Reamer Help

I am new to the machining world and am searching for a little help about reamers. I will try to provide as much information as possible, but if I miss something I apologize. I am running a part on a Robodrill Vertical Mill, out of .188" Vespel SP1. I have 4 holes (that include the origin hole and "skew" hole for inspection) that are a weird size. The print calls out for 1.574mm +0/-.013. I am drilling first with a 1.55mm drill, followed by a .0615" Reamer. My problem is this. When the part is inspected with the 1.55mm holes position is +/- .002mm from nominal (tolerance is +/- .013mm), but after the reamer is ran, I am looking at numbers from 0.020 - 0.030 in both x and y.

My gut is telling me that I am either running the reamer too fast (or slow?) or feeding it as wrong. Currently the reamer is at 4000 RPM, and Feedrate is 1000 mmpm. The part is glued inside a pre-milled pocket in a block of aluminum, with all 4 holes relieved (the reamer does not touch the aluminum). I am not pecking the hole, as it is reaming a total of maybe 15 microns of material. Please help! I cannot get this reamer to run good to save my life!

Jwood1 said:

I am new to the machining world and am searching for a little help about reamers. I will try to provide as much information as possible, but if I miss something I apologize. I am running a part on a Robodrill Vertical Mill, out of .188" Vespel SP1.

Click to expand...

0.188" = 4.775mm

Jwood1 said:

I have 4 holes (that include the origin hole and "skew" hole for inspection) that are a weird size. The print calls out for 1.574mm +0/-.013. I am drilling first with a 1.55mm drill, followed by a .0615" Reamer.

Click to expand...

0.0615" = 1.562mm

Jwood1 said:

My problem is this. When the part is inspected with the 1.55mm holes position is +/- .002mm from nominal (tolerance is +/- .013mm), but after the reamer is ran, I am looking at numbers from 0.020 - 0.030 in both x and y.

My gut is telling me that I am either running the reamer too fast (or slow?) or feeding it as wrong. Currently the reamer is at 4000 RPM, and Feedrate is 1000 mmpm. The part is glued inside a pre-milled pocket in a block of aluminum, with all 4 holes relieved (the reamer does not touch the aluminum). I am not pecking the hole, as it is reaming a total of maybe 15 microns of material. Please help! I cannot get this reamer to run good to save my life!

Click to expand...

4000 rpm @ 0.156mm dia = 9.69 m/min = 58.8 ft/min

Sorry, the unit conversions were killing me while trying to digest this information.

How is the part being inspected? That's got to be one heck of a setup to be accurately measuring the deviation of 0.002mm prior to reaming. Temperature and humidity-controlled room with a CMM I assume?

Is the reamer sharp and new?

0.013mm is a heck of a tolerance on a plastic part. Any chance you can shoot the engineer who designed it?

Henry

EDIT: The more I think about this, the more I'm convinced that you're seeing an artifact of expansion either during machining or from handling after machining. The holes being off in both X and Y is the giveaway for me.

Try drilling the holes and then let the machine and part cool down for a few hours. Try reaming the holes after cooling and check the position. That would at least rule out the machining half of the equation.

Oh how I wish I could shoot the engineer, you dont even know! We are currently working on a predator drone to ship this part to them on!

We have a Nikon iNexiv VMA-2520 (video measuring machine) that I program to check the parts. It is accurate to something ridiculous (rated in the nanometers). The parts we are making are ran with an old reamer, a newish reamer and a brand new reamer, with similar results. Temperature is controlled to +/- .5°.

The tolerance is tight, and also has a TP of .025 (mm).

My gut tells me that I am running the reamer more like a drill, and not a reamer, but I am not finding much information out there regarding reamers feed/speeds

Another option is boring the hole. You can control location much better that way. That is if you have a good boring head. If not, then you would have to have a decent quantity of these to run to justify buying a good head.

Jwood1 said:

My gut tells me that I am running the reamer more like a drill, and not a reamer, but I am not finding much information out there regarding reamers feed/speeds

Click to expand...

The rule of thumb I've been told is half the speed, twice the feed.

Try the old reamer rule of thumb....
Ream at 1/2 the drills rpm and twice the drills feedrate

register said:

[
0.013mm is a heck of a tolerance on a plastic part. Any chance you can shoot the engineer who designed it?

Henry

EDIT: The more I think about this, the more I'm convinced that you're seeing an artifact of expansion either during machining or from handling after machining. The holes being off in both X and Y is the giveaway for me.

Try drilling the holes and then let the machine and part cool down for a few hours. Try reaming the holes after cooling and check the position. That would at least rule out the machining half of the equation.

Click to expand...

X2, on the heat factor and of course the Tol is ridiculous, however you are where you are,

Whats the ambient temp where the part is being machined?

Whats the temp of the machine fixture / vise etc.

Is the part temp being allowed to stabiliise between ops, being moved from say stores to shop etc etc.

You're in Texas ? - doesn't it get kinda warm down there.

You don't say how big the part is, - that can have a big effect.

Watch your clamping pressure / methods etc

tough one

J wood,

I have used that vespel to make some rod seals and it doesn't really ream very good. the reamer doesn't really cut it, just mooooshes it around and when the reamer comes out it is the same size as when you started. We measure with air flow. Boring it with a tiny sharp boring bar is the only way to precisely cut that stuff. We work with PEEK HPV and all those other fancy slick plastics too. Vespel is PRICEY to say the least!

Hope this helps,
Joey

oh yeah, shoot the engineer. With a marshmallow gun.

Ambient temp is 71°F, The "fixture" is a machined pocket with tooling hole bosses to align the part in a block (30"x24"x8") of aluminium clamped to the machine table. Part is ran dry, with an air hose blowing on the bit. The plaque of Vespel is stored in the shop, before machining, and everything done to the part is on site. I am in Texas, and it is 100+ degrees at nominal in the afternoon, but temperature inside and humidity are both controlled, and the part never leaves the shop until shipping (vaccuum sealed with dessicant, and then placed inside anti-moisture bags). This particular part is 40mm x 40mm.

I placed a part on a machine that wasnt ran yet today and that did not have the holes reamed, and they still were out of position. These 4 holes are aligned in a square 30 mm apart from each other, one at each corner of said imaginary square. The top right hole is my "zero" hole, bottom left is "skew". The bottom right hole is shifted 20 microns up in Y, and the top left hole is shifted 24 microns right in x. My gut told me that the part wasnt sitting flat at the time, but after machining a new pocket, milling both sdes and redoing it I got the same numbers. The thickness of the part at 10 points all around the part are within 6 microns, so I know it is sitting flat.

A reamer will not position a hole. A reamer is limber. If the drilled hole is on size and straiaght the reamer will follow it sizing the hole and making it round. If the hole is egg shape, mislocated or located on an inclined surface the reamer will follow the course of least resistance making a round but croked hole.

A standard reamer trick to ensure positive location is to bore the hole 1/2 dia deep to give the reamer a clean entry. I suggest you center drill the hole (just a peck.) Drill for stock removal. Pre-bore to locate the hole entrance, pre-ream with a carbide reamer to straighten the hole and size it for the finish reamer, and then bore for size and location followed by the one-size reamer.

Use a carbide reamer if the hole is deep and peck often to clear chips. A carbide reamer is 3X stiffer (honest) than an equivalent HSS reamer. You need that rigidity to straighen the hole should the rough drill have followed material inconsistancies.

Run the reamers about 20 FPM and feed slow, retract often. The object is to size and locate to very close tolerances so a 5 step operation is necessary. Slam bang production will have to take a back seat.

The shop I retired from used to drill, bore, pre-ream, and ream 3000 to 5000 3/8" holes in tube sheets with one finish reamer in copper nickel alloy. The size holding was +/- 0.0001" start to finish checking with an indicating bore gage.

Look at this site.... Special Reamers | Alvord-Polk
They make a "Jig Bore Reamer" carbide... and that's the tool I'd use.

Here;s another Co that does the same sorta tooling http://www.regalcuttingtools.com/reamers_descriptions2.html

My bet is thermal issues as well; that or maybe fixturing/clamping distortion. Does Vespel have issues with moisture absorption? That might also be a cause. Being out similar amounts after reaming in x and y is a pretty good indicator that something is going on related to one of those issues. Just because your shop is climate controlled doesn't mean that your workpiece and tooling are keeping cool while you are cutting. Air blast doesn't work all that well for keeping everything cool enough at that tolerance level (I also vote that you nerf the engineer). If you are getting consistent results that are just in the wrong position, just use the offsets that put you in the right spot.

Run the reamers about 20 FPM and feed slow, retract often.

Click to expand...

+1

I never ream anything faster than 20-25 sfpm. Much above that & it's easy to get chatter at the hole entry, when the reamer's leading edge touches the material.

I've reamed holes as small as 95% of finished size, and as large as 99.5% of final size. In soft materials like 6061 aluminum (and most plastics) the reamer seems to do the best job when the hole is somewhere around 98.5%-99.5% of reamer size.

I found the 99.5% size purely by experiment. I ream quite a few aluminum flashlight bodies (just after boring and just before honing). The reamer, run at 20-25 sfpm & cutting next to nothing, does a superb job. At 95% hole sizing the reamed finish was awfully rough.

YMMV

-----------------
Barry Milton