Macro B question

[MIL-TFP-41]

I dug around and can't find the answer to this

I want to make a statement saying something like this:

If #3 and #18 are not equal to #0 then go to N400

would the correct format be this?

IF[#3AND#18NE#0]GOTO400

I dug around in a bunch of Renishaw macros & could't find anything like that. There was some that looked like this:

IF[#3AND18NE#0]GOTO400

So the # sign is missing from the 18

 

What would be the correct way?

[Guest]

IF[#3NE#0]AND[#18NE#0]GOTO400

I think that'll get it

Edited March 12, 2018 by Guest

[MIL-TFP-41]

23 hours ago, JParis said:

IF[#3NE#0]AND[#18NE#0]GOTO400

I think that'll get it

OK, I tried that & got an illegal expression alarm.

It did take both this IF[#3AND#18NE#0]GOTO400 and IF[#3AND18NE#0]GOTO400

however.....It didn't react as I hoped so back to the drawing board

[jlw™]

#0 is typically an un-assignable NULL or 0. value used in MTB "stuff."  At least, every Fanuc based control I've had my hands on. I typically try to use all #500 and higher as you get down into the variables the MTB and probe use down in the #0 to #199 area.  I have generally had bad luck with #0 and I always just assign one such as #599=0. for my use.

Then you should be able to use what John offered but subbing #599 for #0.

In my experience any way, hope that helps.

[Guess_who]

Are you wanting to check for 'NIL' or are you checking for a '0'

[MIL-TFP-41]

20 minutes ago, Guess_who said:

Are you wanting to check for 'NIL' or are you checking for a '0'

I am checking to see if "C" and "R" have a value or not. If they both have a value, it will jump to an error message.

[Guess_who]

What do C and R signify?  And are you initializing C and R? 

[MIL-TFP-41]

I got it worked out. Later in the program there is a line, IF[#18EQ#0]THEN#18=0.

The fanuc's read ahead even when you turn high speed off with a G5.1Q0, so it was giving R or #18 a value of zero when it hit that statement ( IF[#3AND#18NE#0]GOTO400 ), even tho the program had not progressed to that point.

So I changed it to read if #3 and #18 had a value other than zero, an error came up. Got it working...so all is well.

[jlw™]

G4X0. will stop look ahead in a Fanuc based control.

[MIL-TFP-41]

2 minutes ago, jlw™ said:

G4X0. will stop look ahead in a Fanuc based control.

I'll give that one a try, Thanks!

[Leon82]

Do you have to restart it afterwards or does it come back on on the next block?

[Leon82]

We had to turn it off in the RenaShaw settings program because it was making the probing Cycles work incorrectly

[Guess_who]

Yes, look ahead in many macros is a no-no. The G04 X0, is an excellent suggestion. I've also seen G53 used for the same thing. Just look at some Renishaw probing code and you'll see what I mean.  

[Matthew Hajicek - Singularity]

When writing macros I prove them out in NCPlot.  They have a free trial for about two weeks IIRC.

[jlw™]

I use the same:

http://www.ncplot.com/macrocalc/macrocalc.htm

[Tim Johnson]

On 3/13/2018 at 5:05 PM, Leon82 said:

We had to turn it off in the RenaShaw settings program because it was making the probing Cycles work incorrectly

I ended up doing that also. Renishaw told me what it was but I forgot. (2002?) They told me to comment it and see if that worked. It did.

[AlbertZini]

 

[Leon82]

11 hours ago, Tim Johnson said:

I ended up doing that also. Renishaw told me what it was but I forgot. (2002?) They told me to comment it and see if that worked. It did.

We have 1604 bit zero on and the install guys put the g5.1q0 in the settings sub program. 

But the ots macro where it spins the tool to touch off isn't working. The guy is coming to look at it but I may try turning the parameter off to see if it makes a difference