Reamed hole undersized

welder2022 · Dec 1, 2017

I am reaming thru holes in a cnc lathe in a tubular part 14" lg, 4135 steel, 26-30 R/C, .280 hole thru to start with, .812 stock o.d.
.2930-.2938 tolerance. Using a .2933 5 flute str. flute cobalt reamer 16" oal, 14.2 hanging out and shank is .250. Right now using 400 rpm, .006 ipr feed, peck cycle 1.0 peck depth. Coolant is pumped in thru one end of the part, reamer comes in the other so it's "swimming upstream" so to speak. Coolant is semi-synthetic at 5%.
Have used 600 rpm. Chatters and cuts over for first 2" so no good. Starting with 400 rpm for first 2" seems to cure that.
Right now using 400 rpm for entire length, I thought the tool was maybe rubbing so running slow to check this.
Parts are coming out .001-.0005 undersize. Have to rework i.d.'s with flap tool to get them to gage.
Help please.

HuFlungDung · Dec 1, 2017

The fact that it chattered at higher speed may be indicative of a problem with the reamer's sharpened geometry, and it may still be chattering at an inaudible level, making a lobed hole that won't allow a gage to pass. Might be detectable with a small dial indicator. Try one of the other two reamers you have handy....you didn't think you'd get away with one, did ya?

litlerob1 · Dec 1, 2017

welder2022 said:
I am reaming thru holes in a cnc lathe in a tubular part 14" lg, 4135 steel, 26-30 R/C, .280 hole thru to start with, .812 stock o.d.
.2930-.2938 tolerance. Using a .2933 5 flute str. flute cobalt reamer 16" oal, 14.2 hanging out and shank is .250. Right now using 400 rpm, .006 ipr feed, peck cycle 1.0 peck depth. Coolant is pumped in thru one end of the part, reamer comes in the other so it's "swimming upstream" so to speak. Coolant is semi-synthetic at 5%.
Have used 600 rpm. Chatters and cuts over for first 2" so no good. Starting with 400 rpm for first 2" seems to cure that.
Right now using 400 rpm for entire length, I thought the tool was maybe rubbing so running slow to check this.
Parts are coming out .001-.0005 undersize. Have to rework i.d.'s with flap tool to get them to gage.
Help please.

I really hate Reamers!! BUT this application seems appropriate for one. They are never exactly what you want or expect. I mean literally, when one cuts on size, it's enough to make a dozen grizzled Machinists stand around in a circle asking what happened to make the Reamer cut on size.

Couple things; what size is the hole that you are Reaming? (actual size, not Drill diameter). How round is the Drilled hole, how on center is the Drilled hole?

Also, I hope that ".006" feed" means per cutting edge, not over all.

R

billzweig · Dec 1, 2017

How do you measure the bores? Lobbed holes might show as undersized. Could be a dull or damaged reamer, too high speed/feed....

extropic · Dec 1, 2017

I would have chosen a spiral flute reamer because there's more resistance to creating a 'lobed' hole. Any chance of getting solid carbide to minimize wind up in the shank?

OT: First post and such a well asked question. Welcome.

Bobw · Dec 1, 2017

I'd bet a 1/2" 1.25loc 4fl .03R Maritool HotMill that the hole is mostly fine on size,
but it isn't straight.

jrmach · Dec 1, 2017

My guess too,,,the "Wankel " effect,,,,,lobed

Revelstone · Dec 1, 2017

If you want a true sized hole. First drill then end mill bore .004 dia. undersize then ream with a carbide reamer. I guarantee a true sized hole within .0002 of the reamer size provided the reamer is indicated in within .0002 and the runout is also negotiable because the reamer will follow the hole.

welder2022 · Dec 1, 2017

litlerob1 said:
I really hate Reamers!! BUT this application seems appropriate for one. They are never exactly what you want or expect. I mean literally, when one cuts on size, it's enough to make a dozen grizzled Machinists stand around in a circle asking what happened to make the Reamer cut on size.

Couple things; what size is the hole that you are Reaming? (actual size, not Drill diameter). How round is the Drilled hole, how on center is the Drilled hole?

Also, I hope that ".006" feed" means per cutting edge, not over all.

R

The actual hole is right at .280-.281 and concentric within .001
The reamer is mounted in a split bushing that was drilled while mounted in the lathe.
The feed is .006 ipr for the tool not per tooth.
I am trying to be conservative with this because I'm taking out .013 on the diameter.
Using 2.5 lg. center relieved Deltronic pin gages. Shooting for slip fit on the .2930 gage.

allloutmx · Dec 1, 2017

You might be leaving too much material for the reamer. I wouldnt leave that much for aluminum but thats just me. You might try drilling closer to size and/or step reaming. If you could bore to within a thou for the first half inch or so this would help ensure that you are going in straight.

Guest · Dec 1, 2017

Bobw said:
I'd bet a 1/2" 1.25loc 4fl .03R Maritool HotMill that the hole is mostly fine on size,
but it isn't straight.

I agree, I could not imagine a reamer cutting that far under on material that is 28RC.

welder2022 · Dec 1, 2017

Revelstone said:
If you want a true sized hole. First drill then end mill bore .004 dia. undersize then ream with a carbide reamer. I guarantee a true sized hole within .0002 of the reamer size provided the reamer is indicated in within .0002 and the runout is also negotiable because the reamer will follow the hole.

This I could do if the hole was a half inch deep. But, per my post, it's 14". Mostly like a smoothbore rifle barrel.

welder2022 · Dec 1, 2017

allloutmx said:
You might be leaving too much material for the reamer. I wouldnt leave that much for aluminum but thats just me. You might try drilling closer to size and/or step reaming. If you could bore to within a thou for the first half inch or so this would help ensure that you are going in straight.

It's not aluminum it's 4135 steel, per my post.
The hole is there already, can't change that in hundreds of parts.
It's actually D.O.M. tubing and does have a bit of bow in it, like .014 max (random) in 14" length.

As an interim step, I can have the reamers I have ground with a step, so they would be .2870/.2933. Sound like a good split halfway?

If that doesn't work, I'm leaning towards going to a carbide step reamer, .2870/.2938.

jrmach · Dec 1, 2017

welder2022 said:
It's actually D.O.M. tubing and does have a bit of bow in it, like .014 max

Bingo,,,need to straighten before reaming

litlerob1 · Dec 1, 2017

jrmach said:
Bingo,,,need to straighten before reaming

Yeah DOM is not straight. And a reamer is going to follow the hole. If the hole needs to be pretty straight end to end, EDM may be your best bet.

R

jrmach · Dec 1, 2017

A reamer is not an EM in this life or another,however they can "fudge a little" .014 or .007 a side you are asking for trouble over such a length is a bit much with the tolerances specified,,,easy to see the problem

Bobw · Dec 1, 2017

47:1+ on depth... That's like shooting pool with a rope.

I'm going to guess the pins are a standard 2" long..
The pin is 3 tenths under the reamer size, so if the hole wanders
a tenth and a half in 2 inches, its not going... Thats .000075" of wander per inch,
with a reamer..... Hanging out half a mile.

I'm actually surprised that you are doing as well as you are.

litlerob1 · Dec 1, 2017

A thought as we haven't heard from the OP. He is passing parts off with rework using a flap wheel, so based on that the hole don't need to be too straight.

OP I would buy a Reamer that is the very top of your tolerance. Assuming the above is correct. Next time use a different technique.

R

I liked Bob's euphemism, I was going to say something about hookers in Southern NM.

jrmach · Dec 1, 2017

litlerob1 said:
I was going to say something about hookers in Southern NM.

please tell

Bobw · Dec 1, 2017

jrmach said:
please tell

I'd like to know too.

Reamed hole undersized

Plastic

Diamond

Diamond

Stainless

Stainless

Diamond

Titanium

Aluminum

Plastic

Titanium

Guest

Guest

Plastic

Plastic

Titanium

Diamond

Titanium

Diamond

Diamond

Titanium

Diamond

Similar threads