[Get lucky]

Al right lets see if I can explain this.

I was wondering if there is a way to make make the machine when threading to come to the end of the thread and stop (not meaning stop the machine) in the z and then retact in the x instead of leading out on the last thread I know this would make a sold line in the part but it is relived at the end so it doesn't mater.

the machine has a fanuc oi-tb

code is as follows

N300M01
G0T0000M8
(THREDING SECO INSERT 16ERAG60-A CP500)
(7/16-14 MAJOR .4361/4258 PITCH .3897/.385 MINOR .3511)
G97S200M3
X.4471Z.3T0000
G76P010060
G76X.3511Z-.995P480Q170F.07142
G28U0W0T0000

Thank you for your input,
Kyle

[ProProcess]

The only way I know would be to nix the canned code and hard code with G32 .... would obviously be more programming intense but you could do what every you want. That would be my approach.
HTH
Good luck

[Get lucky]

I don't really care how I much programing I would have to do i just know that, that caned cycle is not working and all the programing I have done is what I have learned from studying other programs and looking the manuals from the manufacturer of the machine if some body could explain how I would arrive at the #'s to program in G32 that would be great.

thank you
Kyle
:withstupi

[ProProcess]

All G32 does is override the Feed dial to 100% regardless of what you have it set to AND syncronize axial movement with the spindle i.e. threading.

I would suggest that you start by looking in your manul or online for general and specific info about using G32.

What exactly are you trying to do?

[Get lucky]

my problem is that the distance from the end of the threading insert is .075
to the center of the point and the relief in the part is only .08 so the last half thread or so is not cut to depth and the go nogo gage will not thread all the way to the end or to the shoulder of the part because of the retract of the caned cycle.

thank you
Kyle

[ProProcess]

I see.
I don't think G32 will be much help in that case then.
If you explore most control manuals the only guarentee plus one picth at the beginging and end of the thread any way.
If it were me, I would look into a different tool with less shift, maybe a Full Profile insert would get you closer ... this is generally true.
HTH
Good Luck.

[Get lucky]

You maybe right I may have to look at getting a topping insert or something

[chucker]

On most machines I have ran there is a prammeter that you can change to pull straight out of the thread or thper out of the thread I think it was called chamfering off and on I have used it when threading up to a sholder on amce threads

[Get lucky]

Yes maybe I was reading some were else about M24 witch stated champfer off
M23 champfer on not to sure waiting on matl. now so i can try something different then G76

[pdoherty]

According to Smid, most Fanuc controls support M23/M24. See attached.

Smid's book "CNC Programming Handbook" belongs on your bookshelf (or nightstand) if you are at all serious about programming CNC machines.

[ame="http://www.amazon.com/Programming-Handbook-Third-Peter-Smid/dp/0831133473"]Amazon.com: CNC Programming Handbook, Third Edition: Peter Smid: Books[/ame]

[ProProcess]

G76P010060
G76X.3511Z-.995P480Q170F.07142
G28U0W0T0000

The the "00" in the middle of the first G76 should be straight pull out

[Get lucky]

The the "00" in the middle of the first G76 should be straight pull out

That is the way I thought it would work but it dose not it has a half thread lead out
I am going to try that M23/M24 though just to see.

pdoherty, thank you for that page from the book I will really have to consider buying those books just for the knowledge.

[cnc-king]

Al right lets see if I can explain this.

I was wondering if there is a way to make make the machine when threading to come to the end of the thread and stop (not meaning stop the machine) in the z and then retact in the x instead of leading out on the last thread I know this would make a sold line in the part but it is relived at the end so it doesn't mater.

the machine has a fanuc oi-tb

code is as follows

N300M01
G0T0000M8
(THREDING SECO INSERT 16ERAG60-A CP500)
(7/16-14 MAJOR .4361/4258 PITCH .3897/.385 MINOR .3511)
G97S200M3
X.4471Z.3T0000
G76P010060
G76X.3511Z-.995P480Q170F.07142
G28U0W0T0000

Thank you for your input,
Kyle

make parameter 5130 to zero and that will allow the G76 and G92 thread cycles to pull straight out in the X axis at the end of the feed you can set that parameter in 0.10 increments for the chamfering

[sinha_nsit]

That is the way I thought it would work but it dose not it has a half thread lead out

Even the manual says that 00 is for zero chamfer distance, and everybody believes that. If really even 00 gives a chamfer distance of half a thread, then it is a new information for us. Please verify it again and let us know.

You can try G92 also. The chamfer distance is controlled by a parameter. But, in that case also, a zero value may not actually give a zero chamfer distance, if the control is designed with the logic of miminum allowable chamfer distance

[Daleb]

M24 will pull out closer to a shoulder than M23. Years back when I went to training on CNC's the instructor told me when you want to get close to the shoulder slow the RPM down. I've always done that and it has worked. I can't recall getting within .005, but you can try it and see.

[Stebedeff]

That's a parameter isue. I had the same problem on a Fanuc 21it. Changed the parameter and it worked. Don't know which parameter it is for you.

[Get lucky]

I never tried the parameter but M23/M24 did not work and I didn't try G32 the customer was bagging for these parts because the matl. was so late so I had them just open the thread relief. they said that it really didn't have to be that close any ways


Thanks for all your help.
Kyle

[straggleweed]

you should slow down ur spindle speed like Daleb suggested.. the faster you the tool is moving the more time it takes for it to slow down so that it can pull out with out creating a chamfer. the slower it goes the less ammount of time it takes to pull out straight so you have distance of useable threads

[sinha_nsit]

Logically, slowing down RPM may not work. In such a case, use G32. At the thread end, retract the tool by G00 or G01. It will pull out straight.

[straggleweed]

Logically, the cutting move in a G76 is identical to a G32 so the result will be the same. the cutter has to be able to slow down before it pulls out no matter witch code is used. there is a formula for calculating the speed up and slow down distance for threading based on RPM. the faster the rpm the longer the slow down distance will be producing more unusable threads. The slower the rpm the shorter the pull out distance and this will produce MORE usable threads. As long as the the two middle numbers in the P010060 command are 00 then there will be no chamfer. If his control uses the old style one line programming then he will have to use the correct M code to turn chamfering off.

Chamfering is not the issue here, the issue is the slow down distance so he needs to slow down the spindle to decrease the ammount of unusable treads. i had the same issue last month slowing down fixed the problem.