Tolerance...

Some keywords for more contributions:

• Interference fit
• Tight fit
• Snug fit
• Sliding fit
• Rattly-good fit
• Pi$$-fit

etc.

You've left out my fav'rite Brittish class of fit (from reading early engineering literature): "Sucking Fit" = very tight free fit

Oops!

let's say the shaft will be 1/2 bar stock, if this is standard and you want a hole bored to accept it you could specify 1/2" + X / - 0 this assumes the stock is dead to size, you don't want the hole bored undersize (-0) and if you are not sure you can use PW's descriptors instead of a dimension for X.

If you have a bearing and want a shaft for it the reverse is true (+0 / - X)

I hope this helps, I picked it up at my last place, I have a lathe and a mill and would describe myself as a hobbyist.

You could use decimal numbers for your measurements, and remove any ambiguity.

Thusly: the hole = 0.500 +/- .001

the shaft = 0.495 +/- .001

that would give you a clearance of .005 +/- .002

Worse case you would have a hole 0.501 and a shaft 0.494 for a clearance of .007, still a fairly tight fit allowing for rotation/sliding (be sure to use a lube).

You get the idea.

And a good answer for you. Anytime somebody does a one-off project, just put a note on the sketch saying "clearance for 1/4-20 screw" or "loose fit for part b", etc. Machinists are smart about this stuff and can do what you want easily and inexpensively.

BRAVISSIMO!! The "shop-rats" usually have a better 'feel' for fits & the like than office engineers w/ less than ~ 5yr of experience. Tell 'em what you need (real world) & you'll might just discover a very useful resource.

Ken makes a really good point. I worked at a shop where there was a "cost control engineer" who kept changing dimensions to two places to "save money". The machine shop kept complaining that their sloppiest mill had a four place readout and was good to 0.0005" without any extra work. They wanted three places on everything except the really tight stuff. And this was a non-CNC shop.

While the rhetoric that is going on is good, I think that maybe Vermin is asking a basic question that I still don't see the answers for, or maybe its just my questions on the subject.

What is a good tolerance to put on each piece (the block with the hole and the shaft in order to get a fit that will prevent leakage of (ge: a liquid, ) while not being too tight to assemble the piece without undue exertion.

Perhaps the answers don't lie with just telling the machinist to do it. He/she has to have some personal rule of thumb or idea of the necessary tolerances. What are they, or is it a trial and error solution?

After all, fluid leakage between pieces will be governed by the properties of the fluid (like fluid density and viscosity) as well as the pressure difference across the parts. And the ability to assemble the parts will be a function of the thermal expansion properties of the materials of construction of the individual parts as well as the temperatures at which they are put together.

There was no mention of fluids in the question?? I think it was just a very general enquiry as to how we arrive at a particular tolerance.

In general, a press fit for a nominal 1/2" shaft would run from about .0005 to .0010 interference. (The interferences usually quoted actually vary a bit from that.)

Beyond that, though, one needs to either open up Machinery's Handbook, or simply trust the machinist to get the right fit.

In a typical scenario, one piece has already been machined (or comes out of an extruder, etc, with a particular dimension). So in that case, if this is a one-off job, it is almost essential that the person doing the machining have the part in hand, because you want to use the same measuring tools for both parts, have the parts at the same temp, etc. Vermin would not want to tell the machinist to make both parts precisely some dimension, because chances are very good that one precise hole will be enough, and that the piece of stock, whether .498 or .502 or .506 is round enough. The machinist just measures the stock, and makes a hole a little smaller. If he had to size both, it would be twice the cost.

Ordinary 1/2" bar stock from Home Depot is surprisingly precise, but not precise enough for repeatable press fits into a rigid material. At least it is generally quite round, however, so machining a correctly size hole is pretty straightforward, even without touching up the shaft to make it rounder.

I recently press fit some ball joints into holes I machined, and the ball joints (actually made, not just branded, in Germany) were quite far out of round (at least .005, if I recall). So for these, a .0015 interference would have been ideal. But if I made the hole .0015 less than the small "diameter" then the large diameter of the piece would prevent a press fit: it would be more like broaching. I fussed around with the pieces and managed to get them pressed together, but I used bearing mount as a backup: hardly good practice, but for the intended purpose it would work fine.

In production, with 1/2 inch rod, to get a reliable and repeatable press fits, the machinist might have to first make the bar round, and then make the matching hole .001 smaller. You might want a shoulder on the shaft anyway, so you could simply machine the stock to .450 and size the whole appropriately for your process precision. These days, it would be easy to get the interference between .0005 and .0010 consistently.

Machinists will often have rules of thumb for various fits, given various diameters, but even so, the handbook gets opened up a lot, depending on how broad the experience of the machinist.

STL brings up a lot of good points also re the other issues beyond the simple diameters. There is a lot that a machinist will do without having to think about it much, that you would otherwise have to specify, if you were simply handing the pieces to a robot. (Ohh... you wanted the hole perpendicular too!!??)

Many machinists have a good sense for mechanics, too. For example, if the piece of bar stock is long, many machinists might question how the pieces will be pressed together, because the bar may buckle before transmitting enough force to stretch the hole to fit. All this stuff can be calculated, but a good machinist can get stuff done easily and quickly without having drawings that spell out all the details.

In general, unless you want to be darn sure that two pieces cannot come apart, you avoid shrink fits partly because they are hard to work with (what if there is a little bind as the part goes in, and the cold piece gets hot?). It's fairly easy to tell, even in a press without instrumentation, how heavy a press fit is. For many uses, a press fit is far stronger than it needs to be to resist pullout. So usually, an ordinary press fit works well -- but of course there are exceptions. For steel bearings in aluminum housings, heating the aluminum at installation can help insure that there is still an interference in operation, even after the item has reached operating temp (as in an engine.)

I realize, after writing this novel, that Vermin doesn't want a press fit. I read your "without undo exertion" as meaning something you could do with a press. I think he is thinking of something he could do my hand.

Oh, well... the principals are the same: hand it to the machinist, and say make it fit.

I've stated this before. If that's all he wants to do, then all he has to do is use a reamer on the hole after he drills it and the rod will slide in and out by hand and not have any play.

True. I'm not sure what got me off on the press fit tangent. Probably early signs of senility.

interference fit is also called a 'force fit', items are made to the same size and slight variances make them bind.

There are also ways to create interference oversized fits, where you have to chill the center or heat the outer member to allow for an interference fits. freezing shrinks it and you fit it and let it warm, and vice versa for heat expanded.Once they reach the same temperature they can have an almost welded fit. A lot of gun barrels are made this way(or they were in WW2). You can also apply a surface texture to heat/cooling mediated interference fits. This adds to the friction of the system when cooled..

This is one of principles of fits systems.

Unfortunately you have to be careful here in the States in mixing in ISO or metric standards as most machinest are used to dealing with tolerances and 3 place decimal numbers. If the supervisor hasn't spent the time to look it up and explain it to the machinest there is a very good chance that it will be done incorrect if the machinest has to look up that information. Although they teach this in apprenticeship training most "older" prints state it in decimal form and that is what the machinest are used to working with. I think as more and more time goes by they will get unboard with this type of tolerance on the prints!

Yes, yes and no. The standard of decimal places to use in measurement actually is limited only by the measurement devices and the individuals ability to use them.

There used to be a table of ID and OD sizes and tolerances for all types of fit from slide fit to shrink fit published by Newall or Newell. Not sure if it is still available. I think it was called the 'Newell table of limits'.

KennyT

Thanks for that info. It will help me greatly with a project I am developing.

Salutations vermin,

Tolerance is the value of +/-, ie +/- .002" = .004"

If you want a nice fit of shaft to block you ask for .003"-.005" clearance, the difference of the shaft OD and the block ID. That is if the block is less than 3.500" thick where the shaft were to pass through. Now why is that important you say; because in thick or deep bores having less than .005 clearance you'll need lubricant which will take up space causing a tough push/pull action to manipulate by hand. Or if the least small speck of crud or piece of fresh air were to accompany your shaft well it's a deep subject dude and may require a press to extract.

A must have for these type details is "Machinist's Handbook" published by Mcgraw-Hill in 1955, look for 1980-81 edition.

Good blog, I learnt (re-learnt!) some good points here, many thanks to all concerned.

With regards to a fit, tight fit, where is the old trick of heating the "hole" and cooling the "pin" to allow easy fit, but when cooled, holds almost like a weld? or till you weld....

where is the old trick of heating the "hole" and cooling the "pin" to allow easy fit, but when cooled, holds almost like a weld?

..........and then the components are pressed together on an hydraulic press

............then you do have an interference fit

Hi,

For this purpose, we use tolerances on mating parts based on the reference dimension (1/2" in your case). Please check out the following document:

http://www.me.metu.edu.tr/me114/tolerancing.htm

For your case, H7/h6 may be appropriate (see the page)...

I hope this helps you.

Regards,

Sezgin.

Just to add to what the others have said, there are standard charts for the fits between holes & shafts ie. BS 4500 but, as mentioned before, this has to be tempered with a bit of experience. It is very easy to rely entirely on the standard charts but you might then over specify the components which inevitably results in increased cost.

It is perfectly reasonable to just ask the machine shop for a 'sliding fit' or whatever between 2 parts but you must accept that your idea of a sliding fit may not be that same as the machinists.

Of course, life gets a whole lot more complicated when you have say, a part with 2 pins which have to slide into another part with 2 holes & you get involved with positional tolerances on the features as well.

the first question i have is, is there a concentricity issue between the two parts, if one part is driving the other then one must ask how good the concentricity must be, if it is an issue then likely both parts need to be machined and then how close must they be, if it is not important re: concentricity you may be able to go with stock bar size and a not so important bore fit then simply use the 'side-lock' approach (threaded hole thru the side of the bored shaft, using a set-screw to lock into the shaft) note: the shaft would require a flat for the set-screw to lock against. this would give you one part locked into the other without overtolerancing any of it thus keeping your cost down.

I'm not sure that using a set screw in this case is going to keep the cost down. The expense of rigging a jig to hold your part on its side, and then the numerous tool changes, i.e cutting a flat spot, drilling a dimple to keep your drill bit from drifting, the drilling itself, running the tap thru without breaking it, the numerous measurements, the cooling/lube fluid, the chamfering of the finished hole, the cost of the setscrew .... no, this would neither be a time saver nor a cost saver. And in the end, there is no type of seal here, if that was the intent. And in many cases, not one, but two setscrews are needed, separated by about 60 degrees around the center.

And then repeating the whole jigging process on the shaft in order to machine your flat spots!

Being able to make these decisions is the realm of the experienced mechanical designer, process engineer or shop foreman. It all depends what you're trying to accomplish.

Well put. Simply machining a good press fit in the first place would save a tremendous amount of work, and would result in an assembly in which you don't need to worry about the setscrew loosening.

Vermin, this is a classic question that would best be answered by browsing through The Machinery's Handbook. This reference book has been the bible (insert any religious affiliation's book here) of anyone working with metal assemblies. It's generally written in understandable English that you don't need a scholastic degree to figure out.

The section on tolerances and fits clearly explains the answer to your question. And although, as was already mentioned above, most machinists know the science of fits like they know their own name, the key to this is not necessarily knowing all the tolerances of shafts and holes ... but instead knowing exactly which reference materials to read to find the exact answer.

Despite the name of the book (which is often mistakenly called The Machinist's Handbook), you don't need to be a machinist to benefit from owning this book. The amount of useful information in this book has made life easier for at least a couple generations of those working with metal. And since it is updated quite frequently ( I believe it is on the 30th Edition now?) the info remains current. I highly recommend it to anyone. Well perhaps not ANYone ... I don't suppose the nuns in my childhood catholic school would have much use for it ... but you get my drift.

Machinery's is a great book but my 26th edition runs to over 2600 pages. If you can find a CD version it's a bit more manageable, the hyperlinks in the index & other pages are well considered.

The number of pages can seem daunting, but the index seems to handle that pretty well. The only problem with the CD version is that you can't throw it open on your shop table next to your mill and page thru it with your grubby fingers! I prefer keeping it primitive, with paper and ink.

Amen, brother. I bought the CD a couple editions back, then went out and bought the book and shelved the CD.

I know what you mean, I still leaf through the book as well but it's useful to be able to print a page as you need it or paste a paragraph of text into an instruction for the machine shop.

The 28th Edition comes out in February. I have mine on order through Barnes & Noble, only because my B&N membership gives me 10% discount on everything, plus I received a 25% off coupon after renewing my membership, which I applied.

My 22nd Edition was purchased in 1984, so I am due for an update! Not that older editions aren't still usable, but in my current job I decided that an update was in order, and then there was that coupon! Plus, I want to make my co-worker jealous, as she still uses her ratty old 20th edition from 1978!

I like the Toolbox version as well, because it is smaller and lighter (and cheaper) the the large size. I have a magnifier if I really have trouble with some of the fine print, or I just photocopy the page I am working with and enlarge it! It would be nice to have the CD, but I decided I could not afford both. Besides, it looks good sitting on my desk. Every REAL engineer must have one! <grin>

"Besides, it looks good sitting on my desk. Every REAL engineer must have one! <grin>"

So true! It's funny, this book can tell quite a bit about you. If you see someone in possession of an Edition # in the teens, you have to look at them in a new light. Something akin to legendary. But the rule is ... if you update an old edition with a newer one, you must keep the older one in plain site on your shelf. Lest anyone should make the assumption that you are a wet behind the ears newbie. If only the newest version is visible in a person's workspace, I feel an inclination to take them under my wing.

I still have my 24th Edition and haven't updated. It would be an emotional experience. I have always had a slight grudge with the publishers though. Edition 24 does not have the thumb index cutouts on the edges of the pages, whereas both earlier and later editions do have them.

'24th'!!! Damn youngsters, my printed copy is an 18th edition bought when I was at college.

18th??!! In awe, I bow to your grizzled experience.

Yes, my 24th Edition. Didn't get mine till after I spent a bit of time in the military. We had different books in uniform.

I do that with Marks. I keep the 3rd edition in view, but have the 9th edition handy if I need it. Freaks people out for me to pull out the old book.

Twice he cut and still too short (:

I second that motion. This is an EXCELLENT reference for Mechanical and Manufacturing Engineering, and SHOULD be on their book shelf. The 28th Edition is being released this month. It can be purchased on CD too, which probably enables quicker searches.

Vermin,

This handbook has ~45 pages covering the "Allowances and Tolerances for Fits," including definitions and tables. If you have a machine shop at your location, one of the machinists is bound to have the handbook. Go and copy the section you need for further reference.

You must create a tolerance that results in the type of fit you want - it sounds like you need a slight force fit. When you specify your parts you will place allowable tolerances on each piece and the machinist will have to meet those tolerances.

Try the

Dimensioning and Tolerancing Handbook
By: Drake, P., Jr. © 1999 McGraw-Hill

Garyceng, excellent commentary concerning the proper application of tolerances!

Regards,

Ing. Robert Forbys

Not only that but I found with dealings with my own machinest in house that even though it would be understood or even implied depending on the machinest "mood" if it is not spelled out on the print you can bet it will not be what you want or need! it will either not be correct or so correct the guy will spend 2 days lapping in something that could have been a cast or rough finish and will blow the entire budget in just one piece!

It's been my experience that machine shops don't leave things to chance. If the information is vague they will call and get more information. The goal is to get it done quickly, to spend as little time as possible and do it correctly the first time. Anytime there is opportunity to guess on the part, they will call.

If the part is produce at the site you work it all depends on the quality of the machinist. All too often there is no QC department to check their work.

Even is the part is produced offsite with no QC department to check the incoming part no problem will be detected until the assembly people say it doesn't fit or worse when the customer calls up and says the machine is broken or doesn't work properly.

But my reflections are based on companies with less than 50 people with limited resources. But that is much of reality.

Press

Transition

Sliding

Free

The above terms describe the fit bewteen two mating parts. Any machine shop should be able to produce the parts from the nominal size required and the use of one of the above terms.

Fitting a 1/2" shaft through a 1/2" hole isn't that much of a challenge and can be accomplished easy enough using standard tolerances.

Basically just using a standard drill bit and reaming it with a 1/2" reamer is enough to meet that requirement since 1/2" rod is a standard diameter from a manufacturer.

When you're getting into things like machining shaft to fit bearings or or sprockets, or to fit a machined part into an already existing space then you have to specify an exact tolerance.

Machine shops have a set of specific tolerances that they use as a rule of thumb, as soon as you start specifying tighter requirements for tolerance the price will go up.

A shop that is CNC and uses laser cutting methods can hold tighter tolerances then a shop that uses Fred and Barney technology.

When you specify a dimension using fractions the standard tolerance is +/- 1/16" if not specified.

When using decimal form there are several standards depending how many places past the decimal you indicate:

.x is +/- 0.03"

.xx is +/- 0.015"

.xxx is +/- 0.01"

If you're calling out a shaft diameter to fit into a bearing you will want to specify +0/-0.005" you certainly don't want the shaft to be bigger then the inside diameter of the bore of the bearing.

When dealing with forming parts the tolerance for bends is +/- 1/2 degree.

It's also important to specify which dimensions are critical so that time and money isn't wasted on every dimension given. Such as the length of a keyway on the shaft is not important.

"A shop that is CNC and uses laser cutting methods can hold tighter tolerances then a shop that uses Fred and Barney technology."

That could start an argument.

I know that CNC machining gives better repeatability but, if you need parts that fit together precisely and you need an exact match to another part, CNC is not flexible enough. For example, we weld electrical feedthroughs into vacuum flanges & must have a leak tight weld. I can size the hole to be a good fit on the feedthrough knowing its tolerance range but, having the largest toleranced hole with the smallest toleranced feedthrough would give too much clearance for a good weld. Instead we give the machine shop the feedthroughs & ask them to make the holes to suit. You don't get that flexibility with CNC.

I agree with you. I know that none of the statements made really apply to every application.

I deal with the outsourcing for manufactured parts in my company. Out machine shop is Fred and Barney technology. Our press breaks are 40 years old. We cut with a plasma free handed.

When I farm things out those are the standard tolerances for the parts that we use.

We do use large quantities of machined parts that we require precision and they are made using CNC lathes.

We do get somethings that are made by injection molding as well.

Our press breaks are 40 years old.

Press brake, not break. Some may think I am nit-picking on a typo, but I have seen this mistake all too often. People even speak of "breaking the part" to a certain angle, and refer to the past tense or finished condition as "broken", when the correct terms are "bending the part" or "bent". Nothing has been "broken" in the proper operation of a press brake!

Sorry, just a pet peeve after over 20 years around metal production shops and tool shops.

Please give me a brake.

That Press Brake, breaks all the time, so much so that now I'm confused as to which term applies.

Actually, no excuse, please forgive me for not proof reading my posts. I appreciate your bringing it to my attention. I'll try to pay more attention to that.

The reason that it's called a press "brake" is because of its similarity to an old medieval torture device called a brake that worked along the same principal.

Although I'd have to say that they couldn't achieve the same pneumatic pressures back then. The prisoner/bellows combination had a somewhat lower limit to the psi they could reach. Rarely were they able to get the needle into the red zone on the gauge. So they used the more reliable "volume of the screaming prisoner" to measure pressure.

Nothing like the human scream to bring things into perspective.

Thank you for that. I like medieval history. I like history in general and I appreciate the your input.

No problem. I am not complaining about a typo, but about people who think that "break" and "broken" are the correct terms used with this equipment!

I guess you could say "brake" and "braked", but it is just as easy, and more understandable to say "bend" and "bent", after all, the usual operation done on a Press Brake is called an "air bend", not an "air brake"! <grin>

One of the problems is that we don't see our errors right after we've typed them.

On these forums we only have a few minutes to catch those errors and correct them.

After that few minutes to make any changes are up, you're stuck with it.

I just noticed in another one of my posts I put the word "OUT" instead of "OUR" and am now stuck with looking illiterate for the rest of my life.

I use Firefox and every word that is spelled wrong (spelt wrong!) is underlined in red.

It does use US spelling, but who cares. Then I use the Spell checker from CR4 to help me! Naturally it won't notice the out for our, but it does a good job otherwise!!

Actually Jan ... you typed OUT instead of OUR on two occassions. That pesky T is right next to the R on the qwerty Easy to transpose.

Sotty, I didn'r mean ro nirpick yout spelling

Totally agree with what you wrote, except for one minor point:

.x is +/- 0.03"

.xx is +/- 0.015"

.xxx is +/- 0.01"

You mention these tolerances as "standard". It's been my experience that there is no universally accepted standard on what tolerances various numbers of decimal points equates to. If it is not specified in the drawing's title block (what ".xx" equals, for instance), then no assumptions can be made. The creators of the drawing should be contacted to find out what their particular tolerancing specs are.

Agreed, these are not a 'standard', the relevance of the number of decimal places should be stated on the drawing, usually somewhere in the title block.

I apologize for stating that the way I did.

Those are standards that we use and they are printed on every drawing we use so they are out standards.

I was in error for making it sound like they are standards throughout the engineering community.

You wrote: .xxx is +/- 0.01"

Did you mean this? I have never in my life seen a tolerance that large on a dimension spec'd to three places.

It is certainly possible, if their work does not require close tolerances. We do semi-precision work on many of our parts and our standard block tolerances are as follows:

.X = +/- .05

.XX = +/- .02

.XXX = +/- .005

Note that this last is only half of the .01 called out by Janissaries.

On the other hand, I have worked for companies which used +/- .002 or even .001 for three place decimals.

And of course, having more open block tolerances does not preclude a designer from setting any individual tolerance to a tighter one.

Yes that is what I meant. I took those tolerances directly form our drawings that we have specified as standard tolerances.

But usually when we specify .xxx that pretty much means we want less than 1/64" tolerance.

When the occasion calls for tighter tolerances I will specify that in writing on my quote requests. My vendors know that what I state on the quote request takes precedence over the tolerances shown on the drawings because the engineers will only change the picture and not the information. Then from experiences with the part itself not working and always having to be reworked I will specify stricter tolerances in the critical areas.

This is a general question so you realize there is no simple answer to a complicated issue.

R&D of various machinery was my job description a while ago.

Professional machinists if asked for an appropriate fit would in turn ask you what application, materials involved etc..

Then having discernment the MM (master machinist) would consult the machinist bible to ascertain degree of finish required for application or due experience of detail proceed.

Hope am helpful

yOU ARE CORRECT A1/2" BOLT WILL NOT GO IN A 1/2" HOLE . I WIGGLE THE DRILL IN THE HOLE UNTIL THE BOLT FITS, A safe bet is drill the holes 1/64 larger than most holes.

"I wiggle the bit in the hole until the bolt fits"......!!!!!!!!

I thought this was an engineer's forum, an engineer uses the correct size of drill for the job and shouldn't need to resort to "wiggling the drill"

John.

"wiggle the bit..."

hehehe

That is inadvisable ... on sooo many levels ...

But, to be the devil's advocate... it really does depend on the application. I could think of a scenario or two where wiggling the bit might be the best overall solution. But as a rule of thumb??? Uhhh ... no. Definitely ... no.

Sounds like he has a limited number of sizes in his drill set. Either that or a limited amount of brain-power and common sense!

Yes, wiggling the drip is an unsupervised mechanics method.

1/4" bolt use 9/32" drill

5/16" bolt use 11/32" drill

3/8" bolt use 13/32" drill

1/2" bolt use 17/32" drill

5/8" bolt use 11/16" drill

3/4" bolt use 13/16" drill

When bolting several pieces together that have been drilled independently you might have to use a larger hole to ensure getting a bolt through.

Sometimes you might want to go with using slots instead of holes and make sure that the slots on one piece run perpendicular to the slots on the other piece. This will allow adjustments before tightening the bolts.

Drip = Drill

I'm batting a 1000 on spelling today.

That is a great way to get your hand shredded in a drill press.

I hope you meant us to laugh, well I did anyway..... If you did not, God help you!!!

Please invest in a copy of "Machinery's Handbook". It'll answer most if not all machining question you'll have. You don't need to be engineer to use it and engineers do use it for reference. Like other said its matter of determining the "fit" you want. It also a matter of normal tolerance. Fraction like 1/2" has normal tolerance of +/- 1/32 to +/- 1/16. So you see why it'll never fit. It always good idea to let machine shop know what you intend to do. Tell them make shaft and block so shaft slide inside block.

DANG IT! I should have thought to suggest that! It's so obvious!

Invest in a "Machinery's Handbook" and reference the "Standard Fits Section". Your question is simple but rather complicated in exicution. - Al

All good points, mostly. The only thing left out of this discussion is that there is more to making parts fit, and work together properly, than merely size and tolerance on diameters.

For critical assemblies like slip fits, other factors include: straightness of the shaft, roundness (or circularity) of the hole and shaft at specific points, cylindricity (roundness extended over a specified length) and runout (variation from center when part is rotated), and concentricity (centers of diameters at various points falling on same axis line). In the US we call this Geometric Dimensioning and Tolerancing and is covered by ANSI / ASME Y14.5M-1994

In addition, surface finish (measured as Roughness) will play a part because it affects friction where the two parts meet and therefore can cause premature wear-out of moving parts and also create heat which could distort the shape. Either one of these could cause either seizure of moving parts or excess vibration.

Heat distortion is a special concern when dissimilar materials are mated, because they will have different expansion co-efficients. Wall thickness and part geometry can also play a part. For example, due to their geometry, and since aluminum expands more than iron or steel, aluminum car pistons must actually be machined out-of-round (quasi-elliptical) and smaller, so that when the engine comes up to temperature the pistons will be a good slip fit in the round bore of cast iron blocks or sleeves (in aluminum blocks).

Hello,

My understanding of hole/shaft tolerence is simply this:

LOOSE FIT : .0025* 3rd. root(dia.)

FREE FIT: .0013 * 3rd. root(Dia.)

SNUG FIT: .0009 * 3RD. root(Dia.)

Using these formulas takes away any guesswork , follows standard machinist standards and guarantees a predictable fit.

Regards,

John

You can drill the hole to the exact same size of the shaft.

You can bevel the end of the shaft and force it in with a press.

if it is too tight you can chill both pieces to cause them to shrink then fit them together. They won't slip after expanding back to room temperature.

Although all the discussion here has produced a plethora of suggestion, formulas and methods; and fits of all sorts have been discussed, achieved by presses, hammers, heating, setscrews, etc. (and they are all valid bits of information) ... I took another look at Vermin's original question.

The crux of it is:

"...create a shaft that will fit snugly into the 1/2" hole - not too snug, but with no wiggle room... rule of thumb..."

Okay, I will attempt to answer the original intent of his question. No more. No less. How does this sound? The answer to your question is:

As a rule of thumb .002" to .004" difference between your shaft and your hole will in most cases give you a mating that will be "not too snug, but with no wiggle room".

Obviously this will not cover 100% of situations, but based on the specifics of all that you wrote in your original question, I believe this is the bottom line simple answer you were looking for. Does anyone disagree?

Gosh, we sure can complicate things on here!

Do I get a green thumbs up for that??

Tell machinist you want it to fit snug, not to tight/loose but no wiggle. If he asks for a tolerance, that's you're sign find someone else.