Thread deburring

[tex]

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

[WOLOG]

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

[tex]

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?

[WOLOG]

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.

[tex]

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

[WOLOG]

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

James

[tex]

Looking forward to see the picture.

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

Peter.

[tex]

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.

[WOLOG]

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

[tex]

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....

[tex]

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

[WOLOG]

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