Help with thread G Code

[Buckshott00]

Hello,

I'm using NX CAM 7.5.1.5 and no matter what I try I can't get the thread cycle to run correctly.

I know I need to output a G99 code to cut thread on the lathe, but no matter what I've tried it keeps posting a G98.

I've tried changing the insert type, the cutting type, the thread type, the feedrates, just about everything I could think of on the UG pallet side of things.

On the post-processor side I've changed blocks of code, the best I could get it to do was to Output a G99 but in the wrong spot and the G98 was still present further in the post so it cancelled it out.

Any advice would be much appreciated. Thanks.

Has anyone else had this problem?

 

[Jaydenn]

If I'm not mistaken, G99 on a lathe is feed per rev, correct?

Did you try setting your feeds as inches per rev?
I know it seems obvious, but, sometimes overlooked.
See attached picture.

J

NX 6.0.5.3

 

[Buckshott00]

Thanks for the Response J,

Yes, G99 is IPR feed.

I did try that,:-( I even tried changing the method from lathe thread to every other type of method including none and setting the cutting to ipr.

I even went through and changed all the available cut modes to ipr.

Thanks for the help every suggestion brings me closer to the answer

 

[shags72]

Where are you trying to put that code out? It is only available in motion events if I remember correctly. If you try to output it in tool change or the like it is always pm feed. I think I might have a pr in on that but I complained about it awhile ago.

 

[Buckshott00]

Thanks Shags,

I haven't tried there. I will check it out and see what I can come up with.

 

[Buckshott00]

Thanks again Shags, when I input there as opposed to before tool change or in a custom command, I still get the G98.

However, it cancels it out when it gets to the actual thread cutting and inputs G99.

I will keep playing with it.

Thanks again!!

 

[shags72]

No problem. I don't know why it reverts to pm at the start of operation. I asked for it to be available at start of op and that there only be one setting per op so that inadvertantly you don't have rapids set to mmpm and feed set to mmpr which like in fanucs controls the dwell output.

 

[Buckshott00]

That would make sense, You wouldn't want to be cutting and then it switches to a rapid move and messes up your thread. It seems very odd that it is setup this way.

 

[shags72]

Yes yes it does.

 

[shags72]

ROFL

 

[Buckshott00]

LOL

I'm still working on it. I'm trying to get it to actually cut with a proper G76 cycle.

 

[Buckshott00]

The post builder help is saying that it can't do what I'm trying to do. I'm attaching a picture.

I think I'll start another thread to see how others have dealt with this.

Thanks again to all that helped

 

[Buckshott00]

The pic

 

[shags72]

What exactly do you need in the line? I can't remember as it has been awhile since I programmed a thread cycle.

 

[Buckshott00]

I'm trying to run the cycle like this: (I took this example from the practical machinist because it's exactly how our CNC programmer has his thread cycles setup)


8 threads per inch, probable height of thread .060". With a full-form insert .

G99
G0 X2.56 Z.15
G76 P020060 Q20 R5
G76 X2.380 Z-x.xxx P600 Q120 F.125

First line of G76 the P is: 1st pair is number of free passes (a.k.a. spring passes) at final depth
2nd pair is number of "leads" to exit at the Z axis end of stroke ex. 32 means 3.2 turns of pullout, starts pulling X axis out at (.125 x 3.2=.4) from end Z position, offering a stronger thread. Good for high strength studs
3rd pair is the included angle of the thread, needed to work the insert in in the "compound angle"

the Q is: "clamp value", meaning the smallest increment the infeed goes to in the penultimate pass. Working in conjunction with the second line's Q value, this Q value helps determine the total number of strokes it will takes to complete the cycle. Bigger 1st Q, fewer strokes, smaller means more finite stepping down to size. Normally, I never have that R be larger than the Q.

The R is: final pass depth before the "free passes" of the first two digits of the 1st G76's P code.

The SECOND G76:

X is the final "root" or "minor" diameter of the thread
Z is your length from the Z zero point
P is the incremental ("on a side") height of the thread
Q is the incremental depth of the first pass
R is (optional) incremental taper of the thread. Use this when making a tapered (pipe) thread or for correcting slight tapers in a long, unsupported thread.
F is the feed rate for the pitch (lead) of the thread. Your 8 pitch example: 1 divided by 8 = .125


Thanks

 

[shags72]

I think I would try turning on the review tool and then posting a single threading op to see what variables are available when and if you can just redo the Lathe Thread proc to your liking. Now this is just theory.

 

[Buckshott00]

Thanks again shags, I have come to believe that NX is not capable of running a canned cycle for threading the way our machine would read it.

I think I am either going to have to adjust the thread motion to use codes the machine will understand but that our CNC programmer doesn't typically use, or figure out some sort of MACRO for when it encounters a thread operation.

Thanks again I really appreciate all of your help.

 

[joycejo]

As you read in the Post Builder it does not support a thread cycle out-of-the-box. The Thread operation in NX outputs all of the motion to cut a thread, making a very long program. Why it does not out put a thread cycle is another issue. You can however create a UDE to have the user input the values you described. Then output the thread cycle as you desire.

John Joyce
N.C. Programming Supervisor
Barnes Aerospace, Windsor CT
NX6.0.5.3

 

[Buckshott00]

Thanks John,

Would you have an example handy of that User Defined Event? Also, would it be possible to write a macro that can capture that data from the CAM paths/pallet and output the cycle correctly?

Thanks,
--Buckshott00

 

[joycejo]

I do not have an example of that UDE if your interested in learning a little about them I have attached a presentation I did in 2005 on them. Once you learn more you should be able to extract the variables with the post to create the right output.

John Joyce
N.C. Programming Supervisor
Barnes Aerospace, Windsor CT
NX6.0.5.3