Change tool number limit--possible?

[Merlin76]

You know that if you have a 16 tool carousel and try to call up any tool number higher than 16 (T17M6) you get an error. Does anyone know if there is a setting someplace that I can change to allow me to use higher numbers for tool call up?

Reason:
We use specific offset numbers for certain tools, and those have become the tool designators (2" facemill is always H265, 1/4 chamfer is always H311, etc) and I have edited the tool selection program (O9001) to write the current tool offset number in the first 16 offset locations to correspond with the tool location in the machine, getting the data from the currently running program. In other words, if the 1/4 chamfer is in tool position #1, then offset number 001 H collumn will read .311. I did this so I can go to the machine and look in those 1-16 offset numbers to see if a specific tool is in that machine.

I have also edited the tool selection program to allow me to use T311M6 and it will search for and get that tool from T1 if it is in the machine. However, I can't do this until I can change the limiting factor of 16 in the settings....if possible.

I have Sharp SV-2412S 16-tool and a Sharp SV-2412 mini mill 24-tool machines.

I can't seem to find anything on this anywhere.

[dcoupar]

IIRC, these are umbrella-type toolchangers. When you call for a tool number, it puts the tool back in it's station and rotates to the next station. The t-number you program is actually the station number. If you had a random tool changer you might be able to do it, but I don't believe you can with an umbrella type.

[Merlin76]

We have both types actually. But the way I have written the tool selection program (O9001), when you use T1-16 (or 24 on the bigger one) it just changes to that tool position, but if you use a tool number higher than 16 (or 24) it determines which tool position that offset number is in and then replaces your T# with the tool position number it's in. Suppose you use T311M6...it figures out that the tool with offset H311 is located in tool position one, and then changes your T311M6 to T1M6 and gets your tool. I just need to overcome the tool number limitation of 1-16 & 24, respectively. If someone knows how to do that, I would greatly appreciate it. Currently if I use a tool number outside of that range it just tells me I've used a number that I can't, which given the fact that these come with different size carousels makes me think you can change that.

Thanks for the reply.

[dcoupar]

So, your macro is doing all the math, correct? I misunderstood.

In any case, I believe the number of tools is set in the PMC - DATA table. If you press SYSTEM - [PMC] - [PMCPRM] - [DATA] you should see one of the data values set to 16 and 24 on the other machine.

I'm not sure what changing this would do to the counting when the carousel went past tool 16 and saw the switch for tool 1 unexpectedly, though.

[Merlin76]

Yeah, the macro does all the math. Based on the program running, as a tool is called up, it reads the H offset value and stores that in a variable, ending up with a variable for each tool with it's corresponding H offset. If you call up a tool that is out of the carousel range, it looks in those variables to see if the number you called is in one of them and if it is, it calls up that tool position. If not, it ends the macro and doesn't do anything, just as if you called up the tool that is currently in the spindle.

I changed the PMC - DATA table on the 16 tool machine and was able to call up a T17 with no error, and it went into the O9001. I have to test it today to make sure it'll work the way I want it to and I'll let you know the results.

On the 24 tool machine, I changed it but didn't get the same positive results. It just gave me the same error (1195 specify t code....).

Thanks again for your help.

[Merlin76]

Well, I can make it work, but with limited ability. I can change the number of tools available, but only up to 127 for some reason. So, as long as my tool numbers/offset values aren't above that, It'll work. Unfortunately the offset values I need to use go much higher than that. So, unless I can come up with a way to change that limitation, I'm considering this a case closed.

Thanks for your help.