machinist question, threw hole tolerances for pin/part fit?
 

ok ive got a .480" pin.
i need it to gravity drop into a hole(in .110" thick plate). no pressing or pushing required. with minimal slop/play but not critical. but the hole/plate will be anodized. what size to i need to model the hole?:oops:

Re: machinist question, threw hole tolerances for pin/part fit?
 

I would talk to your plater and see what they would estimate the thickness of their anodizing to be. It can vary a lot depending on the type of coating (regular vs hard anodize) as well as their process. They should be able to give you a good idea on what to expect.

The problem you are going to run in to is the thin plate, being roughly 1/4 of the diameter of the pin means that any slop is going to feel like a lot.

I would say that somewhere around .004" of tolerance between the parts would be about right assuming that the thickness (per side) of anodizing does not exceed .0005". You could probably go tighter if you know that your process will result in a perfectly round hole such as a reamer vs. interpolating the hole with an end mill.

Re: machinist question, threw hole tolerances for pin/part fit?
 

I would try .485. It will drop in, and anodizing isnt thick at all. Our powdercoater generally only manages to buildup .005 to .010 depending on size of hole (just for example, anodizing should be much thinner).

If it turns out not to be a gravity fit, some rolled up sandpaper should knock off the anodizing and get you close to a nice fit. Much easier to remove material than add it.

EDIT: SMR beat me, and makes a good point about the thin plate to thick pin, especially if youre only passing through one plate and not two that are spaced apart.

Re: machinist question, threw hole tolerances for pin/part fit?
 

I would consider the tolerance of the pin, which should be .480+/-.00x inches. The hole should also factor in a tolerance to make sure there's no interference. It should be the largest potential diameter of the pin plus a couple thousandths and with a tolerance of +.00x/-.000 to ensure it won't be any smaller than your desired measurement. I'm thinking a max pin size to minimum hole diameter should have a difference of .003"-.005"? You can certainly open it up more if tolerances can be held tight enough and/or a precise fit isn't critical.

Also, I'm not sure, but I think anodizing adds ~.001 or maybe .0001 of thickness. Is the hole punched before anodizing? I assume so.

Sorry, I guess this really isn't all that much help! :ror:

Re: machinist question, threw hole tolerances for pin/part fit?
 

anodize usually has very little build up because of the requirement that parts be etched ahead of time. The etch is typically done to the estimated oxidize growth.. .005" oversize will be sloppy, more like .0015" would allow a slip fit

Re: machinist question, threw hole tolerances for pin/part fit?
 

Good point about the etch forgot about that. I believe that our plater told us to figure in .0005" per side at one point.

I would just fit the pin in the machine until it drops through like you want it and then comp it out .0005" per side for safety. Of course this all depends on what you are actually doing, if you are just making one fit it before you pull it out...If you are drawing a print that you are sending out you are likely going to have to sacrifice a little on fit unless you want to pay for the tight tolerance.


Tolerances are a PITA when people dont size them correctly, happened to me all the time at my old job. They would spec a hole at .498" ±.002" and the mating boss to .500" ±.002" an then blame us when the boss ran high and the hole ran low and the two wouldnt fit together...Their solution was to give us some bogus +.001" -.000" BS when they didnt need that fit anyways! Glad I dont have to deal with that anymore.

Re: machinist question, threw hole tolerances for pin/part fit?
 

I usually go for .005 for a slip fit that isn't critical. When the parts need to mate really tight without interference then 0.002 is about as tight as I like to spec, but it really depends on the process as SMR stated. Reamed holes are much easier to tolerance vs other methods, and the roundness of the bar and plate hole play a big part in it too.

What I would do is 0.480" -0.002 +0.000 for the bar D and 0.482 +0.001 -0.000 for the plate hole D. Gets the parts between 2 and 5 thou clearance. If you already know tolerance of the bar then design the plate hole around it to guarantee the slip fit (assuming your machinist isn't daft).

Re: machinist question, threw hole tolerances for pin/part fit?
 

The tolerance for a gravity slip with only .110 thickness to make friction. Damn tight. The .480 pin needs to have the same attributes as a gauge pin. Like +0.0-0.0005 dia and a nice surface finish.

Can you make the pin after anodizing ?

I have saved companies a lot of money buy educating them on what is expensive and whats really expensive to do in a machine shop. Good luck :)



Evan

Re: machinist question, threw hole tolerances for pin/part fit?
 

I always spec on drawings "slip fit for 0.480 pin" etc. Model 0.480 for the hole. The machine programmers or operators can comp the hole to the correct size/use appropriate tooling.
In our programming we use nominals and then the drawings indicate size requirements. For instance if I was endmill boring the final diam on the 0.480 I would include a .001 offset on the programming, and then the operator can check and adjust the +-.001 that it may or may not need.
Modelling oversize would not make sense to me. Programmers need to use the drawings as well as the cad when laying tool paths.
Anodize buildup is so small that you won't need to worry about it. If it was snug after ano, running the pin through once or twice would make the perfect hole.

Re: machinist question, threw hole tolerances for pin/part fit?
 

I'd machine the bore after anodizing if possible. A chamfer will also help to line the pin up easier also. If the pin doesn't drop into your liking you can polish the bore a little.

Word. Mostly engineers that think they know but don't.:ror:

Re: machinist question, threw hole tolerances for pin/part fit?
 

agreed. my engineers are well trained to spec everything +.005/-.001 for this reason. I can program on the minus side, and compensate out. Drawings should typically be done to leave excess stock, as its easier to remove a little extra than to add a little back on.

Re: machinist question, threw hole tolerances for pin/part fit?
 

Thats the difference between a good machinist and a great machinist. One particular fellow refuses to do work unless I spec everything for him. I can't just say slip fit or press fit, drives me mad sometimes but at least I know what is being done.

Re: machinist question, threw hole tolerances for pin/part fit?
 

If the machinist is in house something like "slip fit on pin" is acceptable because he can check with the engineering team and determine if the fit is acceptable for your purposes. If I had a job shop and someone sent me a plan that said something like that for a quote I would reject it until they fixed the issue. There is no general understanding of what the terminology means, I dont want to make you parts that dont work for you and I dont want to charge you more to hold a tolerance tighter than you need it.

Of course it also depends on how many parts we are talking about, are we talking 1 part of 10,000 parts. Hell any machinist will easily dial in a very tight slip fit for you on 1 part but when you do volume they will need to know the acceptable range to plan budget accordingly.

Re: machinist question, threw hole tolerances for pin/part fit?
 

Aluminum plate & steel pin, lots of chances for the tolerance to change just on temperature alone.

Lots of good comments here, hope it works out.

PS, I do small runs of parts for myself & club members. I usually get a drawing with dimensions, then I go back and ask, "What is important, which way can I go on sizes."