rotary shoulder connections on TL-3

[alain aleman]

Hi guys, i have a TL-3 and i have problems to make rotary shoulder connection, the principal trouble is the vibration, the thread look so shake it and the tool chatter continously, someone make this connection for oilfield industry using TL Haas lathe model?

Sorry for my english, i from Peru.

Alain

[WOLOG]

Alain,

What connections are you cutting? I have had this problem also. It has to do a lot with the setup and all the other associated things you might expect. Give me some info and I will try to help. Do you know that you can change your rpm's for a thread as long as your starting "Z" point is an increment of the thread pitch from "Z 0" Ex. 8 pitch=.125 , thread starting point... Z.250, Z.375, and so on.

[alain aleman]

Originally Posted by WOLOG Alain, What connections are you cutting? I have had this problem also. It has to do a lot with the setup and all the other associated things you might expect. Give me some info and I will try to help. Do you know that you can change your rpm's for a thread as long as your starting "Z" point is an increment of the thread pitch from "Z 0" Ex. 8 pitch=.125 , thread starting point... Z.250, Z.375, and so on.

Hi Wollog, i make the following connection: REGULAR, INTERNAL FLUSH, H-90, EXTERNAL UPSET END, NON UPSET AND MORE, BUT THESE ARE THE PRINCIPAL THAT A COMPANY MANUFACTURE.

This is the program:

%
O00040 (MOLINO 5 1/2 X 20)
T101 (2 7/8 REG PIN)
(DESBASTE-ACABADO)
G20
G50 S1000
G97 S900 M03
G96 S300
G54 G00 X5. Z0.1 M08
/ G71 P1 Q2 U0.014 W0.008 D0.05 F0.012
N1 G42 G00 X4.9 Z0.1
G01 X1.875 F0.005
X2.193 Z-0.159
X2.89 Z-2.875
Z-3.3125
G02 X3.015 Z-3.375 R0.062
G01 X3.578
X3.875 W-0.1485
Z-15.75
X4.6457 Z-16.
W-0.75
N2 G40 X4.9
G54 G00 X5. Z0.1
/ G70 P1 Q2
G00 X8.
M00


T202 (ROSCA 2 7/8 REG)
G20
G50 S1000
G97 S150 M03
G54 G00 X3.3 Z0.1 M08
G76 X2.6544 Z-2.875 I-0.38 K0.1178 D0.022 F0.2
G00 X4.5 Z0.1 M09
X8.
M30
%

[WOLOG]

OK,

How much of the connection is out of the chuck? I would say that a lot has to do with the insert you are using. Are you using "V bottom" style inserts? I have more problems with those type inserts. They do not have any type of chip breaker which can cause chatter. Another thing that you may try is setting your thread insert height a little low rather than right on center. Are you using coolant or cutting oil. As much as I hate to poor cutting oil in my semi-synthetic coolant, it works much better. The coolant is not slick enough for threading deep threads.

Try threading a little slower. You may have to slow down to about 50 rpms for the last couple of passes. I would also try getting rid of the G76 and go to G32. You have better control of your threading. Also, try taking deeper cuts. Light cuts leads toward chatter.

Let me know if any of this works. I will look at some of my programs to see if anything looks similar. I guess the material you are cutting is 4140HT?

[CNCBoss]

We use to thread rotary shoulder tools. The best advice I can give is check your workholding. Chuck up as close to the thread as possible, use pie jaws to increase surface contact and damped chatter. Make sure your toolholder is as close in as possible. If the tool hangs out too much you will get chatter. If all else fails use the tailstock and center in the connection. After that it is all about finding the "sweet spot" for speed. Good luck.

[alain aleman]

Wolog, i try to make with 50 Rpm but is same. The insert has a special geometry , and center tool is ok, also i trying with 0.017" deep of cut per pass, nothing. you are right, the material is SAE 4140.

Hi, CNCBoss. I´ll be thankfull if you send me some pictures when you make this kind of connections (rotary shoulder connections), i tell you that i used the tailstock because the leng of the crossover that i make is 20" or 25" and the diameter of 5" to 6", my HAAS TL-3 has 3.5" of spindle bore. Also I use steady rest, also nothing.

Thank guys for your attention,

Greetings from Peru.

Alain

[DEAN]

It looks to me like toolholder is not rigid enough. The insert is not staying in the cut because of rigidity or geometry.
What does your insert look like? Are you sure it is seated in the tool holder correctly?

[pdoherty]

alain,

I bet that sounded awful when it was running. Makes me cringe thinking about it.

A depth of 0.017" or even 0.012" per pass seems like a lot, especially that far away from the chuck. We don't do these types of connections, but we do cut a lot of 4 TPI 60 degree threads and sometimes ACME and we normally go 0.005" per pass and this is on a box way Daewoo lathe. Sometimes we go more, but we usually start at 0.005".

The other trick that we learned is to make that center hole as big as possible. We use a 1.25" diameter combined drill & countersink and bury it in the end of the part. This provides way more contact with the live center in the tailstock and much better support/dampening.

If you have a way to program 'zig-zag' threading (cutting alternating flanks each pass) that would help also. I'm a little weak on G Code programming but I believe that most CAM lathe packages have this cycle.

[WOLOG]

Alain,

You may need a bigger machine. The fact that you are using the tailstock/steadyrest is a problem with a connection that far away from the chuck. The TL-3 Big Bore has a 8.8 or so hole. I really don't think you will have a lot of luck with a Tl-3 standard machine if you are doing a lot of connections and crossover subs. Have you tried to use the tailstock and the steady rest at the same time? I know that will only help with the pin; however, that's half of the battle. Post some pictures of the toolholder and the inserts and such.

[alain aleman]

Ok guys, here post another pictures where looking the toolholder with the insert and the part to cut. Dear pdoherty, thanks for your advice but i got a questions, you say me that i should put 0,005" per pass but in HAAS control exists a formula to obtain the deep of cut, D= K/ sqrt N.

D: deep of cut per pass
K: high of thread (radius value)
N: number of passes

If i put 0,005 in "D" and the value of "K" for the thread that i cut is 0,11784", i obtain more than 500 passes. What are you think about it?

Thank you for your time.

Alain

[CNCBoss]

Are you infeeding this thread? Radial feeding will put too much surface contact and cause chatter.

[pdoherty]

Alain,

It looks like you are doing 'constant load' threading.

The constant load cycle reduces the depth of cut as the thread gets deeper, so I guess 0.005 is not a good place to start unless you can specify a minimum depth of cut. Looking at the Haas Lathe manual, it appears that there is a way to do this.

There is also a way to change the infeed angle as CNCBoss has suggested.

Based on your photos, I would definitely want to have that live center go deeper into the part - i.e. a bigger center hole.

It looks like you are using a 'top-notch' style insert, so there should not be any helix angle issues the way there are for 'lay-down' inserts.

I wish I knew the details on the Hass threading cycles better, but I don't. Sorry.