(scared)....Post question

[Grant]

Hi Guys,

It's with a little trepidation I ask a post question. I am using a slightly modifyied MPFANBAX post for our horizontal Mori's and Toyoda, and to avoid waiting for tools I am pre-staging the tool call. So the post generates the tool call (for the next tool), after the tool change and then again before the tool change. (The tool gets called twice) The Fanuc controls cannot handle this, and throws me an alarm . Is there an easy way to remove the last tool call??,

Thanks for a great forum

Grant

[CAM-mando]

If I understandyou want to keep tool staging (ie. call the next tool after a tool change, but at the actual toolchange you just want M6 with out T2.

 

I dont know what your post looks like but ... If thats what you want you probably have something like this in the post:

 

ptlchg

 

if stagetool <> two, pbld, n, *t, "M6"

 

change to:

 

if stagetool <> two, pbld, n, "M6"

 

(ie. remove the *t,)

 

If its more complex than that I think the standard answer around these parts is call your VAR

[chris m]

What Fanuc control are you using? It is possible to use a macro to avoid this alarm in some controls (we do it in our 18M). The macro is transparent to the operator (and programmer) except for the fact that the "T2" and "M6" need to be on separate lines. This way you can call the tool at the toolchange; if you eliminate the call at the toolchange you can get REALLY screwed up when picking up a program in the middle. If you like I can email you the information, assuming I can still find it.

 

C

 

[ 03-24-2003, 07:36 AM: Message edited by: chris m ]

[CAM-mando]

To piggy back on what Chris said ... if you cant live with the 2nd tool call just be sure to imbed the tool number in the tool comments to make the prodram easier to read.

[Guest CNC Apps Guy 1]

The root problem with the machine. The Mori Seiki has a parameter, usually K7 bit 3 but may be slightly different. Open up your Electrical Circuit Diagram Book (usually manilla-ish in color) and look in the "K" Parameters. I'd suggest you take a good look in the D and K paramaters. You can turn on some terriffic functionality like multiple M Codes on the same line, 8 digit program numbers, 8 digiyt tool numbers, etc... Check it out.

 

For your Toyoda, there shoudl be a similar parameter that controls this.

 

I know this is not exactly what you were looking for but I just want to see you get the most out of your machine tools.

 

HTH

[Guest CNC Apps Guy 1]

Oh one more thing. You rteally only need to fear asking post questions like the one listed in the FAQ at the top of the posts.

[Grant]

Thanks for the replys Guys,

CAMmando, you advice worked a treat, that line was in the post twice, so I removed the *t on both and bingo!! Chris I would be interested in having a play with the macro program, I'll be in touch,

Thanks,

Grant

[chris m]

Grant

 

I found the info on the macro calls we are using in our machining center with the 18M control. It is fairly straightforward; both the T word and the M word call O9XXX macros so the program still reads

 

T2;

M6;

 

but the machine doesn't freak out when it sees the duplicate tool statement.

 

Pretty easy to try; if you're interested, why don't you email me directly and I'll send you the info?

 

C

[Mick]

Jeez Grant,

 

I could have sorted this for you while I was in there on Tuesday.

Remind me to smack you with a Mastercam mousepad when I see you next. Actually, I might use a Sanvik Coromant catalogue.

 

Mick

[chris m]

Grant

 

I emailed you that macro info tonight, let me know if you don't receive it

 

C