questions about using a reamer

8ntsane · Aug 17, 2005

Hello all

I have a job that I need a finished size of 5/8
hole. I have never used a reamer, but I need this hole as accurate as possible. This job will be done on my mill BTW. I need to know if I could drill the part to 9/16 and then use the reamer to
take it to the finished size? Or should it be closer to the final size before useing the reamer?

I could bore the hole slightly under if I had to.
Then use the reamer to finish it to 5/8
Like I said, this is something I have never done, so maybe these seem like stupid questions , but hey, when ya don,t no the proper deal its better to ask.

Though it would make life easyer if I could drill it to 9/16 as mentioned, then take it out to 5/8 with the reamer,,,,,,,,but I,m really unsure about this,,,,,Guys I need you to set me straight on this. I don,t need to screw up the parts trying to do this the wrong way.

The parts are spindles off a RX7 , and the tapered
holes where the tie rods normally go in, need to be 5/8 to use a rod ends. This is why I need the hole as accurate as poss. The 5/8 bolt needs to fit with out being sloppy.

These spindles are a small fortune, and cannot be obtained at any old junk yard, so a screw-up would be very costly.

Thanks Paul

precisionworks · Aug 17, 2005

5/8" = .625" = 40/64"

Even a 39/64 drill will leave .015 to ream (.0075 on the radius) which is a ton. You'll want to take off no more than .003 or .004 from the radius. So the hole needs to be around .618 before reaming.

Options? Depends on your budget. A spade drill could be used to get your hole close, they will usuall hold +/- .001. If you have a surface grinder you can grind the insert to cut this size.

An undersized twist drill + a boring head will also easily produce a .618 hole. Takes two setups instead of one with the spade drill.

Both will produce a bore that is ready to ream to final size.

------------------------------------------------

Cool race car!!! What are the ET's and trap speed?

WILLEO6709 · Aug 17, 2005

If you are seriously putting a straight hole in place of a tapered tie rod en in something going back on an automobile then you sir, are even crazier than I am.

Team FAST · Aug 17, 2005

Before you go reaming the hole to .625" you better check the diameter of the bolt you are planning on using!

The only accurate diameter bolts that I use are close tolerance GROUND finish aerospace bolts, such as an NAS 6200 series. They are typically .001 to .0015" under nominal.

8ntsane · Aug 17, 2005

precisionworks , do you think a 2-flute end mill that is slightly under,produceing a .620 size would be suiteable to use? If I drilled to 39/64,then useing the under size end mill to .620
and useing the reamer to final size? Does that sound more doable?

Didn,t realize that when using these reamers they could only remove a few thou.
The car is a 93 RX7 that I just tranplanted a L-S1
and T-56 6-speed trans. No track #s yet, but looking to see 10s . This install required the rack to be lowered, and the reason for this mod.
Drilling spindles for rod ends is a standard mod on race cars Willie, but like I said, I can,t just go get another set at the local bone yard if things go wrong.

Crazy? yep. Thats what they all said way back in the late 80s when I built a 2700lb door slammer and planed on running 6 sec @ over 200mph ,and I guess thats where the name 8ntsane come from.

Cheers Paul

Ralph_P · Aug 17, 2005

Drill with 39/64 and it will ream just fine. Low RPM for the reamer, about 80. Plenty of cutting oil.

precisionworks · Aug 17, 2005

Paul,

Geez, no wonder it's fast - a Corvette motor in a car made for 150HP!!! I imagine you'll see 10's.

The undersized end mill sounds workable. Four flutes tend to work better than two in harder materials. They can be grabby when used as an enlarging drill, so control the downfeed.

Barry Milton

Rex TX · Aug 17, 2005

A '93 RX7 is good for about 300 HP stock, more with mods - which all of them got, apparently.

toolmakerjim · Aug 17, 2005

drill it 9/16" then bore to .615 then ream use lots of sulphur base cutting oil...jim

deckelnut · Aug 17, 2005

9/16"...0.075" on radius taking a ton off....You'll want to take off no more than .003 or .004 from the radius. well that's a new one on me. 15 to 25 thou allowance on diameter for reamers between 3/8" - 1" diameter is about right. As a rule of thumb, use half drilling speed and twice the feed rate(a reamer is a cutting tool not a rubbing tool) taking too little a cut at to slow a feed and too high a speed will wear out the reamer lands in no time. for best accuracy drill to say 9/16" then bore to 0.600" then ream

toolsrul · Aug 17, 2005

No control with a reamer, you get what you get. If drill walks reamer will follow & possibly not clean up bad finish from drill & leave inaccurate hole. Best way is to bore to size - you control size, finish & breakout.
If you have to ream make sure reamer is indicated & trammed in. Good luck.

deckelnut · Aug 17, 2005

toolsrul. i'd agree with you that a reamer will folow a drill, so i'd recomend boring to 20 thou undersize, this way you can maintain position, by allowing the reamer to CUT and NOT RUB you will get a good finnish (assuming stock reamer and lubrication/flushing) for the best finishes you would use a "shefcut" type reamer, i've seen good results with "Brunswick" and "David Brown" type reamers also

matt_isserstedt · Aug 17, 2005

I'd buy a .002" undersized and a .001" undersized 5/8 reamer.

Then you can press fit the bolt in and avoid nasty problems with backlash and "looseness". Measure first, really want about .0005" of press, you can open it up if necessary with some sandpaper dressing. If the .002" U/S is too far under then go with the .001" U/S for future holes. You can also try chilling the rod end and mild heat ~300F on the other part to create more of a shrink and then the press won't want to gall nearly as bad.

Keep in mind the production rod ends *are* tapered as you probably already know...they wedge solidly in the hole for good all-around contact and are retained by a castle nut & cotter pin. Kinda like a nice MT with a drawbar!!!

Adding, use a lower spindle speed and a firm feed on the reamer with some cutting oil.

-Matt

deckelnut · Aug 17, 2005

for the best finishes you would use a "shefcut" type reamer, i've seen good results with "Brunswick" and "David Brown" type reamers also

sorry i should add that these reamers tend to be used in production not in jobbing shops

deckelnut · Aug 17, 2005

I'd buy a .002" undersized and a .001" undersized 5/8 reamer.

good point, but consider this

This is why I need the hole as accurate as poss. The 5/8 bolt needs to fit with out being sloppy.

</font><blockquote>quote:</font><hr /> Before you go reaming the hole to .625" you better check the diameter of the bolt you are planning on using!

</font>[/QUOTE]a reamer will produce to H7 and with a g6 shaft would give a close running fit but i suspect the bolt is not precision ground so your 0.002" U/S may just come in handy

precisionworks · Aug 18, 2005

Jim,

You like .615 and I like .618, so a good compromise might be .6165, more or less (say +/- .0015 and we are both EXACTLY right <LOL> )

Bored holes are almost always more straight, more circular, and more dimensionally correct that holes made with a twist drill. But - Murphy's law does apply to bored holes - using a too-small boring bar with too much extension (anything over 4X the smallest diameter of the bar) will generate a nicely tapered bore. Which is why THE REAMER was invented (IMO).

A carefully bored hole, with correct setup, will yield a hole approaching the surface finish and dimensional accuracy produced by a reamer.

But the reamer is lots faster, which is why it is always used in a production setting.

-------------------------------------------------

You probably don't want to know about the time I had my femur reamed...................sure hope the doctor knew what he was doing!

Tumbleweed Tim · Aug 18, 2005

These spindles are a small fortune, and cannot be obtained at any old junk yard, so a screw-up would be very costly.

Ream or just bore undersize and get it honed if you are concerned you may not get it right.

If you have the time and it's not a production thing then a barrel lap may work good for you on the last couple of tenths.

darryl · Aug 18, 2005

I'm going with the comment about checking the exact size of the bolt first. You probably have mic'd them and know the size for sure, but -

8ntsane · Aug 18, 2005

Thanks for all the replys guys.

The most important detail mentioned by Team Fast
was to measure the size of the bolts to be used.
This was a detail that saved me from opening the hole to .625 with the reamer. The bolts measured up .618 and with that finding I started to measure
other 5/8 bolts only to find that none of the ones I had in stock where .625 Most all come up .618

Ok, so a new plan had to be used. Since I didn,t have a under sized reamer, and I didn,t want to chance boring and possibly getting a tapered hole.
I ended up using a under sized 5/8 2-flute end mill. After first drilling the hole to 9/16, then using the end mill. It produced a smooth finish, and a very snug fit to the bolt. Just tight enough
they needed a lite tap in with a brass hammer to set the bolts in the hole.

All went well with the job, I,m happy with the fit. I didn,t get a chance to try out the reamer,
but as allways the information from everyone is valuable, and have learned a thing or three for the next time when I do have to use a reamer.
I think I will pick up a few different sizes and try them out on some scrap just to get the feel for the next time.

Thanks guys for all your input.
Cheers Paul

willbird · Aug 18, 2005

Something else to remember for stuff like that is they DO make expansion hand reamers, they can be adjusted to create a size you want, they usually offer a decent adj. range. The MSC catalog will give you a good feel for what is out there, but for just 2 holes as it sounds you needed I would just bore them to size as other posters said.

the .618 dia on the bolt is because most bolts the threads are rolled on not cut...and even when turning a part for a 5/8 thread I would be more inclined to shoot for .620 dia not .625 .

Machineries handbook has tolerences listed for major and minor dia. of threads.

Bill

questions about using a reamer

Aluminum

Diamond

Diamond

Aluminum

Aluminum

Stainless

Diamond

Titanium

Titanium

Cast Iron

Aluminum

Cast Iron

Diamond

Cast Iron

Cast Iron

Diamond

Stainless

Hot Rolled

Aluminum

Banned

Similar threads