Thread deburring

[tex]

I have a lot of trouble deburring (blunting) threads at the beginning and at the end of them. The G-codes that I do are generally for 1/6" pitch rounded threads on a HAAS SL-30 lathe (supposed to have Fanuc6T controller or similar).

Any ideas about how to make a G-code for "cleaning" the start and finish portion of the thread?

[WOLOG]

Do you mean a thread clip where you are cutting part of the thread off to allow for easy makeup?

If you do, use a grooving insert. program another threading cycle using the grooving tool and the same thread info. The part you have to play around with is the amount of thread you want to remove. Set your "Z" length accordingly. Now move your "Z" starting position until you "clip just the starting thread and not the second thread. Make sure that you use a M24 before the G76 line.

If you don't understand what I am saying, I can Email you a sample program so that you can see what you need to do.

As far as the rear of the thread, I never had to worry about that.

Good luck

By the way, I have a Haas SL-30 Big Bore.

[Rekd]

Are you deburring before you thread? That's how I do it.

'Rekd

[tex]

I'm working on SL-30 Big Bore......it's not mine, though...

The beginning of a thread is "sharp" and needs to be "flattened", so it would look better and nobody could cut himself while twisting it in his hands...here's a sample of a sequence I use for making an OD thread:

G99 M24
X72.2 Z0
M19 P180
G97 S400 M03
G76 D0.8 X65. Z-19. K2.5 F4.23

This cycle is making an almost perfect 70mm thread with 4.23 pitch (1/6"). I do the spring pass afterwards.

In this case I am using M24, but when I do IDs I use M23.

I have tried different "P" and "X" settings, but to no avail. Never thought about changing "Z", though......I wonder whether a grooving insert would follow the same thread lead if I change "Z".

I have tried to do the deburring operation in a tapered way (with an “I” command), but without any success.

If it would be not much trouble to you, please contact me on:

tex707@net.yu

and send an operation code that could do the job. I'm almost desperate about this...

[tex]

Originally posted by Rekd Are you deburring before you thread? That's how I do it. 'Rekd

I am not quite sure what you mean...if I do the deburring before I do the thread, the threading insert would leave the sharp edges at the beginning and at the end of a thread. I do a spring pass after a deburring pass and the abovementioned sharp edges are still there...

[Rekd]

I chamfer meh holes before I thread them. Usually .015 or so bigger than the major dia. Pretty much anything left after that, like razor edges or small burrs can be taken off with scotch-brite or what ever.

'Rekd

[cncrunner]

Give this a try:
1. Run your finish chamfer/turning tool.
2. Run the threading cycle, no spring passes required.
3. Call the finish chamfer/turning tool back up and run it again. This will remove the burrs from the o.d.
4. Last, run the threading cycle again. You can increase the depth of cut so that it those not take as many passes. This will remove the burrs that were kicked in from the turning tool.

This process may seem long, but it those not add much cycle time when done correctly. You will get a burr free thread every time.

Bill.

[tex]

Chamfering/threading/rechamfering/spring pass does not work...that's the first thing I've tried. The customers want a product with "flattened" thread beginning and end....

[tex]

I suppose that you guys understand my problem, but I've attached these screenshots to make everythnig easier. You can see the way "my" thread looks like at the top shot and the portion that should be "flattened" with a grooving tool at the bottom one.

[WOLOG]

TEX,

Did you get the email I sent you earlier today?
It had an attached file for a clipped 3 pitch acme male thread. That is what you are looking for. If you didn't get the file, I will send it to you again.

[tex]

Originally posted by WOLOG TEX, Did you get the email I sent you earlier today? It had an attached file for a clipped 3 pitch acme male thread. That is what you are looking for. If you didn't get the file, I will send it to you again.

No, I haven't received any mail from you yet. You could try to resend it using these two addresses:

tex707@net.yu
tex707@shortonfinal.net

Is the file any different from the file you've attached in this post?

One question about the program...what does "A14" command stand for, and how come you do not use "M19" command to position a spindle at the right angle before you apply a second tool..?...seems like these are two questions...

WOLOG, thank you very much for your effort to help me...and all you guys, you're great!

[WOLOG]

Tex, it is the same file. The A14 is a 14 degree infeed angle for the acme thread. The M19 spindle orientation should not ne an issue for this. My software "geopath" codes the threading cycle like the example. The start position X2. Z.2 M08 determines the start position. If you change the start position to X2. Z.3, you are out of lead. In order to clip the thread, you must split the lead. You have to actually cut the creat of the thread and not the root as you did in the first threading cycle. It will take a few minutes to figure out where the correct start position and the correct Z length needs to be to only cut the starting thread.

I am going buy a digital camera tonight. I hope to send you a picture of the 4" 3 pitch acme connection that the g-code file describes. As soon as you see the picture, it will all make sense.

give me some specifics on your machine, maybe I can figure out your M19 question.
Does it have live tooling?

I hope this helps
|James