Changing G30 position

[within a thou]

Good morning,

 

I have a bridge style VMC with a fanuc 16m controller. G28 Y0.0 is machine home position. G30 Y0.0 is tool change position. The tool changer doesn't work and the operator has to manually change tools. Since it is a bridge style the head moves on Y and not the table. Both machine and tool change position (G28 and G30) send the head to the back of the machine. If I know where the machine position I want to send the Y axis to in this case Y-82.5 what should the line of code whihc appears after the G91 g28 Z0.0 look like to command this after the end of the cycle or is there a way to change the G30 position (which we don't ned any mopre since the ATC doesn't work) in the controller so G28 G91 Y0.0 sends the spindle to machine position Y-82.5. Thanks in advance for any and all help.

 

Mat

[Allan]

On the position screen when in jog or handwheel there should be a SET FRP soft key, this memorizes the current position as the G30 position.

If you do not have that then it will be in the parameters most likely as a metric value from the home position (sorry I do not know what parameter number it is)

 

Allan

[Dave Ball]

Parameter 1241 is for the 2nd reference position, 1242 is for the 3rd. reference position. You could set the 3rd. position and use G30 P3 in your code, leaving the 2nd position in case you ever fix the tool changer. NOTE: you must power down after setting these parameters for them to become active.

[within a thou]

Dave,

 

I tried what you said and changed parameter 1242 tyo the metric value I wanted.

 

When I type in G91 G30 P3 Y0. it still goes to G30 Y reference point.(back of the machine)

 

When I type G30 P3 Y0. it comes to where I want it then heads back to the back of the machine.

 

When I type in G30 Y0. it does the same whether or not the P3 is in there or not (comes front to back).

 

Is there something I am missing? How should my block of code look?

 

Thanks again for all the help.

[specv]

can't you just have a line that says G91 G30 Y-82.5? I realize this is a workaround but then it can be adjusted when ever you want.

[within a thou]

When I try that it does a incremental move from wherever my tool is. The work around I am using right now is G90 G54.1 P100 Y0. Then in my offsets I have my Y value set for the P100 offset at Y-82.5. We never use those offsets with the work we do here so this will work in the meantime. Thanks for the help

[Charlie Pierson]

As I recall, the G28, G30 etc commands are a 2 step function.

 

Go to reference point, but first go thru the point specified by the XYZ sections of the block.

 

normally you can see this happen if you execute the G28 command in single block mode.

 

ex: G91G28X0Y0Z0 says to go 'home' but first go nowhere (G91X0Y0Z0)

G90G28X0Y0Z0 says to 'go home' but first go to X0Y0Z0 cuz' of the G90.

 

Methinks the parameter values are trailing zero metric so an english value of -.001 will be represented by a parameter value of -25, -.1 represented as -2500 etc.

 

hope this helps.

 

cp

[specv]

Do you have a G53 code? On our Makinos we send the pallet/table to G53 Z0. but we can change that to whatever we want. It's a machine zero but in absolute.

[Roger Peterson]

There's nothing wrong with using the G30pxx to do this as it can be changed at the machine which can be useful. but like Pete said G53 is machine coordinates, it doesn't mess with any work offsets or preset positions so you could do a G0G90G53X-82.5