they coincide exactly. Because G00 or G01 mode is "on" by parameter perhaps, it begins a movement to that position. So, that explains why the lathe begins the movement. It would be interesting to know where G53 X0Z0 really is on your machine. You should be able to determine where this is, by what the displays readout, as soon as the machine is homed after power-up.

    On a lathe, the position that the tool turret takes when the machine homes is basically at a random location relative to what I would call a "logical" reference point on the machine. On a lathe, the spindle centerline is all important, so that is definitely logical to call the centerline X0 in the G53 coordinate system. The chuck face makes a logical Z0 in the G53 coordinate system, too, but there could be other positions that the machine maker set up to serve as G53Z0. Every machine might use different chucks, or whatever, so the factory may opt to use some other Z0 reference.

    When the tool turret is sent to "home" on a lathe, it does not return to G53 X0Z0, because, as you have discovered, the position may be inaccessible. But on a mill, all the axis do return to G53 X0Y0Z0 because the position is accessible.

    Instead, a lathe uses a predefined point called a G28 position, which is based off the G53 coordinate system. Parameter settings in the lathe setup, define what the G28 position is. It typically places the turret somewhere out in front of the chuck, back off of the X axis far enough so that turret rotation will not cause a tool to hit the workpiece. Typically, the X axis will retract far enough to stop just short of the X+ overtravel limit switch.

    G00 G28 alone will cause the turret to move to this stored position. If a value is commanded with the G28, then the turret will first move to that commanded value, and then to the home position, a dogleg sort of movement. Many guys forget that an XZ value with a G28 is an intermediate position. This is why it is common to see G91 G28 X0Z0 because then the intermediate point is incrementally "zero" away from the current position, so then the machine returns straight to the G28 stored position. On lathes, it is common for a U and W value to be interpreted as an incremental movement (no G91 required), so a lathe command might be G28 U0W0. The reason it is done this way is that you don't have to remember to set the mode back to G90, which could be a problem. But, I digress from the discussion

    Now, for your reference tool problem. You would need to know if the controller has automatic calculation of the offset, and how to make it store the values.

    When the G28 position was set up in parameters in your machine, it would make the most sense to have them correspond to the datum point of an external finishing tool, in pocket #1 of the turret. This is what I did when I set up my machine. I took trial cuts, using the display values of the G53 machine coordinate system. I determined by trial measurement, how to adjust the G28 X parameter so that it actually corresponds to the real position of T#1, relative to the part centerline. This may seem kind of a$$ backwards, but once its done, its done. Now I know that for this reference T1, the X tool offset will always be very near zero. Any other tools that I might use, if they cut the correct diameter, then their offsets are automatically "related" to T#1, because T#1 is correctly set in the machine coordinate system.

    The Z offset for T#1 is not as unambiguous. The operator needs to determine what he will always use for a Z reference. Since I use one chuck on my lathe, I use its face for a reference. Again, I touch off the chuck face with T#1, and note the display coordinates in the G53 machine coordinate system. This should read Z0. If it does not, then the G28 Z parameter needs to be adjusted until it does. The goal is to make the Zoffset of T#1 = 0, and to remain this way, perhaps with wear offset or tip radius offset being the only adjustments ever made for the Z offset of T#1.

    Now, I touch all other tools off the chuck face, and they are all related to T#1 automatically.

    With this system, you should be able to machine without using G50 fictitious work offsets. The G50 is akin to the old G92 used on the mill, which has a certain danger associated with it.

    And, when you wish to put a part of any length in your chuck, the G54 offset only needs a Z value, and this value equals the distance between the end face of the stock and the chuck face, if that is where your Z0 reference in G53 is located.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  5. #5
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3154
    Downloads
    0
    Uploads
    0

    Default

    Guys

    I, as well, am familiar with using a VMC (my way ;-)) and have just purchased my first simple CNC lathe (Fagor 8040T control).
    I am in the process of figuring things out and getting some training.
    Hu - fairly impressive and confusing post, the water started to clear about 3/4 of the way through. It sounds as though you do a lot of 1-offs (as I do) and set the machine to be versatile and easily set for the next part.
    Can fixture offset not be quickly set as well be touching or skim cutting the virgin stock and inputting an offset zero? (Such as you would do on DRO?) Similar to what DMayfield is saying only without all the calculations?

    www.integratedmechanical.ca


  6. #6
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Darebee,
    I don't claim that my way is the only way You feel free to explain alternative methods.

    I derived the logic for my method on my own. I got tired of working with coordinate system offsets that had no useful relationship to the machine. You think that was confusing, well, I couldn't ever explain the way I used to do it before that A person can always find some kind of a method that works, but whether it makes sense, is another matter.

    I changed methodology to get away from using the G50 (aka G92 on mill) method of creating a coordinate system.

    All the calculations I described are a "one time" deal. They have everything to do with initial setup of the machine and the reference tool. Once the reference tool position is accurately described by the displays when the tool is at home, the rest of the settings are child's play.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  7. #7
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default

    Hu -
    Thanks for the reply, a very good logical one I might add. I like the idea of setting up the machine from known logical coordinates and the reference tool - I am just not sure how to get there from where I am at with this machine. Did some checking of how the machine is set currently. The G53 X zero appears to be where the spindle center and center of the boring tool pockets are in line. The G53 Z zero is the face of the chuck. The confusing thing is where the machine is setup for G28. This is the same as the G53. If I am understanding you correctly, the G28 is both a reference point and also the tool change position. So based on that I have no idea why the previous owner had this setup where G53 and 28 are the same.

    Looking forward, I guess I need to figure out what parameter(s) the G28 settings are in and change these. The X position would be somewhere a 1/2" or so from the axis home (full back) and the Z position would be back (Z +) an amount I determine to be a safe distance, taking into consideration what my longest part will be from chuck face + my longest tool. Getting the G28 to correspond to the reference tool is a bit confusing still. If I keep adjusting the parameter for G28 to make the Z display read zero when tool 1 is touched to chuck face, and if I cut a piece of stock right to 1.0" dia. then the X display should read .5" - doesn't this change where my G28 reference position actually is?? I guess I really like the concept you have outlined and are helping me get to, I'm just fully understanding it yet. Thanks for the help thus far!



  8. #8
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    2
    Downloads
    0
    Uploads
    0

    Default

    Face The Part With A Preset Turning Tool And Set G54 Z Zero At That Point. In Most Lathes You Will Not Need An X Offset.

    Kc
    Application Engineer For A Mori Seiki Dist.



  9. #9
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    MM4039,
    I think I understand your confusion about the reference point. I also suffered that same confusion. I think it might be best to imagine the G53 X0Z0 as a "derived coordinate" which has a relative offset from the G28 position. When we home the machine, it goes to the G28 position, whose display coordinates are preset in parameters. Once the G28 position is reached, this in effect defines where the G53 X0Z0 must be. That is not saying that the G53X0Z0 is at the G28 position. But it does have a well defined offset from that G28 point.

    Whether the machine was ever set up correctly so that the reference tool position is correctly described in the G53 coordinate system, is what I strove to accomplish. Before I did this, the G28 coordinates on my machine were just "tape measure coordinates", not really anything to be relied upon.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  10. #10
    Registered
    Join Date
    May 2005
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    i am very familiar with the fanuc 10t, how i set up all of my lathes is first home out the machine, go into the relative position screen and zero x and z values (origin key on my 10t) i use the face of the chuck as my reference point so i bring the tool down to the chuck and the z value in the relative, will be a negative number, and you manually enter that number into the z column in the geometry offset page. for x i take a cut or position the tool tip on a known diameter and add that to the x value in the relative position, and input that into the x value on the geometry page. so in z that number in the geometry reflects the distance between the tool tip at home position, and the face of the chuck, and in x, the distance between the tool tip in home position and the centerline of the spindle, now to set the g54 go to the work offset page and on both of mine there are 4 sets of values here, #00 is shift,or g53, the numbers in the x,z,and c-if you have it must be zeros in all. next are #01-g54, #02-g55, and #03-g56, all the x values in all the columns set at zero, there should be no reason to change them, now the number you put in the z value of the g54 column will be the distance between the face of the chuck and the finished face of your work (or where z zero in the program will be). the g55 and g56 i use when i have a part i need to flip and want to program both sides at z zero, example: if the g54 is 3.100", and the g55 is 3.050" i will run the first side of the part with the g54 (insert the g54 in the line directly after the tool change of every tool) and programed from z zero, flip the part, then pick up the g55 offset and you have .05 facing stock for the second side of part, in that instance the g55 would be the finished length of the part. on this control you cant change the value of the g54 by trying that in mdi, what you programmed told the machine to pick up the g54 offset, if it was zero the machine understood it as wherever the tool was touched off at, and g1 and g0 are modal commands, they are in effect until it is changed and you dont need to type them in every line for them to be in use. and when it read x0 z0, it was moving to where the tool was touched off at in both axes. there are a lot of ways to set the tool geometry, ive seen a shop that leaves the g54 at zero and touches every tool they use off in z on every part they setup. if anything is unclear please let me know i will explain it differently, i run 2 machines now with the 10t control



  11. #11
    Registered
    Join Date
    May 2005
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    and i think i was unclear about my x teaching, example: say i take a skim cut and the diameter after was 3.050" and in the relative position for x was the number -15.956", the number i would put in the x column in the geometry page is -19.0060, you moved minus in x to get to the position you skim cut, and you need to add the diameter you turned to that negative number to get to the spindle centerline.



  12. #12
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3154
    Downloads
    0
    Uploads
    0

    Default

    Soooo... in G54 T1 will be at X0 at the theo centerline. So what do you do when you switch to T2?
    I would assume that you continue to use G54 with a calculated tool offset -like- M6, T2, H2 (sorry, VMC lingo) right?

    Setup guy is to be here to set parameters and give me the run through today. I hope everything is good, I have a couple of weeks of work on backlog for it.

    www.integratedmechanical.ca


  13. #13
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3154
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by HuFlungDung
    Darebee,
    I don't claim that my way is the only way You feel free to explain alternative methods.
    Hey man - that wasn't a dig, just showing my ignorance in the matter - JK.
    In a couple of days, weeks, months, ? I hope I can be knowledgeable enough on the subject to actually have a "Way"

    You guys are helping - Thanks

    www.integratedmechanical.ca


  14. #14
    Registered
    Join Date
    May 2005
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    in x all of your tools are touched off on the spindle centerline, and when the x in the g54 is always at zero this is where it always goes for x zero, in the program when you change tools(index) the line may read: G0 T1010;- which tells it to index to tool ten and pickup offset ten, then in the next line pickup a work offset like g54 or g55. the x will be correct as long as it was taught correctly



  15. #15
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Darebee,
    I didn't think you were taking a dig at me. I thought maybe you did have a different method to offer

    I should back up a bit and say that there are two methods of setting tool offsets on every machine, whether it be mill or lathe. The operator needs to decide if he is going to use an absolute reference point, or a relative reference point to set the tools to.

    On a mill, some guys will set the tools off the top of the part. This is a relative reference point. It has drawbacks: If the next type of part is a different height, all the tools must be reset, even if they are the same tools. A-hah, they say, they will just use the G54 to take care of that. Sure. Except, they have to add in a couple more tools for the new program. The old part is gone, now what do they set the new tools off of?

    On the mill, using an absolute reference plane might be a little more work, but it is worth it. Use a "standard" of some sort to set all your tools off of and stick with it. No matter what job, any old tools can be trusted to have the correct offset, as will the new tools that you have to add. There is a little bit more work involved though, because instead of leaving the G54 Z at or near zero most of the time, you actually have to measure the difference between your tool setting reference plane and the top of the part. But once that is done, you are good to go.

    Lathe is similar: using the relative method, some guys will set all the tools off a given workpiece. For this method, it doesn't matter where T1, the reference tool is truly located in the machine coordinate system. The tool offsets will be the distance from the G28 position to the face of the part. Again, all the Z offsets must be reset for every part that has a different Z face position. It is possible to fudge new part Z0 positions with G54 offsets, but pretty soon with additional tools added in, you get yourself lost, because you've got too many relative offsets involved.

    So, if you always set your tools Z offset off of a single known reference plane such as the chuck face, or a standard jaw height, then those offsets become portable and correct in any work coordinate system that you want to use.

    I'll continue a bit later.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  16. #16
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    There are a few parameter options to explore in lathe that determine how you will do your tool offset measurements. These options have to be known, otherwise you may attempt to set offsets by a certain routine, and they will not be correct.

    On some systems, a parameter setting will decide if the tool measurement point is (or is not) a pre-defined point in the machine's coordinate system. If the machine has a tool eye (presetting device), then the location of the sensors is defined by parameters. The sensors are so and so far from the X0Z0 of the machine G53 coordinate system. This is an absolute reference point, but in and of itself, represents an internal offset from the machine G53X0Z0. When this point is correctly set in parameters, it means that when T#1 (reference tool) touches the sensors, the offsets (in the offset table) should be zero in both X and Z.

    It is not strictly necessary that the T#1 offsets actually be zero, but theoretically, they should be. Once again, we see how important it was to have the machine coordinate system set correctly relative to T#1.

    The wonderful tool eye system simply allows you to then touch all the rest of your tools off the sensors, and the offset measurements are calculated and recorded by a few key presses.

    Without a tool eye, most guys would rather use the manual measurement system. Many controls have a method to assist you by auto-calculating the offsets by following a given procedure. On the Mitsubishi, I can take a cut, then immediately press an axis button to store the position, then back out of the cut, and then input the actual measured diameter. The control calculates the offset automatically from an internal comparison of the stored value with the measured diameter.

    Now, to do the offsets entirely manually, the same procedure can be followed, but longhand. The controls typically have several options for the displays, showing the current position in
    1), the machine coordinate system,
    2), in the current work coordinate system (if one is active), or
    3), in the operator screen coordinate system (G52, I believe). The operator display of position is quite ambiguous, as you can zero any axis on the operator screen at any time. You just need to find the keystrokes that do it.

    If T#1 reference tool is already defined correctly, you can jog it to touch any accurate surface that you have chucked, and the display in the G53 machine coordinate system should give you an accurate reading of the current diameter setting of T#1. You can even take a cut with the tool to prove it. But as luck would have it, lets say it is off by a small amount. You simply calculate the difference and enter that into the X offset for T#1.

    Now, we cannot arbitrarily change the coordinates in the G53 machine coordinate system. But, we can switch to the operator position screen and zero it whenever we like. So lets zero the X axis in the operator screen while T#1 is still touching the freshly cut surface. Jog clear of the work, measure the part, and jog (handle mode) the X axis towards X0 centerline. Now, we have measured the diameter of the part, so we know where X0 should be. However, the operator display will show us moving into X- but that is ok. Move to an X- value that equals your measurement of the diameter. Zero the operator display again. Finally, T#1 is accurately located for the purposes of the operator position display, and we must remember to not zero the operator display again until the rest of the tools are set.

    Begin to touch the rest of the tools off the cut surface, using a shimstock to feel the moment of the touch. Each time, note the position on the operator display, and if it does not match the actual measured diameter of the part, then either a positive or negative difference is calculated and entered into the X offset for that tool. Positive or negative is dependant on which way the new tool is offset relative to T#1. There is a 50% chance that you'll get it right if you don't know what you are doing

    Watch out for yet another parameter setting in your control, that reckons the X offset amount to be either diameter or radius values. Diameter is the easiest choice, if available, because you don't have to worry about the "divide by two thing".

    For your manual Z offsets, simply touch all the tools off the chuck. Again, touch T#1 first and zero the Z axis of the operator position display. Now, touch all the rest of the tools off the chuck and enter the value shown in the operator position display into the Z offsets for each tool.

    Now, go back to T#1, recheck that the display is still zero when touching off the chuck face. Chuck the part, and move the tool so that it touches the face of the part. Retract in X and, if necessary, move a few thousandths in Z- to give yourself a facing amount. The Z value shown in the operator position display will be your G54 offset amount, if your machine's G53 Z0 is located at the chuck face.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  17. #17
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3154
    Downloads
    0
    Uploads
    0

    Default

    Nice post Hu
    Thanks for taking the time to be so comprehensive.
    Considering I run the VMC with all tools Z0 on the table (to expidite set up) and program my part above Z0 (as you have mentioned above) it would only stand to reason for me to datum my lathe tools similarly for ease of single part runs.

    www.integratedmechanical.ca


  18. #18
    Registered
    Join Date
    Jun 2005
    Location
    usa
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default

    Thanks for the great posts here, this has really brought me along on understanding how to properly setup my machine/tools. I think I am almost there, but not sure, so I thought I would throw my thoughts out here and let you guys tell me if I'm getting there, or still lost - partially lost...??

    The item I am most confused of is how the machine coordinate system is set vs. the way I would like it to be set. I would like it set so that X0 is where my reference tool #1 is at spindle center, and Z0 is where this same tool is touched on chuck face. The machine is NOT set this way now. It is close to this, but not exact. If I am understanding correctly, I am unable to change this??

    At this point the way I would go about to setup the work/tool offsets is like this -
    Home machine, zero the relative displays for X,Z, with tool #1 (ref. tool) in cutting position touch that tool to the chuck face and enter the value on display for the Z offset for tool #1. For X find postion for when this tool is on spindle center and enter that value for the X offset for tool #1. Next, jog off to a safe spot and index turret to next tool and repeat the same procedure for Z, X offests. Repeat this until all of my tools are completed. When I am ready to cut parts - re-home machine and with tool #1 jog and touch face of chuck, zero the Z axis display. Jog over and touch tool to face of part - enter the value on Z axis display into the G54 Z offset. If I want clean up stock, subtract .020", .030" (whatever is needed) from the display value (the Z axis # will always be positive) and enter that value.

    In this manner there will never be any X axis offsets in the work offsets, reason being the tool offsets are all set to center of spindle. The work offsets will only have Z axis offsets. The only thing I have to absolutely make sure of is to call the work offset after each tool change. This makes sense to me, so I hope I am on the right track. Please post if you see something that is wrong, or may cause me problems down the road. Again, thanks for the sharing of knowledge.



  19. #19
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    I don't have any manuals for your particular controller. However, someone must have programmed the reference position at some time (in parameters), so it should be adjustable, but the trick might be to find out where to tweak the settings. As I mentioned earlier, a good place to look is at the G28 settings. The G28 position is set after the machine homes, and from this position, the origin of the G53 system is inferred as being so and so far away from the G28 position.

    This might be one of those parameters that won't take effect until you shut down and restart the control.

    Now, as I read the rest of your method, I think the one thing you may have done "wrong" (aka different ) is that for T#1, you should set the display to zero when the T1 touches the chuck reference face. This is because you want the Z offset of T1 to be zero, and all others get set from there.

    If you do it the method you described, then you might have quite a large Z offset for the T1, and this will throw you way out of position when measuring the G54 from the reference face of the chuck.

    Just try it out (carefully, with rapids turned down low) and see how it pans out.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  20. #20
    Registered
    Join Date
    Jan 2007
    Location
    United States of America
    Posts
    69
    Downloads
    0
    Uploads
    0

    Default

    .

    Last edited by WCIS; 11-19-2013 at 11:45 AM.


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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

CNC lathe tool and work offsets

CNC lathe tool and work offsets