Engineering type question

I am not an engineer and have no metal working experience, thus the questions.

If I were to have metal parts made by a CNC shop, at the cheapest rate, what tolerance could I expect. For example, if my file calls for a 5mm hole, what would be acceptable 4.8 -5.2mm?? Again, I have no idea of what is typical.

If designing a hole, that is supposed to have a rod go thru it, but be held tightly, like a 8mm rod and a hole, If I call for my hole to be 8.1mm is that enough of a gap to fit or do I need more clearance. Mind you I want it to fit tightly, but not so tight that I can not get the rod in the hole without a sledge hammer lol

If I have a 5mm screw, that I want to thread the hole for, should I spec the hole at 4.5mm and then tap it or spec it smaller or larger?

Thanks for any advice!!

For smaller hole they gonna use a drill bit anyway so it will be the precision of the drill bit( unless you require a really high tolerance), I dont think it will be so off as what you think, not 4.8 or 5.2 it will be 5 something if you need tolerance at only part you name the tolerance requirement in your blueprint, a normal if its not so important say 0.003- 0.005 inch will cost WAY less than 0.001 but if you need a 0.001" somewhere specified the location.

for your 8mm hole its depend of your shaft diameter and how good the tolerance is on the shaft,you can use some bearing fitting tolerance from tight to loose. But the less tolerance requirement the less is gonna cost, like your 8mm holder, maybe you can redesign it to have a loose tolerance and put a slot and a screw so when you tight the screw the hole grip the shaft. You can even but those holder already made that grip the shaft and all you have to do is screw them on your plate and this will also allow adjustment of your shaft. vs a straight hole.

Also dont forget to put some tolerance on your tap hole, if two part screw together you can some tolerance on both hole that gonna match I dont mean the diameter here, I mean the distance from edge and stuff, if you screw two plate together the one without a tap can have a large hole and less tolerance and bonus allow you to adjust later.

As for tap in aluminum you want 75% thread so a 5mm hole not gonna be 4.5 but 4.2 ish. check some chart around the web you can even use some imperial bit also , some chart recommend what drill bit to use.

There a lot of design trick you can use to avoid tight tolerance

It's up to you to supply the tolerances. With no tolerances specified how can the fabricator know what you want? Bear in mind that the tighter the tolerance, the more it will cost. e.g a hole with a loose tolerance can likely be drilled, but a hole with a tight tolerance will likely be drilled undersize then reamed to the the correct size, meaning an extra operation, hence higher cost. Engineering drawings always have dimensions and tolerances. e.g 5mm +/- 0.01 mm meaning it can be 4.99 to 5.01 mm. Or 5mm +0.02/-0.00, meaning it can be 5.00 to 5.02 mm.

This site may help for calculating fit tolerances.
[www.tribology-abc.com]

For threaded holes, I use one of these sites:
[www.shender4.com]
[www.shender4.com]

Why not talk to the CNC shop!
They will give you real answers and prices??

Hey they want to make the part right
and have happy customers!

Hi, I am possibly a bit late to the party on this but I might be able to help for future reference.

In general you are quite safe specifying the machining tolerances given in ISO 2768 MK for any non specific tolerances, save tighter tolerances for when you need a really specific fit or you will only add unneeded cost to the parts.

Drilling tolerances are given by the standard drilling capabilities on MIL AND10387-6. This gives the hole size tolerances a normal twist drill will achieve. Tighter will require more expense, so again stick to tighter tolerances than this spec when you need a specific fit.

This site brakes down the ISO standard fits well: [www.roymech.co.uk]
(seems to be over its bandwidth allowance at the moment, perhaps try the cached version).

For thread tolerances "6g" for external threads (bolts) and "6H" for internal threads (nuts) is fairly standard and all that is needed for most applications, tighter or looser fits are only needed when you have an unusual mating component.

Regards, Simon.

My first advice is to give up on getting the cheapest thing you can. focus on getting what you need and then consider the price. There have been several suggestions that may help. You could learn the tolerance specifications referenced by Hairyscreech, they insure you get what you asked for, but not what you may want or want to pay for.

Think of getting your car repaired, do you specify everything down to the torque of the bolts on the parts you specified or just tell them to fix it?

Cosmicray may have the best suggestion, talk to them, let them know you are tight and they may be able to pull some stock from under the bench and get you going. Depending on the shop, they may need a fully dimensioned print and order certified material, cause that is how they do it. Finding the right shop is more important than having the perfect print.

I would give general advice to describe the features you need done more like this: it needs to have a slip fit for the rod I am holding, can you measure it? It would not be good to give a ± dimension because you do not want it minus anything and only + so the tolerance (if you were to write it down may be 8.01+.02-.00mm) The right shop does not want or need you to write it down, they want a sample of the rod and an idea of how loose you want it.

As far as calling out the tap drill size for a threaded hole, there are charts with tolerances based on where you will use the thread from a wheelbarrow, to a jet engine. Do not bog down on that either. Tell them what thread size you want and let them do it.

Many shops will put a blank in a machine, touch off an end mill and do most everything from the model. If you don't have a model, they may need to make one. Big radii are usually cheaper.

The idea that there will be a drill then ream operation is probably not going to happen. Most machines can interpolate a feature tolerance of .01mm easily, more easily than you can inspect it. When you start buying reamers for a specific feature the price and lead time start going up.

You need to think about position tolerances also. if features need to relate to each other, let them know that also. Two locator pin locations may need to be related closely to each other more than to the edge of the part. If the pattern is off it may not be what you want.

The first part costs the most. If one part is $50.00 the one hundredth one is $5.00. If it takes an hour to set up a machine to make one, someone needs to pay for that, each part gets cheaper, that is one reason prototypes are expensive.

If these are simple parts, let me take a look and see what I can do.

Ken

The answers to your questions depend almost entirely on what process is being used.

Quote
n9jcv
If I were to have metal parts made by a CNC shop, at the cheapest rate, what tolerance could I expect. For example, if my file calls for a 5mm hole, what would be acceptable 4.8 -5.2mm?? Again, I have no idea of what is typical.

If your part is "flat" and can be cut by tilt-compensated waterjet (or laser in some situations) every feature will be +-0.05mm or better. Waterjet is also very cheap in comparison to other processes because you throw a plate on the table and press start.

If you are paying someone to machine a prismatic part from bar stock then standard tolerances are +-0.1mm but they are likely to achieve +-0.02mm or better just because of the processes being used. This will be expensive, especially if its CNC.

Drills will produce holes +-0.1mm but they aren't really designed for precise fits.

Quote
n9jcv
If designing a hole, that is supposed to have a rod go thru it, but be held tightly, like a 8mm rod and a hole, If I call for my hole to be 8.1mm is that enough of a gap to fit or do I need more clearance.

Precise holes are made using reamers. In most cases a reamed hole will be +-0.002mm or better, and will not be much more expensive than drilling assuming you are using a standard reamer size.

For metric shaft fits there are standard over under reamers, so 8mm, 8.01mm, and 7.99mm are all standard sizes. The over and under reamers are designed to slip and press fit respectively. Note that your shaft has to be of a known size for this to work, but linear shafts will work fine.

Be aware that a press fit will require an actual press to assemble. This is quite easy (and arbor presses are fairly cheap) but you might want to ream to 8.01 and locktite (or use collars/snap rings) instead.

Quote
n9jcv
If I have a 5mm screw, that I want to thread the hole for, should I spec the hole at 4.5mm and then tap it or spec it smaller or larger?

There are charts for tap hole sizes. A 5mm tap generally wants a 4.2mm hole but in rare situations you might go smaller or larger.


Design for manufacturing is tricky because decisions that look cosmetic or irrelevant can alter the cost 2-10x if they force a process change or complicate things in some way. It is almost impossible to design a part intelligently without understanding how it will be made.

Try to use a small shop willing to spend half an hour with you. Go over the key features and how they will be used, they will know what tolerances you need.