3"-6 thread 35" long

[ATG]

I'm trying to thread a piece 35" long. Everything is great until the last 4 passes then the chatter starts. I'm using a Haas sl30 with the big bore and long bed option. The journal on one end in the spindle and the other in a live center. My settings are as follows.

 

Spindle speed 450

Cut equal amount

Amount of first cut .004

2 spring passes

 

Thanks in advance.

[dolphin1]

sounds pretty fast for that course of a thread.what kind of material.what kind of shap is your insert by the last 4 passes.

[ATG]

The Material is 1018CD. The insert looks good. I'm kinda wondering if its the free passes. Maybe it likes the preasure.

 

What would you run it at speed wise I'm will to try almost anything at this point...

[Mr. Dayshift]

Also, confirm with your sales guy or in your catalogue what shim is required below the insert to cut that TPI on that diameter (-1, 0, +1 deg.) This clearance issue will start to show as you approach full thread depth.

 

Does the thread have any signs of rub (maybe an excesses burr).

 

Does that chatter improve towards the chuck or is it even.

 

Is the center engaged enough? Could it be deeper?

 

The spindle speed sounds a little quick aswell.

 

Let us know how you make out.

[ATG]

The Chatter does improve towards the chuck, and as I stated earlyer it does only seem to chatter on the last couple passes. I'll try slowing it down. I'll have to check on the shims I purchased the holder and inserts specifically for this job. Its a Vardex I'll have to check the specifics. I might be able to take the center alittle bit deeper, but not much.

 

Thanks for the help, Keepem comming....

[Philcott]

Are you using a G76 call? If so try making the

"P" address P010030 This will cut down on one spring pass but more importantly will change the infeed angle. This often solves problems I have with single point threading.

 

Disclaimer: I have not ever turned threads 30 plus inches long so I am coming from much shorter parts.

[ATG]

I'm not sure I'm following the p010030 address. Here's a sample of my code.

 

%

O00000 (1004106-C)

(DATE - 09-10-09-14:19)

 

(START TOOL LIST)

( T4 THREADING TOOL )

(END TOOL LIST)

 

 

(T4)

(THREADING TOOL)

N100 G0 G40 G20

N110 G00 G129 X0 Z0 T0

N120 T0404

N130 /M8

N140 G97 S350 M03

N150 G00 G54 X3.2 Z33.0545

N160 G76 X2.7955 Z-.15 I0. K.1022 D.004 A29 F0.1667

N170 M9

N180 G97 S100

N190 G00 G129 X0 Z0 T0

N200 M30

%

[ATG]

In the book it just calls a p1 through p4

p1 being single edge cutting, cutting amount constant.

p2 double edge cutting, cutting amount constant

p3 singe edge cutting, cutting depth constant

p4 double edge cutting, cutting depth constant...

 

Is his what you are referring to?

[Alvaro Gil - Cimquest-inc.com]

You would want P2 or P4 then... this alternates the cutting side of the insert.

 

Id almost go with p4 since you say that towards the end when the material is not cutting much , it starts to chatter. The P4, will keep the cutting depths constant as opposed to keeping the cutting area constant by gradually making the cut depths smaller.

 

If this is not clear let us know.

[ATG]

Ok I'll give the p4 a try with a spindle speed of 300. Thanks guys well know shortly.....

[ATG]

No luck about the same results. I'll Try p2 in the mourning.....

[hugh jars]

A couple of things you could try:

If cycle time is not critical you're still a bit quick on RPM

 

If it's possible to drop centre height a touch that might help, especially if you are rubbing at all due to helix angle

 

Use a partial form insert so that the it doesn't suddenly increase its engagement as you get to depth - in the past we have even got out of trouble by using a neutral T insert for ISO/Unified and neutral D for Whitworth - but it still leaves you some work to do.

Best of luck

[Philcott]

This is an old school trick that has got me out of a few jams.

 

If your machine is not all closed in and you have access to the part while it is running, I have heard, you could try (be careful not to hurt yourself) resting an old broom handle on the part and let it follow the cutter down the part. Again BE CAREFUL not to let the handle catch a jaw or anything and go flying out of your hand. What this does is lets the wooden handle absorb any vibrations created in the cutting process.

 

Did I mention be careful and wear your safety glasses?

[Kevangel]

quote:

---

What would you run it at speed wise I'm will to try almost anything at this point...

---

On long parts and chatter the RPM thing can kill me on my CNC lathe..did you try one going real slow to the extreme and see if that helps? or turn RPM down for last passes? I also have used Phils wooden helper

[DavidSV]

We would use a rubber mallet and hook it under the part and pull. We did about 15 shafts here a few years ago, but a much smaller thread, like 1 1/2 - 12 by about 20" long or something like that. We wore out 2 hammers and 2 operators, but got the chatter out.

[jhjr]

I agree with you guys, with the haas I run if chatter is a problem wile threading I do all the things you guys said P2, broom handle, and slow down rpm. Usually p2 and rpm works. If you have a follow rest that may help also. Your rpm does seem fast, slow way down like Kevangel said. I must say though that the haas lathe I run is less than a year old and is the most chatter prone lathe i've ever run. Haas repair man says there's nothing wrong with it. Last haas lathe my employer will ever buy!

[jhjr]

I had a brain fart earlier not p2 use p1. You already have A29 in your code whitch is tool nose angle, that looks good. P2 cuts on both sides of insert while P1 uses leading edge only. I'm not sure but I think the default for haas if no "P" code is called in the G76 line is P1 if thats case the "P" code won't do anything for you.

[Thee Rickster ™]

+100 to philcott's old tricks.

 

i got a few in the bag similar to that for turning long tapered graghite shafts without a steady rest

[Philcott]

I had another thought on this.

 

We had a lathe once that would sometimes give us chatter if the cutting forces were pulling up on the turret. We would use a threading tool that had an offset head, run the lathe spindle in reverse and the problem would go away since the cutting pressure would now be forced down onto the lathe bed.

 

Just be sure of the tooling and direction of the spindle or you might end up with a left hand thread.

[ATG]

Thanks guys I've tried them all,I still have to try running the spindle in reverse and see what happens. Thanks for all the advice.