[Michael82]

I had a dissucssion with the head of the cnc dept. at work today and he said that if you typed in the tool change command and have the tool # and the m code on the same line that on some fanuc controls it will freak out and just keep changing the same two tools over and over.I told him that I have been doing it the whole time that I have working there. He said it was only on some Fanuc controls not all of them. So I showed him that my machine did not do any thing but change tools when I put in the two codes on the same line just like this T1M6;then press insert,then cycle start. Is there any Fanuc controls that will not except these two codes on the same line?
This is the only machine that I have ran at this company I just started this job.Should I try it on the other machines or not ?

[cam1]

Hi:
Just a suggestion, why not bet a steak dinner on it first.....

regards

[psychomill]

To clear this up..... it's actually there are some machines that will not accept it on the same line... not the control. It depends on the builder's ladder and/or tool change macro. Now, granted, I have not seen this in a very long time and for the most part, I think most builders have addressed that issue (if they were having it) to allow the tool change commmand on the same line. Many years ago, I have run machines that would either tool change forever, or not tool change at all. On another instance, it would tool change even if the tool was already in the spindle and run "empty" or the wrong tool. That was an old practice for some machines and there were other controls that did this as well. But, I have seen it on FANUC machines... but it's not FANUC's deal. I would say, that unless there some particular instance of a machine (or some machines) doing that in the shop you're at, its pretty safe to continue what you're doing UNLESS the shop is going to force you to abide by some format. You'll definately know right away if you're on a machine that doesn't allow it...

[CAD/CAM Man]

It also depends on the style of the tool changer. If the machine has an arm that changes tools from a position (netural pocket) where the next tool is waiting to go into the spindle, you need to break up the tool change line, because "T1" will place the next programed tool in the pocket, then "M6" will cause it to swing to a verticle position, the arm will then swing to grab both tools, drop down and swing 180 deg to swap one tool with the other, and so on. I think it is the diffrence between a side mounted tool changer, and a carousel type. On a diffrent note, I have a FADAL with a FANUC 18-i control, that will only take the tool change comand as "M6T1". Normally the controlls should take it either way, but not on mine. Any one else seen this?

[psychomill]

Any one else seen this?

Yep... on another FADAL....

... and good point on tool changer style which is another possible reason....

[ragman]

It also depends on the style of the tool changer. If the machine has an arm that changes tools from a position (netural pocket) where the next tool is waiting to go into the spindle, you need to break up the tool change line, because "T1" will place the next programed tool in the pocket, then "M6" will cause it to swing to a verticle position, the arm will then swing to grab both tools, drop down and swing 180 deg to swap one tool with the other, and so on. I think it is the diffrence between a side mounted tool changer, and a carousel type. On a diffrent note, I have a FADAL with a FANUC 18-i control, that will only take the tool change comand as "M6T1". Normally the controlls should take it either way, but not on mine. Any one else seen this?

I have a YANG HMC with a Fanuc OM-D control that will only accept M6T1 not T1M6.

[Michael82]

The machine that I am talking about has an arm that changes the tool not the carousel type it has a ( neutral pocket or a pocket that stays empty ) and it puts the tool back at random, but there is a parameter that you can change to where the machine will put it back in the same spot.But the head of the department says it takes too long and he's right it does ,but any way back to the question the machine is that type that you were talking about in the reply and I put the two codes on the same line and I have had no trouble. I think it is a parameter that I can change to make this work on all machines?

[MazakMikeO]

I run a Mazak V550 with that type of tool changer and you need to call up the tool first then use M06. It does toolchange if you don't but not always to the correct tool.

[nanda23]

It is not the question of Fanuc /Siemens CNC control. its all depends on the Machine tool manufacturer. Some manufacturer will use sub program for tool change.there u can't command tool# and M code on the same line.if the complete tool change logic is done by PLC logic then u can command tool and m code on the same line.

nandakumar