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

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,

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
%

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?

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.

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

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?

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.

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.

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

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

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.

I'm in the same boat as pdoherty. I do not know the Haas cycles and can only give general suggestions. I also agree that anything you can do to stiffen up your part will be a big help.

Alain,

i would say that its your insert. That on edge insert has absolutely no chip breaker which causes smaller machines problems. We have two DS&G hollow spindle lathes with 10 5/8" holes and we still have some problems with chatter every now and then. I can not stand to thread with "v bottom" style or "on edge" inserts. Especially on deep threads like IF and Regular.

I have another suggestion. Try running two threading cycles. The first one would be to remove the majority of the material. Maybe a 60 degree thread or so. Then try running your topping insert to finish the last couple of passes.

Also try an infeed on your thread. I think a G32? will work better. I will try programming a regular connection in the morning with an infeed angle and see what will happen. If I have a few minutes, I will cut one to see if I can solve the problem on my TL-2.

http://www.vardexusa.com/vardex-pdf/vardex_tt_inserts_17-92.pdf

Check out Vardex for a laydown insert for your regular connections. I would find a laydown style insert with a positive rake on the nose.

Alain,

One more idea for the evening. Cut your connection before you machine the rest of the part. The added mass may dampen some of the vibration. Can you move your steady rest closer to the pin?

By the way, I hate cutting connections because of things like you are going through with this part.(nuts) SORT OF FEELS LIKE THAT!

Alain, could you do me a favor and post some detailed photos of that steady rest. How it mounts to the lathe and it overall structure. Thank you.

Alain,

i would say that its your insert. That on edge insert has absolutely no chip breaker which causes smaller machines problems. We have two DS&G hollow spindle lathes with 10 5/8" holes and we still have some problems with chatter every now and then. I can not stand to thread with "v bottom" style or "on edge" inserts. Especially on deep threads like IF and Regular.

I have another suggestion. Try running two threading cycles. The first one would be to remove the majority of the material. Maybe a 60 degree thread or so. Then try running your topping insert to finish the last couple of passes.

Also try an infeed on your thread. I think a G32? will work better. I will try programming a regular connection in the morning with an infeed angle and see what will happen. If I have a few minutes, I will cut one to see if I can solve the problem on my TL-2.

http://www.vardexusa.com/vardex-pdf/vardex_tt_inserts_17-92.pdf

Check out Vardex for a laydown insert for your regular connections. I would find a laydown style insert with a positive rake on the nose.

I used on edge inserts, i´ll be thankful if you cut a regular connection in your TL-2, send me some picture to see the cutting part.

Thank you for your time.

Alain

Alain,

Mi nombre es Milton Ramirez y soy Ingeniero de Applicaciones para Haas Automation, Inc. en Oxnard, California (La fabrica). E estado leyendo que has tenido algunos problemas roscando con tu TL-3. Yo con mucho gusto te puedo ayudar si asi lo deseas. Por lo pronto e estado viendo algunas de tus fotos y note que tienes usando la luneta fija y contrapunto. Tambien note en uno de los ejemplos de programas que pusiste que estabas usando RPM de 150. Con respecto a las revoluciones por minuto no se que material estas usando pero cuando hice los calculos basado en cortar material no aleado de alto contenido de carbono o sea un acero de herramienta, las RPM recomendadas son de 350 a 750 revoluciones usando una herramienta de corte de carburo de tungsteno. Habiendo dicho esto, dejame recalcar que la maquina Haas a sido diseñada para cortar preferiblemente a altas revoluciones y cargada con corte.
El otro punto muy importante que note en tu programa en la Linea de G76
(G76 X2.6544 Z-2.875 I-0.38 K0.1178 D0.022 F0.2) fue que no tienes una definicion de P1 o P3 que son las mas recomendables para este tipo de roscado. El P1 o P2 debe ir acompanado de la letra A (ejemplo A60) que indica el angulo de la rosca para que vaya deslizandose sin cortar en el angulo de atras. En fin, prueba esto que estoy seguro te va a ayudar. Hay otros settings importantes como el setting 86 y 99 y tambien la letra D en la linea G76.
Me encantaria poder ayudarte mas si lo necesitas. Por favor contacteme direct a la direccion de abajo y dile a los compañeros de el Thread este que Haas tiene excelente ayuda disponible para cualquier usuario de nuestras maquinas en Ingles y español segun la necesidad. Espero tu respuesta. Saludos.

Milton Ramirez
Applications Engineer
Haas Automation, Inc.
www.haascnc.com
mramirez@haascnc.com

For us english speaking folk, Courtesy of Babel Fish:

My name is Milton Ramirez and I am Engineer of Applicaciones for Haas Automation, Inc. in Oxnard, California (it makes It). And state reading that you have had some problems threading with your TL-3. I with much please I can help you if asi you wish it. So far and been seeing some of your photos and he notices that you have using the lens fixes and counterpoint. Also he notices in one of the examples of programs that you put that you were using RPM of 150. With respect to the RPM not that material these using but when I made the calculos based on cutting to material nonalloyed of high carbon content that is a tool steel, the recommended RPM are of 350 to 750 revolutions using a tool of tungsten carbide cut. Having said to this, dejame to stress that the maquina Haas to designed to cut preferably to high revolutions and loaded with cut. The other very important point that it notices in your program in the Line of G76 (G76 X2.6544 Z-2.875 I-0.38 K0.1178 D0.022 F0.2) was that you do not have a definition of P1 or P3 that is but the recommendable ones for this type of threading. The P1 or P2 must go acompanado of the letter A (A60 example) that indicates angulo of the spiral so that it is slid without cutting in angulo of atras. In short, test this that I am safe is going to you to help. Settings like setting 86 and 99 are important others and also letter D in the G76 line. Encantaria me to be able ayudarte but if you need it. Please contacteme direct to the direction of down and dile of the companions of the Thread this that Haas has excellent aid available for any user of our maquinas in Ingles and Spanish segun the necessity. I wait for your answer. Greetings.

Dean,

Thanks for the translation, I focused on helping our friend Alain in his native language and forgot about how important this forum is to a lot of people, since it could easily be the only source or contact with technical people or advice. I am in contact with him directly already via email. Babel Fish does not do a good job when it comes to technical terms so from now on if and when I reply to threads I will write in both english and spanish if its neccesary.
Thanks again and please do not hesitate to give me a call or send an email if you were to have any questions or need of assistance with your Haas products. It is my Job to assist the customer to achieve their production goals and use the Haas machine efficiently.

Regards,

Milton Ramirez
Applications Engineer
Haas Automation, Inc.

Hey Milton, I am glad that there are members from HAAS here to answer questions. Babel Fish does do a pretty weak job on tech terms.

Question: Why doesn't HAAS have a official forum??? It seems like it would be VERY easy for a company like HAAS to set one up. Look at it as a just another tool in their customer service. I know there is the 'Answer Man' but it would allow users to meet.

Hi Dean,

It is a good point that I am sure our marketing department has considered. I think the reason why it does not happen is because it would take away from our personalized customer service which is our goal. Forums for the most part are very casual but sometimes are also used as a debating platform which is something we are definetely not interested in doing. We also have a very strong network of local dealers to whom we direct our customers to so that the support is localized, personalized, quick and effective. Also, the workload is distributed per region worldwide. A forum might still be something to consider in the future.

Regards,

alain;

I suggest taking the Steady away and moving your threading tool to the other side of the toolpost. This will allow you to move the saddle closer the the chuck and move the Tailstock so your center is not hanging out as far. Also as someone suggested use a deeper center hole and a shorter center.

I have tried to cut Rotatry shoulder conections on a TL-3W, using a heavy duty steady rest with the tailstock in and had the same problems. The tailstock, steady, toolpost and entire saddle would shake, rattle and roll.

The really experienced guys in the shop gave me there 2 cents and I tried every depth and rpm combo, but it would still end up full of chatter. We had a tooling tech rep from Kennametal and all of his ideas wouldnt work either.

We solved the problem buy doing them in a big bore SL-40, so we could chuck as close as posible. Even with that there is still slight chatter issues, there is just so much thread ingagement going on.

The shop manager was not very pleases, thats what the TL-3W was bought for and it cant do it worth a crap.