Purpose of system variables #5081-#5084 ?

[sinha_nsit]

Has anybody any idea?
On 0i Mate TC these are always 0, even after executing a T-code (I tried T0101). The operator's manual describe these variables as "tool offset value" in the table for "system variables for position information." The 0i MB manual describes these as "tool length offset value."
Any interpretation / guess?

Sinha

[stevo1]

Hey Sinha.....I am not exactly sure. The book is very vague on the description of these. Maybe try executing a move after the T() call and then try to see if they hold a value. How are you checking the value of them? Are you writing them to a common variable?

Stevo

[chucker]

I think they are only used during a skip signal

Position Information ( ** READ ONLY **)
Axis 1-8 Position Information Coordinate System Tool Compensation Value Read Operation During Movement
#5001-#5008 Block End Point Workpiece Coordinate System Not Included Enabled
#5021-#5028 Current Position Machine Coordinate System Included Disabled
#5041-#5048 Current Position Workpiece Coordinate System Included Disabled
#5061-#5068 Skip Signal Position *1 Workpiece Coordinate System Included Enabled
*1) If Skip Signal is turned on posiotion at signal point is recorded, otherwise endpoint is recorded
#5081-#5088 Tool Offset Value Disabled
#5101-#5108 Deviated Servo Posiotion Disabled
*1) If Skip Signal is turned on posiotion at signal point is recorded, otherwise endpoint is recorded

[sinha_nsit]

Originally Posted by stevo1 ... 1. Maybe try executing a move after the T() call and then try to see if they hold a value. 2. How are you checking the value of them? Are you writing them to a common variable? Stevo

1. You are possibly right. It might contain offset information used in the previous move command. I will check.

2. Yes. I used #500 series just to make sure that these are not inadvertently reset.

Sinha

[sinha_nsit]

I did some experiment on a machine with 0i Mate TC control.

I found out that #5081 and #5082 contain wear-offset values for X- and Z-axis, respectively, corresponding to the current offset number.
No movement command is needed. It is sufficient to execute a T-code.

Any guess why wear offset has been given so much importance?
Possibly for an errortrap, alarming out when wear offset value is too large?

[sinha_nsit]

Presently I do not have access to a milling machine for experimenting. So, I do not know what these variables mean on a milling machine. The manual says these are "tool length offset value."

Can somebody please execute this program and report the result:
O0001;
G43 H01; (store some value in H01)
#501=#5081;
#502=#5082;
#503=#5083;
#504=#5084;
M30;
What do the permanent common variables contain in the end?
If the values are all zeroes, insert, say, M06 T01 in the beginning, and execute again.
The confusion I have is, there is just one length wear value for the selected tool, but there are several system variables (#5081-#5084). Is only #5083 relevant for a VMC?

Sinha

[Fanuc Mate]

Having previously worked for GE Fanuc for several years, i have never even noticed these variables (#5081-#5088) before. I would normally use the #11001 e.g for tooling. Seen all the others and played with them, but not this one. Weird!!!!

I will play tomorrow. And let you know.

Fanuc Mate
Fanuc Mate - Every Fanuc Machinists best mate.

[sinha_nsit]

There is a difference between this variable and 11000 series variables, though both contain wear offsets.
11000 series stores wear offset values (length offset, on a milling machine, if parameter 6000#3 is set to 1) corresponding to the chosen offset number (so you need to specify which offset number you are talking about).
On the other hand, this variable stores the wear value corresponding to the current offset number (so you need not know which offset number is being used currently).

[Fanuc Mate]

Hi Sinha.

Yes thats right. Its basically the amount of compensation for each axis for that current tool. Not a bad function to breakdown compensation. In the past i have worked this out myself with something like #[11000+#4120].

Did you find the answer to your ASCII sub call program? I just tried it.

[sinha_nsit]

Originally Posted by Fanuc Mate Did you find the answer to your ASCII sub call program? I just tried it.

No. Pl share your experience.

Did you run the program suggested by me?
I guess, only #5083 is relevant on a VMC, and it will contain length wear value of the current tool. Pl confirm.

Sinha

[Fanuc Mate]

Yeah, basically #508+ axis number, dependant on param 1020.

In regards to ascii call. Param 6090 = ascii number (A = 65).
So by having 65 in P6090, when A[NUM] is read in a program, program O9004 is call and the [NUM] is passed to #146

So...

A123. -> O9004 & #146=123

Hope that explains it ok.

Fanuc Mate

[sinha_nsit]

I will try the ASCII call method.

But how did you come to know about #146 storing the value?

Edit: Was #5083 wear length offset or geometry offset?