Chattering bore

[Howard Jones]

Hello. I am trying to bore a 1.8 in dia x 5.25 inches deep in a CNC lathe. The starting hole size is 1.75. The material is 3.5 inch round 4142. I am holding on to .55 inches of the part in jaws. I am using a 1.25 " shank Kennametal bore bar which is the biggest shank my machine can hold. I am using a triangular Kennametal insert with 321 corner. I have the bar extending 5.35 inches. What speeds and feeds would you fellow CNC'ers recommend? How deep of a cut per pass would be recommended? I have tried different speeds, feeds and depths but still get ugly chatter. Please help. I am very frustrated.

 

[kenton]

I would start at 100 SFM .05 removed from the diameter of the part and .005 per rev. Those are very conservative but almost everything I do is a one off. That should get you started assuming your aren't using 7X14 HF lathe you converted to CNC.

 

[Howard Jones]

I would start at 100 SFM .05 removed from the diameter of the part and .005 per rev. Those are very conservative but almost everything I do is a one off. That should get you started assuming your aren't using 7X14 HF lathe you converted to CNC.

Thank you. I may have been rotating part too fast. Was trying 750 rpm. Will try the conservative approach

 

[Howard Jones]

Too much information.


NOT!

SIZE, power/features or make & model?



Why so little if it is a vanilla cylindrical workpiece?

"Jaws" on what.. as-in CHUCK size & type?
Or are you using some other type of workholder?

Kinda-sorta hints at a too-small "CNC lathe" that won't have any rigidity at the bed, saddle, cross, or toolpost EITHER?

OTOH, if that's a Doosan Puma with FANUC controls, the problem is more likely between your ears than behind its doors.

With adequate workholding, tooling, setup, and code that isn't a hard job for it.

It's a Doosan Lynx lathe with fanuc controls. There is an 8 inch chuck on the machine. The only reason I held on to so little of the part was to try to save an extra op. I can grip deeper on the part and just run a third operation. I have jaws that are 1.3 deep for this dia.

 

[EmanuelGoldstein]

Hello. I am trying to bore a 1.8 in dia x 5.25 inches deep in a CNC lathe. The starting hole size is 1.75. The material is 3.5 inch round 4142. I am holding on to .55 inches of the part in jaws. I am using a 1.25 " shank Kennametal bore bar which is the biggest shank my machine can hold. I am using a triangular Kennametal insert with 321 corner. I have the bar extending 5.35 inches. What speeds and feeds would you fellow CNC'ers recommend? How deep of a cut per pass would be recommended?

You didn't aay anything about speed and feed but I'll give you a lecture anyway - don't even start with rpm. Train yourself to use sfm exclusively when discussing cutting.

Also you need to say whether you are using positive or negative rake inserts. That's important.

5" deep with a one anda quata bar should not be a chatter problem. In steel, for an overall average start point, 400 sfm is good.

I hate -1 inserts. Way too sharp and fragile. -322's will serve you much better.

I'm a fan of negative rake and pushing it. You won't break a chip with less than .015" feed. With a 1.25" bar down a 1.75" hole your biggest problem will be getting the chips out. You do NOT want stringy chips. Make sure they break, and coolant for sure. If nothing else, it helps to lubricate the bore and the chips come out better. If you make sure the bore is open on the back it will help, you'll need to evacuate chips or the bore will be all scarred up or worse, rat's nest, destroy the bore, destroy the insert, potentially destroy the boring bar.

You've only got .025" on a side, that's barely enough to get a nice finish with negative rake. I'd take it in one pass.

That should give you a starting point. You want to cut it, not rub it off.

 

[D Nelson]

Use a Sandvik silent bar
Don

 

[guythatbrews]

Hello. I am trying to bore a 1.8 in dia x 5.25 inches deep in a CNC lathe. The starting hole size is 1.75. The material is 3.5 inch round 4142. I am holding on to .55 inches of the part

Help yourself with a better explanation.

Is the part 5.25 long with a 1.75 thru hole or longer with a 1.75 blind hole? Hope it's thru it's easier. Blind hole that deep sucks. Use as much well directed coolant as you have. You need a thru coolant bar.

Holding .55 deep in a 6"chuck isn't helping you. Not very rigid there, and possibly not very safe. PHold with your deeper jaws and see if chatter subsides. General rule of thumb 4 times length to diameter ratio for steel bar so you are exceeding that by a bit. Others seem to disagree but I'd use a tpg insert. Consider cermet since cutting forces are lower. If #1 radius won't work go to .008R. DO talk about SFM, not RPM. 400 SFM seems reasonable and you are close to that. Chipload will vary with your insert choice. Can't suggest chipload because we don't know chipbreaker style, etc. Look it up online. With only .050 diametral to remove you are talking 2 passes at the most, maybe one depending on finish and size tolerance. Again, a better initial description will help.

Don't hesitate to call tech support. Most (not all) of those guys are very good when you are having a problem. They will help you select the best insert. You'll be time and money ahead.

 

[michiganbuck]

QT I have tried different speeds, feeds and depths but still get ugly chatter. )

If you can safely reduce the length to 4" that may be a small plus.

Sharpness and clearance are often the culprits in boring...and a positive top rake for steel. Good to hold the boring bar with insert or tool bit and check/eyeball that the existing bore radius there is 7* + under the cutting edge and none of the heal is rubbing the ID.

The inside of a bore diminishes the clearance so just having 7* on the insert does not give 7* inside of a bore.

In a pinch draw the radius, perhaps 3x scale so about 16"..and set your protractor on that sketch to see how your insert/bit has clearance. Yes, draw the insert/bit 3 x bigger also.

 

[atex57]

Sometimes the easiest is to make the blank extra long and face it off on the 2nd op. Sometimes I make the blank 2X long and make two parts back to back, lots to grab that way. Sacrifice material to gain stability.

Ed.

 

[cyanidekid]

chattering bore, reminds me of some people ive known...

 

[Mtndew]

I would start at 100 SFM

You're joking, right?
It's 4142 not 60Rc D2.

OP, If you have access to a dampened bar like the Sandvik Silent, use that.
Otherwise you want to go fast enough to actually CUT the material not tear it off.

Now, getting a bar to not chatter is a pain in the ass because every situation is different and every machine has their own quirks.
If it were me, I'd try 750 SFPM (not 750rpm) and feed it about .008ipr for a moderately decent finish. And if you have .05 left in the bore, take it in 1 or 2 cuts and flood the hell out of it.