Bspt thread mill subprogram question

[DetMach-EDM]

We have some Bspt thread mill subprograms we use on a bi weekly basis and we have to edit the program every time (change the d value because we use different tool locations)
My question is, Has anyone ever used the variable for the tool number(T=12) to set the D (D=12) value in the sub? (this way no matter what tool we use it will automatically use the correct D value???)


Thanks for your time

Steve

[txcncman]

Probably right after your tool call you could use: #7=#20 (D=T). This would mean you could not prestage tools.

An alternative is use another variable right after the tool call: #100=#20. Then make all D calls: D#100.

[christinandavid]

I use variables for all my tool numbers. Saves a lot of hassle when using big tooling in fixed tool magazine

DP

[christinandavid]

Now that I recall, I had the same issue with a helical macro we were provided with by the MTB...ended up using the value stored in exec macro #1035 (spindle tool no) to locate the correct tool rad in the offset table and use that in the formula for the arc size...that was on a Doosan. You could do something similar using system variable #4120 (last T number).

DP

[DetMach-EDM]

Now that I recall, I had the same issue with a helical macro we were provided with by the MTB...ended up using the value stored in exec macro #1035 (spindle tool no) to locate the correct tool rad in the offset table and use that in the formula for the arc size...that was on a Doosan. You could do something similar using system variable #4120 (last T number).

DP

Yeah this is the kinda thing i was thinking of.... doing it this way there would be nothing out of the ordinary i would have to put into the main program.

Thanks I'll try this and let you know

Steve

[DetMach-EDM]

Well I tried the variable #4120 Idea.... it worked except for the #4120 is the prestaged tool number not the tool in spindle.

Do you know the tool in spindle variable # of hand???

Thanks
Steve

[christinandavid]

Hmmm, this is why I use the #1035 - it ALWAYS knows what tool is actually in the spindle. As far as I recall, the #4120 is the last T# defined in the program and #4320 is the next T# in the buffer, so neither will help you if you need to get the next tool ready.

You could edit your M6 macro to store the last called T# in, say, #500 and refer to that in your threadmill sub.

DP

[sinha_nsit]

#1035 may not be described in Fanuc manual, but many users have reported that it contains spindle-tool number.

[DetMach-EDM]

Thanks guys I got it to work.

I ended up using #4311 (H value) that way if we have multiple heights for the same tool we can have multiple dia also.

Thanks again for all the help

Steve