Machine YCM machining centre
Control Fanuc 200i (same as 0i MC)

Problem: Customer wants to set the table as z zero.

To set his tooling and the z zero of the component he wants to do the following.
Toollength - set in H offset as positive value.
Z zero of job - Measure from table with height gauge and insert this positive value in work coordinate offset in G54.

This method works on 0 mc control , setting size from spindle to table in parameter no 710.

Also om 18i M set value in parameter no 1250.

On the 0i control parameter no 1250 has no effect.

Any advise please.

Regards
Deon

Let the reference point of the spindle (say, lowermost part) touch the location (table top) which is to be made Z0 in G54. In this position, execute (can use MDI mode also)
#5223 = #5023 - #5203;
This would edit G54 offset distance to make the current position Z0.
Add job height incrementally to #5223 in the beginning of the program, and restore the original value in the end (otherwise Z0 would permanently shift).
Now use appropriate tool length offset.
Is this what you want?

I think he wants to actually shift the Z0 position like in the other controls. This is the way I set up all of my machining centers. There is 2 ways to do so. There is a parameter for the Oi control. I do not have the manual with me at the moment but can look it up or Sinha I know you have the manual. It will be the 1st reference position parameters.

The other way to do this is to put the negative distance from Z0 reference to the table face in the “common” workoffset N00. This will shift all work coordinates that are used and will create a positive value using gauge line for tool offsets. So IOW if the distance from Z0+ to the table face is 25” then the “common” Z should be -35.0.

I prefer the parameter so no one can accidently change this value and screw up all the distances.

Stevo

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

I am not getting any e-mail alerts for new posts. Does this site not alert the subscribers (if so, it can never be a forum with heavy traffic) or do I have to change some personal settings?

On 0i, parameter 1240 contains coordinate values of the first reference position in the machine coordinate system.
!241, 1242, 1243 are for second, third and fourth ref positions, respectively.
Cycle power after changing these parameters.

Sinha....did you check the settings that I specified in the "cutter comp" thread?
cutter comp error

Stevo

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

Thank you Guys for your help , I set par 1240 and it solved my problem.

Regards
Deon

Your welcome. I am glad you got it working.

Stevo

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)