Boring bar backoff value problem

[kappullen]

I am training on a Mazak Nexus-250-II Quick Turn.

I have a threaded (ID) part and need to adjust the threading, and boring tool,
back off so the bars don't crash into the back side of the bore.

I believe the backoff in the software is around .078" which limits the bar size
for a .500-20 thread severely.

Is this a parameter that can be changed easily?

Thanks,

Kap Pullen

[extanker59]

On our mazak nexus qt-100 it's in TPC (and parameter) U7
Double check in your Parameters book to make sure yours is the same.

[fizzissist]

Funny ya mention that....I just had to reset mine today for a job...a 9/16-18 hole.

'99 SQT250M

U7 is the back-off value....I'm in inches, and the value is in integer units/ .0001

Mine is set at 800 , which translates to .080"

You should REALLY have the manual with all the values. Screwin' around with parameters can get real expensive real quick. Whoever you're training under should know what you're doing, in case you change something they don't know you've changed and .... things get real expensive on a later job.

You should also have access to the parameter, operation, and programming manuals. I think they're horribly written, but you should still have 'em.

..Btw, you can also do MNP and do plain ole G-code for the boring bar if things are just too dicey. My boring bar was way too big, but only option, so I programmed it in G-code, and lowered the threading tools U7 parameter for clearance on it.

[extanker59]

I mentioned parameters in parenthesis but I first said TPC. If you do it in TPC it changes it only for that op. And if you don't like it just cancel TPC with -9999 and you're back to square one. No harm.
What I like to do is make changes in TPC and then run graphics. Watch the tool path. It really does what you changed. If I'm not sure, sometimes I will change it a lot to make sure that it is moving and moving in the direction I expect.
I agree with fizzissist that you should have the book. And that if you change it in Parameters that it could get expensive on a later job. Do it in TPC. Watch your tool path either way you do it! Very powerful tool.

[jimiscnc]

Guys - double check this.

U7 is for Fusion
TC38 is for Matrix.

Same exact concept, just differing parameter address.

-jim

[extanker59]

Originally Posted by jimiscnc Guys - double check this. U7 is for Fusion TC38 is for Matrix. Same exact concept, just differing parameter address. -jim

Thanks for clarifying. Yeah, you're right. We have a fusion control and it's U7.

[cnc-Mick]

Definitely TPC for this. Go to program edit, select your bar in or thread in sequence, hit the TPC soft key (menu), and it will list all your clearance dimensions. On the QT20HP I run, clearance in, out, face and back are all set to .080". I would start by changing clearance in to .020 (I've had to use even less before), just make sure your sequence show a highlighted "+" sign, that lets you know TPC is active in that sequence. Good luck, and proceed with caution!