Oi-TC add comments to macro variable table

[nracingdev]

Hi guys new to the forum. I am a programmer and I sometimes have operators interface with the machine changing values in the macro variable screen (#500+). I have noticed that there are two columns other than the data entry column. I believe the other two are names and comments. Does anyone know how to enter text into those fields? I have not been lucky searching on the net nor reading the operator manual. Thanks Chris!

[stevo1]

Chris....welcome to the group.

Yes you can label them. I did a quick search thru the Oi manual and I could not confirm the function in your control. On my 15 series control it is done with the SETVN function. So in MDI mode or in the program you would do this

SETVN500[TEXT]

This would put the word “TEXT” in variable 500 in the comment section. If you wanted to set #501 then change the 500 to a 501.

Stevo

FYI you can also lock specific variables in the control via parameter if you have some that you don't want someone to accidently change.

[nracingdev]

thanks for the reply. I will give that a try. This enters the "text" into the comments section. how do you enter it into the name section? also what parameter locks the values? that would be a very good function to have. thanks again i have been scratching my head on this for a while!

[dcoupar]

I find SETVN in the 15i, 31i, and 0i-TD manuals, but not the 0i-TC manual. Here's the section from the 0i-TD manual.

[cnc2149]

The SETVN is used in the Series 11/12/15 and 30i series of CNC controls. FANUC allows one to program the NAME field on the Macro page using an optional feature in most controls that is called Pattern Data Input. Actually, with the Series 0i-C this feature is standard so you should be able to use it.

Go to the Pattern Data Input section of the Operators Manual and you'll see an example. Programming it is not as easy as the SETVN, but it should help you out.

[stevo1]

Dave,
I was looking in the Oi-mc manual and could not find it either. I would think that if it does have the "Name" section in the variables that you should be able to write to it but who knows until Chris tries it.

I was also looking for the parameters to protect specific variables. In my 15 series it is #7031 is the start of variables to protect and #7032 is the last variable to protect. So if I wanted to protect #500-#520 I would set #7031=500 and #7032=520. I however could not find this variable in the Oi manual.

Chris,
Yes I meant to say "name" not comment.

Stevo

[dcoupar]

Originally Posted by cnc2149 The SETVN is used in the Series 11/12/15 and 30i series of CNC controls. FANUC allows one to program the NAME field on the Macro page using an optional feature in most controls that is called Pattern Data Input. Actually, with the Series 0i-C this feature is standard so you should be able to use it. Go to the Pattern Data Input section of the Operators Manual and you'll see an example. Programming it is not as easy as the SETVN, but it should help you out.

Damn I love this place. You learn something new every day.

Thanks CNC1249

[nracingdev]

no go. Error 113, improper command is the error I receive when trying to use the SETVN command.

[cnc2149]

That makes sense since the 0i-C does not support the SETVN. You'll need to use the Pattern Data Input feature to set up a macro variable name in this control.

The reason the 0i-D controls support SETVN is because they are a derivative of the 30i series control family. The 0i-C is derived from the 16i series controller and does not allow SETVN commands.

[axis india]

hi guy
can anybody tell how to use mdi dpl i m having one

[stevo1]

cnc2149,
I got your PM. Yes I missed your post. Thank you for the info. As Dave said “learn something new everyday”.

Stevo

[dcoupar]

Originally Posted by axis india hi guy can anybody tell how to use mdi dpl i m having one

Why did you post this here? You should have started a new thread. What's an "mdi dpl"?