[Ashish B]

Hi,

I want to make the values of X,Y,Z as 0.000 on absolute page through a macro program.

Is it possible to do such thing ?
I probably think that its possible because some parameters may be keeping track of X,Y,Z values. If we assign the parameter value to Zero, then automatically the Values of X, Y, Z will be assigned to zero.

Does anyone knows about the parameter which keeps track of X,Y,Z Values ?

Thanks
Ashish

[Ashish B]

Hi,

Searched some books and finally got the variable which tracks values on Absolute page. They are -
#5041 - X axis
#5042 - Y axis
#5043 - Z axis.

I also made a macro program to assign the values to 0.0.
G90 G54 G80
#5041=0.0
M30

But it doesnt works. The value of X axis (on absolute page) remains unchanged.....:-(


I think that these variable are READ ONLY & user is not allow to change the values.

Thanks

[dcoupar]

What model control is this?

[Ashish B]

Mitsubhishi M64 Control

[ksc]

G90G10L2P1X0.0Y0.0Z0.0;
G11;

this should zero your g54 work offset, I have never tried it with the variable # in the formula but it may work.
might look like this.

G90G10#5041=0.0;
G11;

BE SURE TO INCLUDE G11, shuts data setting off!!!!!!!

[Ashish B]

The following codes work absolutely fine. The workoffset is set to Zero properly.
G90G10L2P1X0.0Y0.0Z0.0;
G11;


But if the following codes are commanded that alarm (ILLEGAL ADDRESS ERROR) is generated.
G90G10#5041=0.0;
G11;


Need help

[dcoupar]

The following codes work absolutely fine. The workoffset is set to Zero properly.
G90G10L2P1X0.0Y0.0Z0.0;
G11;


But if the following codes are commanded that alarm (ILLEGAL ADDRESS ERROR) is generated.
G90G10#5041=0.0;
G11;


Need help

A couple of things:

#5041 is READ ONLY.

G11 is not required for setting work coordinates with G10. It is required for Program Parameter Input with G10 L50 or tool life management data setting G10 L3.

What exactly are you trying to accomplish?

[Andre' B]

If you want to set the work offsets without using G10 the variable numbers for the standard 6 generally are.
I do not remember any machine/control where they are at a different location.
The extended offsets and tool offsets are not as well defined.

     X axis Y axis Z axis 4th    etc.
G54  #5221  #5222  #5223  #5224
G55  #5241  #5242  #5243  #5244
G56  #5261  #5262  #5263  #5264
G57  #5281  #5282  #5283  #5284
G58  #5301  #5302  #5303  #5304
G59  #5321  #5322  #5323  #5324

EXT  #5201  #5202  #5203  #5204

The EXT work offset is basically added to the values in the normal work offsets. So if you put a 1.0 in #5201 you move all the work offsets 1 inch in the X axis.

[Ashish B]

Hi,

Thanks for your prompt responses.

I actually don't need to enter G54 work offsets through a program.

I am actually looking forward to zero out X,Y,Z axis (on Absolute page) of machine screen.

Thanks
Ashish

[dcoupar]

Hi,

Thanks for your prompt responses.

I actually don't need to enter G54 work offsets through a program.

I am actually looking forward to zero out X,Y,Z axis (on Absolute page) of machine screen.

Thanks
Ashish

WHY???

[stevo1]

Your absolute values will read 0(zero) on your absolute page if you program our G54-G59(which ever you are using) and then program X0Y0Z0. Other then that there is nothing you can do with these. As Dave asked....."what are you trying to do" and why???? As I am sure you know your absolute values are nothing more then what you specify as your origin and what position you are from that.

Stevo

[Ashish B]

Hi,
Thanks for your reply.

I am looking forward to keep track of certain values (when m/c is working) & hence wanted to make the Absolute screen as X0Y0Z0.

Thanks

[stevo1]

Hi,
Thanks for your reply.

I am looking forward to keep track of certain values (when m/c is working) & hence wanted to make the Absolute screen as X0Y0Z0.

Thanks

Your absolute position when the MC is running is going the be the distance at which the machine is from your active coordinate. You can not just zero them from the program (not that I am aware of anyway). You can however take the current value of the absolute position at any given time and use the difference between the 2.

There may be a better way if you explain what you are using the numbers for.

Stevo

[Ashish B]

Hi,

Extermely sorry for late reply. I was out of town so couldnt get in touch with CNC Zone Dot com.

We actually have production parts. Many similar parts are been clamped on a baseplate & Subprograms are been executed accordingly.

The problem is that as the Machine starts the subprogram, the Absolute screen shows coordinates with respect to the Subprogram. I want to keep track of machine axis ( with respect to Main program ) so that i can calculate the air cutting time and improvise accordingly.

I hope that i was not too confusing.

Thanks