fanuc 15M #4120

[medaq]

I wanted to modify my tool change program #9006 to be more similiar to my fanuc 16i control.

 

In the 16i control it maintains the next staged tool in #4120. A simple #100=#4120 stores this value just fine.

 

My problem is, on the 15m control. It is always 0.0 when I try to call in the number. #100=#4120. If on the line after a tool change, I can grab the tool number going into the machine. So at some point the #4120 is being updated.

 

This is a hx300 kitamura machine. anyone out there have any experience with this machine/control that can help me find the staged tool value?

[Ron Branch @ Verisurf]

Might have to be after the G43 is called. Try to #4160 = #100 as a different method to assign the macro variable. Backwards stating the Macros should not matter, but can't hurt to try.

[medaq]

I get a variable out of range alarm when I try 4160.

[Ron Branch @ Verisurf]

Typo on my part 4120 was the one you were using that the one I used sorry about that, but you are probably right about out of range the control will probably limit you to user parameters to call ni a program and not allow anything that high since they are considered machine parameters.

 

Thinking about it it would not be smart to call it that way. the way you were originally doing it is the correct way. The idea I had would not work and again thinking about it would strongly recommend against it.

[Dave Ball]

Are you sure #4120 isn't the tool currently in the spindle? Can you post the tool change macro from the hx300 kitamura machine, this would help us see whats currently going on.

[medaq]

The tool change ( O9006 ) is pretty simple.

 

what we had on the 16i control was this line.

 

IF[#4120EQ#517]GOTO40

 

What it did was, if the tool in the spindle is the same as the tcode m6 being called up. We would goto40, to skip all the g30x0y0.

 

So right now, we are getting unecessary movement when dancing a tool around the pallet. So trying to find a way, for the tool change macro, check if the tool is the same as the tool change line. and if it is to skip going to tool change home position.

[Dave Ball]

#4120 holds the T code value, not necessarily just the tool in the spindle, so if your using tool staging you may have to run your check before the T code for your next tool is called.

[medaq]

For some reason though, all I get from #4120 is 0.0 But if I do a #100=#4120 right after a tool change, it does grab a value.

[Guest CNC Apps Guy 1]

Yeah, I've found that you need to grab the variable immediately following the tool change while in the macro. After you've staged youor next tool it's too late.

[medaq]

So if I am getting a 0.0 for #4120 after a tool stage? Is there any solution I can not think of, for checking if the tool in the spindle is the correct tool to continue, and bypass g30x0y0?

[Guest CNC Apps Guy 1]

In your Tool Change MACRO, immediately following the M6, capture it there and then do what checks you need to.

[medaq]

Its working now, thanks for the help.

 

I do have another question just maybe someone can help. I am assuming it is a parameter, but I have scoured the book looking for any kind of data set parameter.

 

For me to edit a common variable. I have to stop the machine go to mdi mode to make the numeric change.

 

Really need to find a way to edit variables with out stopping the machine

[Kyle Waters]

All of the Fanuc machines I have ran have had a key sequence of some sort to access the variables. Once on the page you could adjust from there

[medaq]

The problem atm, I can access the macro variable page no problem. I just can not edit the number unless I am in mdi mode. Which means the machine has to stop. I assume, sicne I have never seen a fanuc do this, it must be a parameter.

[Guest CNC Apps Guy 1]

We don;t have to do that on the 16's, 18's, 21's, O's, 30's, 31's and 32's I've used.

 

I change them on the fly all the time.

[medaq]

I know, I have never seen this before, this is a used machine. And to be honest, who ever was running did not seem like they knew what they were doing.

 

But we have a om, oi, 16i here and none need to be in mdi, just this 15m. Very weird