[jimsy]

G"day all. I have a goodway cnc lathe with a fanuc o-t controller and i am experiencing problems with my tool lenght off sets in z when setting with the tool setter. First I go and touch the tools with the face of the setter ( boring and turning ) then get the turning tool and touch on the face of the job, turn on the work shift and press the soft key. I then run my program and the z axis is way off where it should be. The x axis is fine. Any help would be appreciated.
Cheers
jimsy

[hawkburger]

set the part in chuck, face off with facing tool (#1), set Tool length offset (#1 = 0.0)
See Machine position, z- 25.00 for example, input this same number on "work offset" position or g54 z - 25.00 . Always start machine, manually zero return all axis, cancel numbers or verify machine position is at x=0 z=0 . When using tool setter, ther is a parameter to "Comp out" for fine tuning to Zero your face tool.
Cut face set position to 0, then touch probe, add the difference to your work offset.

[dcoupar]

Does your machine have G54-G59 work coordinates? Usually after setting all the tools, I activate the turning tool and offset (T0101, for example in MDI), then touch the face of the part. In the Work offset G54, press Z, 0, and [MEASUR]. Your Z ABS position should read 0.

[jimsy]

I have only been running this lathe for 6 months so pretty new to this. Basically i have been getting away with the z off set by touching each tool on the face of the job and inputting this number into my program. eg
g10 po x0. z -565.
g50 s1000
t0909 g96 s300
go x100. z 2.
but most of the work we are doing are 10 off jobbing type work and wonder if there is an easy way to touch on the face on any particular job with the turning tool once only and all the other tools will be set by the tool setter. So basically touch once then start running the program.
My machine does not accept g54 for some reason.
The funny thing is that the x axis works fine after touching with the tool setter and just adjusting the wear to machine the correct diameter. When I touch on the tool setter I am getting values like 7.983 turning and 97.032 for boring. What values do I add. An example would be great.
cheers
jimsy.

[g-codeguy]

I have only been running this lathe for 6 months so pretty new to this. Basically i have been getting away with the z off set by touching each tool on the face of the job and inputting this number into my program. eg
g10 po x0. z -565.
g50 s1000
t0909 g96 s300
go x100. z 2.
but most of the work we are doing are 10 off jobbing type work and wonder if there is an easy way to touch on the face on any particular job with the turning tool once only and all the other tools will be set by the tool setter. So basically touch once then start running the program.
My machine does not accept g54 for some reason.
The funny thing is that the x axis works fine after touching with the tool setter and just adjusting the wear to machine the correct diameter. When I touch on the tool setter I am getting values like 7.983 turning and 97.032 for boring. What values do I add. An example would be great.
cheers
jimsy.

You are doing things the hard way. Change a tool, change the program. First of all you don't add anything to the geometry. That is why you have a probe. It sets the tool geometry for you. If X is off then you need to make the necessary adjustment to its corresponding parameter. No need to ever change the Z parameters. If the X is off a bit, use the OFFSET page to make minor adjustments. If all tools are off about the same amount (in the same direction), change the corresponding parameter.

None of our lathes with OT controls use the G54-G59 work offsets. Not familiar with your machine so I can't tell you how to set the workshift. I can give you an example for a couple of our lathes. Using the number from your example:

For our Hardinge, Mori and Daewoo lathes with OT controls you go to the workshift page after touching the tool to the part, type in MZ7.983 INPUT...or MZ0 INPUT and then W7.983 INPUT. Most use the former. At least one of our setup guys uses the latter.

Now I have run a lathe that allowed me to MDI T0202, touch it off, and set zero without using its geometry. Can't remember the machine or the control. Maybe it is a parameter change, but most of our lathes require you to use the tool's geometry when setting Z zero. Some machines have another button that needs pressing before doing the MZ...etc. Otherwise the workshift will be way off.

Touch off tools. Set workshift. Run job. Set next job up. Touch off any new tools. Set workshift. Run job. Burn up a drill, probe new one, hit cycle start. Its that simple. Having to program a tool's geometry in the program is asking for trouble, IMO.

BTW, I prefer using G10 to G54-G59. We have lathes with both methods.

[slick500]

I assume that the tool data set by the probe is correct, if not you need to adjust the parameter