I need a Good Reamer

[mewhg]

This might sound odd but I am trouble reaming a .1565" dia hole in 3/16" thick annealed 8620.

I just can't seem to get a good, on size consistent hole with a variety of reamers I have tried. I am looking for a hole that does not vary in diameter by more than +-0.00015"

Finally I found a reamer in my toolbox that just happened to be the right size. A carbide, 4 flute made by ProCarb in Fullerton, CA.

I got about 1000 parts from it before a part moved on the VMC tooling and the reamer broke.

This reamer gave me just on size, perfect holes.

ProCarb appears to be out of business.

Has anyone had particulary good luck with other brands of carbide reamers?

Regards,

 

[BillPSU]

You are asking an awful lot out of a reamer for that tolerance. One technique I have seen used is to get a reamer which is reaming slightly oversize and turning the spindle in reverse and using a flat diamond hone. Hone the OD or the reamer until it cuts the proper size. This means you will have to scrap some parts or some other test material.

 

[unclesyd]

Go in with a hone then lap it out.
Both companies are very good to work with.

http://www.engis.com/techsupport/bfcasestudies.html

http://www.helicallap.com/

My question is how are you going to measure the hole to your tolerances?

 

[jbel]

Considering that steel dowel pins are usually +-.0002, I don't think this is a lot to ask. There is nothing like the feeling of a correctly sized dowel hole in steel. Just tap it right in with a hammer and you get that smooth feeling.

I have had much sucess with Yankee reamers. Especially the 400 series. Check them out at

http://www.yankeereamer.com/

 

[Kenneth]

I would point out that those +/- 0.0002 O.D. dowel pins are centerless ground. IMO (shared by others in this thread), +/- 0.00015 from a hole (even a reamed one) is a lot to ask. With these kind of tolerances, taper (even for a relatively expensive honed or lapped hole), if nothing else, is always problematic. And as already pointed out, does mehwg even have the capability of verifying/measuring a hole to these tolerances?

 

[jbel]

Kenneth,

You are correct in pointing out the centerless ground nature of dowel pins. I have personally built many, many stamping dies with reamed dowel holes made with the forementioned reamers. I have consistently achieved a light press fit assembly between dowel and reamed hole. With the tight toleranced nature of the dowel pins used in the assembly, this could only be possible with the ability to maintain a tightly toleranced reamed hole.

Also, as BillPSU pointed out, it is possible to find a reamer that cuts slightly oversize and then hone the reamer until it cuts to the size you desire. It may take some upfront work to set up but once dialed in the would probably work well. As mewhg stated he was able to ream approximately 1000 holes with a single reamer and the catastrophic failure was due to other tooling issues. 8620 is reletively easy to machine so once the reamer is set up correctly, it should produce a lot of holes within this tolerance.

I agree with the fact that this hole may be difficult to measure. Some additional insight from mewhg would help.

 

[mewhg]

Gentlemen,

From my limited experience I have found some reamers to cut lously and others to consistently produce a hole that is consistently sized closer than +-0.0001 in tolerance.

I know that others have different opinions on a reamer's ability to do this but there are reamers that can do this, like my last one.

I could go from part to part with a set of Class X gage pins and it was amazing how consistent and on size the holes would be.

As I set this job up with the 1 man machine shop who is doing the work for me I tried various HSS jobber length reamers (the long ones). The holes varied by about 0.0005. Then I went and got a short carbide reamer from MA Ford. It would cut 0.0003" under its nominal size. A mystery. Ok, now I am starting to believe my machinist who tells me I'll never get reamers to do what I am asking. Then I find this Procarb reamer that I think I bought at a flea market for a buck. Bam, on-size nice holes.

One option for doing close tolerance holes like this is using a diamond hole with an expanding mandrel. They work but they also wear over time and you have to keep fooling with the adjustment. After several hundred holes the adjustment stablizes (I guess as the high diamonds wear down) but you still need to keep a close eye.

I think what I will do is try different short carbide reamers from different mfgs. Maybe Ill find another good one.

thanks for all the replys

 

[ajack1]

There are many factors in achieving what you desire. Firstly as you say longer reamers are less predictable than shorter ones, hardly rocket science, the shorter anything is, the more stable.

Secondly the amount of material you leave in to ream will affect results; basically the less you leave in the more predicable the result.

Thirdly reamers come in different grades, just like slip gauges they are all accurate, but some more so than others, why not get a rep in from a reputable company?

Fourthly what lubrication you use is important, soluble oil based coolant cuts tighter than cutting compounds and with the more “greasy” type quantity matters as well with the limits you are trying for.

To sum up what you are after should be easily achievable IMO, but only in controlled conditions and I would look at changing the reamer way before 1000 parts.

 

[RRBD]

The accuracy of a reamed hole lies mostly in the operations leading to it, if you are just stabbing a drill in these parts and then reaming the hole, I can see the trouble. I usually, drill, plunge with an endmill and then ream if possible.An endmill will make the hole round, on location. A drill makes a triangle shaped hole within a reasonable proximity to location, see the problem(s) You are asking alot from a reamer. I would consider plunging with an endmill that is very close to finished size and then running a ball broach thru the hole to size it. You'll be happier with the results.

Scott

 

[mewhg]

Scott,

After drilling you plunge with an centercutting endmill? then ream? I will have to try that.

What is a 'ball broach'? A google search comes up with a tool for doing valve guide repair.

thanks

 

[jbel]

mewhg,

Refering to RRBD's posting, a centercutting EM should not be necessary as the predrilled hole would not require the end mill to remove material from the center. I believe the rest of the post has many good suggestions.

 

[MEMO4EVER]

the best one is adjustables reamers .

 

[ajack1]

Can anyone actually hold 0.00015” with an adjustable reamer? If so I would like to know how I have never been able too.

 

[jbel]

mewhg,

The following link to Yankee Reamer's technical page gives a wealth of information. They state to tightest tolerance you can hold is 0.0005 total or +-0.00025. They also give great information about pre-ream hole sizes for different materials.

http://www.yankeereamer.com/Tech_Info/tech_info.html