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?

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.

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

'Rekd

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...:)

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...:(

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

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.

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....:(

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.

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.

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!

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

OK, I've downloaded the file and am studying it now...no need for you to send it by mail again.

I'm using M19 command followed by "P" to stop the spindle at a right angle every time I want to do the thread in the same "phase" with the initial one:

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

Here the start point is X72.2 and Z0 (metric). M19 P180 stops the spindle in an angle 180 degrees offset from zero. Then the threading starts down to 65mm diameter (0.8mm first pass). It is 19mm long, K2.5 should determine thread depth, meaning (if I've understood this command well) that the thread OD is 65 + 2*2.5 = 70mm.

The machine I work on is same as yours...HAAS SL-30 Big Bore...I'm not exactly sure what you mean by live tooling, but if you refer to milling options it does not have any. It does have vector drive, though (which makes M19 command possible to use).

Thank you once more

Peter

Peter, if I am right, you should keep your M19 the same. You should just shift the starting Z to cut the crest of the first thread. All you need to do is get out of lead of the initial thread.

James

Yes, I think I should keep M19 command too...all that is left to be done is to determine X and Z changes between threading and deburring cycle. I have noticed that you change from:

X4.315 Z0.0889 M08
M24
G76 X3.753 Z-1.75 K0.177 A14 D0.008 F0.3333
G00 X4.315 Z0.1605

to:


X4.315 Z0.27 M08
M24
G76 X3.761 Z-0.275 K0.177 D0.008 F0.3333
G00 X4.315 Z0.1605


X4.315 stays the same which is normal...I suppose you change Z coordinate start position from Z0.0889 to Z0.27 to make a grooving tool enter in a right place.

However, I can’t figure out why you change both X and Z coordinates in a "cleaning" pass...from X3.753 Z-1.75 to X3.761 Z-0.275. I understand the change of the Z coordinate (you want to touch just a portion of the fist thread), but why do you change X and how do you determine how much should it be changed? Is there a rule for this or I have to make a few tests before I find the right coordinates myself?

Peter, the change in X was to avoid gouging the connection. After all, it is only .008" larger. You can't hardly see that if the thread was clipped correctly.

You are on the right track. When you go to clip a thread, think of it like this. You are going to cut a thread, but then you will cut that thread off using the same threading cycle out of lead from the first. Only things that will change are the tool and the Z length. I cut a lot of acme threads for the oilfield. I have to clip them so the connections will make up without galling. Once you get it figured out, it is eay to apply that to all threads.

You stated earlier that you needed to clip the rear of the thread. use the same technique, just thread toward the tailstock. the tricky part is figuring out what position the thread exits the connection.

Thanks once more. I will give it a try on Monday. Hope to achieve a good result after a few tests.

There will be more trouble to deburr the end of the thread...we'll se whether is it possible at all.

Will let you know what I have achieved late Monday.

Regards

Peter

Peter, hopefully I will be able to send you the picture by then. Have a good weekend!

James

Looking forward to see the picture.

Have a nice weekend yourself, too...and thnx once more.

Peter.

OK, I've tried to deburr the thread the way that was suggested. It looks fine to me (It is really smooth), but the problem is that the part of the first thread is flattened on one side, vertically...it looks like the grooving tool exits the thread NOT in a helix path (in the phase the thread pitch), but it enters a plain circular path at the end of "Z" and gets out of the thread that way...have no idea how to avoid this.

Peter,

When you say circular path, do you mean like it pulling out of the cut like in a G02 or G03 interpolation? My next question is how wide is the thread you want to cut and what size grooving insert are you using? The grooving insert must be as wide as the width of the thread or wider. Is there a way you could email me a copy of the thread form and the dimensions? I may be able to solve this if I can see exactly what you are doing.

James@glencoofhouma.com

James

James,

I'm sorry for the way I'm trying to explain the problem...I'm not doing it right, obviously....:(...sorry for that.

Let's try it the other way...when I said circular path, I was not referring to G02 or G03 interpolation...the RESULT looks circular on the body (thread). For instance: the first thread was cut (I'll use your example) at the length of 1.75" (Z-1.75) with 0.3333 pitch (F0.3333) and I am doing the second cut at 0.275" length only (Z-0.275) using the same pitch. I've changed the thread starting position according to your instructions, but it is irrelevant to the problem I'm having.

Now, the grooving insert starts going into the thread following the pitch with a certain depth (X3.761 in your example), then it reaches the Z limit (Z-0.275) and then, while still down inside the thread (X3.761) Z motion STOPS, the insert starts getting out of the thread but since the spindle is still rotating and there is no more Z motion, while pulling out, it leaves a mark on the incoming (next) thread. What I need is the insert to follow the pitch until it is completely out of the thread, meaning that when it reaches the end point along the Z axis (Z-0.275) it should already be completely out of the thread, or, in other words, the grooving insert has to still move along the Z-axis following the pitch while getting out of the thread.

The grooving tool I'm using is definitely wide enough (5mm while the pitch is 4.233mm or 1/6").

I hope I have made myself more clear now.

I am mailing you a few files that could help you understand the way the part I'm working on looks like.

Thanks a million....:)

PROBLEM SOLVED!

It looks like somebody's been playing with G95 setting and changed it from default 1.0 to 0.1...this made deburring of the thread virtually impossible. I couldn't believe my eyes when I saw this setting changed...

Anyway, the threads look perfect now...at the beginning AND at the end...:)...thanks everybody, especially WOLOG.

Peter

Peter, I am glad everything worked out. If you ever need anything send me an email.

I will still send you those pictures just as soon as I get a chance.

James