Machining Chatter 1

[Schuyler]

I have a component that has machining chatter on the threads. The threads take a locknut which has a torque of 1,000 in-lb. The material is a 1050 temper PH hardening stainless steel. The threads are acceptable via "go", "no-go" gaging. Is there a typical criteria or methodology for determining if chatter is acceptable? Is there a specification which spells out specific acceptance criteria for chatter?

Thanks

 

[EnglishMuffin]

Well, if there is a surface finish criterion and the part meets it, that would be one possibility. But I don't believe chatter is ever really acceptable, and since it either occurs or it doesn't, there is usually some way to avoid it. Just out of interest, are you plunging radially in (cutting on two thread flanks simultaneously) or are you feeding in at 29 1/2 degrees (cutting essentially on only one flank)?. The latter approach is less prone to chatter. Of course, if you are using some form of die approach you don't have much choice.

 

[ccw]

Hi Schulyer,
I have seen this (chatter) more on SST internal threads where boring bar support is difficult. But, here you imply these are external threads. EnglishMuffin is correct in that you probably need to "stiffen" the setup. The chatter usually occurs on or near the final pass when you are using a 60 degree tool to make Unified profile and there is maximum drag on the cutter. Are you cutting with a single point tool? Are you as close to the headstock as you can get? Are you going for maximum rigidity on the tool holder? Are you using a tail stock or saddle support? New cutters?

One other thing that might make a marginal difference is to take the 1050 temper material to its "free machining" temper before threading. For instance 17-4 PH SST has a 1150M temper optimum for machining. However, this doubly complicates the final temper process if you need to get back to 1050.

If you decide to use as is, you might consider electropolishing the finished threads, then heavy use of a thread lubricant such as molylube or graphite to compensate for the friction of the chatter marks. This would be to asssure the 1000 in-lbs lock nut does not give a false sense of clamping load vs. torque.

 

[GeWood]

Hi Schuyler,

I agree with the other posts.
You do not say if this is a CNC or manual machine.
1) The first thing I would look at is your cut speed. Too high a cut speed will affect your chatter as much as too little depth of cut per pass.
Use recommended cut speeds to start with if you have a rigid set-up.
[INCH] RPM = 3.82 * SFM / Dia. of the cut in inches
[Metric] RPM = 318 * SMM / Dia. of cut in mm

2)You want a short rigid tool holder machining as close to the chuck, or tailstock as possible. Use as high a chuck and tailstock pressure as can be tolerated with out distorting the part/chuck/jaws.

3) Typically for harder materials it is preferable to decrease the infeed angle as low as 10-12 degrees. At 29.5 using decreasing depth (Constant Volume Threading) the tool pressure on this tough gummy material keeps building up, even breaking some carbide insert tooling towards the end as each pass keeps building up more deflection. Decreasing the infeed angle helps to alleviate this problem. It is important to get enough bite in this material; at least .002" to .003" minimum depth of cut. No "Spring passes" as they only rub the tool wearing it out faster anyway. It is important that the tool is on center, and not leading (above) the center, or it deflects down and into the material adding to chatter problems.

Chatter is a poor business card to send to your customers.
Thanks,
GWood@gbiCincinnnati.com

 

[griffengm]

Schuyler,
The other posts are correct but there are a couple of other factors that I found make a difference as well.
The relief ground on the cutter can cause a rubbing action and so set up flexing. One of the other posts suggests varying the infeed and sometimes finding the correct combination of relief and infeed works.
Somewhat related to this is the height of the tool relative to centerline. In my experience, we ran the tool slightly above the centerline when ID cutting to maintain a good relief. If run too high, you will end up trying to wipe material with an extremely negative rake relative to the material; if run too low, you lose the benefit of the relief angles on the sides and nose.
When working on ODs, you will want to be slightly below centerline. By running here, you may be able to decrease some of the relief and thereby use a little stronger tool.
It sounds from your post as though you are taking some relatively wide cuts relative to the cutting edge. I found that as width of cut increases, sometimes the rake needed to increase to lessen the shear pressure on the edge.
Chatter generally seemed to be a matter of pressure building up to the point that the tool or work had flexed as far as it could and snapped back into position. Then the next cycle started. Consequently, uniform loading through either depth of cut, rate of feed, or tool geometry would reduce the problem.
Hope this helps.

Griffy

 

[Nate101]

Most B/P's, customer manufacturing requirements or thread spec.'s have ASME B46.1 called out, or something similar to, for the surface features of a thread. Chatter looks bad and even lowers the striangth of the thread. PH series stainlesses work hardens also so don't cut back on the depth of cut because of a weak setup. Like everyone said, a rigid threader and setup is required, proper surface footage and depth of cut, material grade and coating of threader, also.
Good luck.