Relationship of nose radius to chatter?

I am trying to use a Multi Directional Turning tool to do some profiling on aluminum (specifically an ISCAR TGDR -4 type). To achieve the profile I am using the round nose insert, radius is 0.079. It squeals like Ned Beatty in 'Deliverance', especially when feeding in X, cutting on the right hand side of the radius. Less so on the left hand side (which generally means the tool is feeding out in X). It happens even in light depth of cut passes. I have explored a range of speeds and feeds without any real difference, though I am running very slowly for carbide in aluminum. The usual 'decrease speed increase feed' does not seem to work here - though I haven't pushed anything to the breaking point yet .

These tool holders have a very narrow section, like a cut off blade. Is this the nature of the beast? Would using a more square, small corner radius insert make a big difference? That wouldn't help on my finish pass anyway, because the profile cannot be achieved with that insert. In the MDT videos from Iscar, Seco, and others they show going after steel much more aggressively than I am attacking this aluminum. Wonder what I am doing wrong? Is running at low SFM making the problem worse?

A narrow section tool shaped like a parting tool will lack rigidity in turning operations, can't fight physics. Having a relatively large radius just increases the engagement of the tool, increasing the likelihood of chatter. Rough it out with a 15 degree diamond inserted tool with a small toolnose radius if possible, and finish with the smallest toolnose radius you can use (although if this then dictates using an even narrower tool b/c you need a full 180 degree toolnose radius, then it's not likely to get better).

Joe

If you are turning in both directions, you need to eyeball the square end of the insert positioned almost touching a chucked cylinder to make sure it is perfectly parallel to the part. A relatively aggressive feedrate is required to deflect the insert just enough to produce the clearance that prevents chatter. Typically you could finish at .015"/rev and get excellent results, but your final depth of cut needs to be about .03" to work. Lighter finishing passes are to be avoided.

Having said that, the 2mm radius is a large radius on the insert. I typically use no more than 1/32 nose radius, and profile the part radius if it is larger. Of course you cannot get a good profile at a high feedrate, so you might have to feed aggressively almost to the shoulder, then retract and recut the shoulder with a facing path ending with the fillet radius. On the light facing cut you can feed more slowly, but since you are using the insert in its strongest plunge configuration, it should not chatter.

Whats the length / dia ratio of your workpiece?

Is it supported by the tailstock?

scudzuki said:

A narrow section tool shaped like a parting tool will lack rigidity in turning operations, can't fight physics. Having a relatively large radius just increases the engagement of the tool, increasing the likelihood of chatter. Rough it out with a 15 degree diamond inserted tool with a small toolnose radius if possible, and finish with the smallest toolnose radius you can use (although if this then dictates using an even narrower tool b/c you need a full 180 degree toolnose radius, then it's not likely to get better).

Click to expand...

I agree they would seem to lack rigidity, however the manufacturers show quite aggressive profiling with these tools. I need nearly a full 180, I was trying the part using a VNMG type tool but on the faces it is cutting nearly on the straight part. I am roughing by plunging a cut off tool because the MDT chatters so much - but if you believe the literature I shouldn't have to.

I have a -3 of the same series (0.059 nose radius) is the consensus that the smaller radius would chatter less? The tool holder is that much narrower, so less rigid....

HuFlungDung said:

A relatively aggressive feedrate is required to deflect the insert just enough to produce the clearance that prevents chatter. Typically you could finish at .015"/rev and get excellent results, but your final depth of cut needs to be about .03" to work. Lighter finishing passes are to be avoided.

Click to expand...

Since this is a round nose tool (it cuts around about 235 degrees) there is no such thing as deflecting the tool to achieve clearance, as there would be with a square tipped one. I have tried depth of cuts from 0.005 to 0.030, deeper cuts just make it sing louder.

Having said that, the 2mm radius is a large radius on the insert. I typically use no more than 1/32 nose radius, and profile the part radius if it is larger. Of course you cannot get a good profile at a high feedrate, so you might have to feed aggressively almost to the shoulder, then retract and recut the shoulder with a facing path ending with the fillet radius. On the light facing cut you can feed more slowly, but since you are using the insert in its strongest plunge configuration, it should not chatter.

Click to expand...

The profile is a continuously changing tulip shape, a special "tulip" sheave for a custom sailboat block. So there is no bottom or face really, all a continuous curve. Since it cuts much better coming out of the tulip, I could cut from the bottom each way, but curiously plunging with it seems to chatter worse than anything.

Limy Sami said:

Whats the length / dia ratio of your workpiece? Is it supported by the tailstock?

Click to expand...

3" 6061 aluminum, about 3" hanging out of the chuck, no tailstock. The tool chatters as badly right next to the chuck as at the end of the workpiece.

Iscar says 1200 rpm (1000 SFM), .060 depth of cut, 0.008 ipt. I haven't tried running that deep (but the singing gets worse the deeper I go), and I haven't tried running that fast (would have to stop and shift gears). I am only running about 400 rpm. For plunging they recommend 230 rpm and 0.010 feed. Would running a lot faster be expected to reduce the singing?

Can you get away with a little wider tool?

I do this kind of work pretty regularly with a .125 wide tool in 6061.

Pretty much got to keep moving to keep the chatter at bay. But I generally don't have a problem.

BTW. I use Manchester MTC tools.

I use Seco MTD tooling a lot in aluminum and as mentioned you MUST take a sizeable cut (depending on your radius) and you must feed it aggressively in order to get the tool to deflect and cut as it should.

Now I've never tried a full radius insert like you are using, but I can only imagine the science behind it would still be the same......get it in there and get it done. The finish will come out beautiful!!

If they are telling you to take a specific minimum depth of cut at a specific feedrate and you are not..........therein could be your answer.

Later,
Russ

Turning with too shallow of a cut with a large nose radius tool turns axial force into radial force. The tool won't deflect under this condition but the workpiece will.

We can better evaluate what's going on with a few more details:
1. Diameter of workpiece
2. Length of workpiece extended from chuck
3. Depth of cut
4. Feedrate

-Sol
Glacern Machine Tools

ARB - the tool I am using is 0.158 (0.079 radius).

Wrustle - the explanation for feeding hard to gain relief clearance is not valid for a round nose tool. The same profile is presented no matter how far you bend it. I need to try running at the SFM they suggest (but I am not running flood coolant), but I have tried the other parameters. What sort of speed/feed/depth are you running with the Seco tool?

Sol - see previous posts, all the info is there. I can feed all kinds of other tools at pretty much any speed or feed on this setup with no squeal. For example at the same speed/feed I can plunge a 0.120 cutoff tool without trouble the round nose 0.158 squeals badly.

I am curious as to why feeding the tool at around a 45 deg angle in towards the center and chuck squeals so much worse than it does feeding at a 45 away from center and towards chuck. Same speed, same feed, same dia, same material, same tool. With the round nose on the in feed it is cutting a little more towards the tip, feeding out a little more around the side, but not much different. Dramatic difference in the noise and finish.

Oops. I mistakenly thought your were talking width. I should have known.
I have found that some directions of travel can be more problematic than others. It usually comes down to DOC and feed.

I am going to be running some 3 inch balls this week and I'll check my parameters. Usually going like hell.

Swarf_Rat,

What they are talking about is loading up the tool so it cannot bounce.

That tool acts just like a boring bar. If you don't load the tool up enough, the springiness gets you. The tool deflects downward when you engage the cut, if you don't have enough load on it, it'll bend so far, then spring back. This sets up the oscillation known as chatter as it repeats. Any tool that is weak will do this. Go to the recommended feeds and speeds and see what happens. Turning too slow is just as bad, if not worse than turning too fast.
Especially in aluminum, because it builds up on the tool, then breaks off, changing loads on the tool. 400 RPM is way out of the ballpark on SFM.

You may want to experiment with changing tool height.

Despite what many will say there is nothing "magic" about being on C/L on a lathe unless you a cutting to a zero dia.

As I don't have prints for your inserts, do not know your part dia. and haven't seen a used tool I don't which direction (up or down) to go. Up will decrease clearance and make the tool "rub" more damping vibration (sometimes at the expense of tool life). Higher federates also decrease heel clearance which is why they will often "dampen" chatter. It's a common mistake to think increasing feed loads the tool more when in fact it's the change in clearance (in the area the material springs back after cutting) that dampens the system.

That said regenerative chatter can come from lots of areas. Without suitable vibration measuring equipment it can be a real pain in the arse to nail down.

Try changes that will move the tool about 2 degrees.

Note that this just a suggestion, I hate trying to diagnose a tooling problem if I can't touch, feel, and smell the machine.
Bob

Tonytn36 said:

Swarf_Rat,

What they are talking about is loading up the tool so it cannot bounce.

That tool acts just like a boring bar. If you don't load the tool up enough, the springiness gets you. The tool deflects downward when you engage the cut, if you don't have enough load on it, it'll bend so far, then spring back.

Click to expand...

I may be mistaken, but I think we are talking about sideways deflection to gain clearance. MDT tools are unique in that the square nosed versions do not have side clearance because you can turn both directions with them. The theory is that the tool deflects to the side if fed hard enough, which changes the angle of the insert and creates clearacne. Does not work on a round nose though. And to clarify, these inserts are round - the useable cutting edge extends about 235 degrees around the insert. If springyness down was the culprit, I would think that there would be no difference turning on the right flank vs. the left flank. But then I have no other theory to propose either.

Tonight I am going to try running up to the recommended speed, hope nothing breaks.

Edited: I should have said clearance, not relief

I made a mandrel the other day to bend some tubing out of 2.125 od 1215 steel. It was just a groove .375 deep with a .187 radius in the bottom of the groove. I used a seco mdt tool with a full radius insert. IIRC the insert was 4mm wide. I used seco's recommended speeds and feeds. I don't remember the exact speed but it was around 1000 rpm with .008 ipr feed and I used .060 doc. The tool worked flawless no chatter at all. I almost had to duck from the shower of chips it threw off, the machine was a Haas TL-1, so no enclosure I only made one part and the insert looked like it was new afterwards. I would start with the mfg's recommended speeds and feeds and just let er rip.

I use the GHDR-4 on a Haas TL-1 with the 4-position tool changer (which has no adjustment for height).
I had all kinds of chattering problems, until I checked the tool height.

I ended up lowering the cutting height by milling about .020 from the bottom of the GHDR tool holder -- this greatly reduced the chatter.

Thanks for all your thoughts.

I bucked up and tried a few things. I must admit to being a pussy (cat) when it comes to running fast and hard. I tried several different feeds and depth of cut, no difference. Then I started speeding things up. At 1000 SFM, cut was smooth, no singing, mirror finish, feed and depth of cut didn't matter. Slowing down it kind of goes to hell around 800 SFM, and its pretty bad by 600 SFM. I had been running at 300 SFM. You are right about having to duck the chips (but fortunately the Trak has an enclosure!).

I know you guys do this all the time, but I cringe at running this 10" chuck at 1400 RPM. Just seems like if anything goes wrong something is going through the wall. The chuck is a Bison steel bodied, rated at 3500 rpm so why should I worry? I do though. Seems like a lot of energy involved.

Mostly I have been turning stainless. Maybe tough, but you get to run it real slow.

Edster, when you say DOC of 0.060 is that dia or radius?

I know you guys do this all the time, but I cringe at running this 10" chuck at 1400 RPM. Just seems like if anything goes wrong something is going through the wall.

Click to expand...

Let 'r rip. I had a 12" scroll chuck on a Milltronics ML20, ran it at 2200 rpm all day long.

I agree with the centerline "adjustment" suggestion. Oftentimes tweaking a tool very slightly above or below centerline can make a world of difference.

Oh, 1400 rpm's would be fine for the 10" Bison chuck.

Edster, when you say DOC of 0.060 is that dia or radius?

Click to expand...

Radius. I plunged in .060 than moved to the side and plunged again and moved to the side again until the groove was roughed out. I've been using these tools for a while for cutoff but this was the first time I did any actual turning. So far I'm impressed with the tool and I can't wait until the next job I can use it on. Btw, the toolholder I was using was also the longer reach one, I bet the shorter one can be pushed a lot harder.

Thanks for the info.

I have rewritten the program to speed everything up and use the MDT tool for roughing as well. Since the DOC didn't seem to make any difference on chatter or finish, I will probably be a little more conservative there.

Next I am going to try using one of Iscar's MDT type face turn-groove tools to cut a ball track in the face of my sheave. I tried a couple of test cuts, it doesn't seem to squeal like the straight one, even at somewhat lower speeds. I guess because the curved insert support stiffens it sideways considerably. The ball track has to be undercut so that the Torlon balls snap into place and are retained. I think this tool will do it, not sure how else they might be machined.