Mechanical Design Tolerances

This is very dependent on material,machine, and budget. Single point diamond turning of high purity aluminum can have form accuracies in the

50-70 nanometer range, with surface finishes under 1 nm RA, and opthalmic injection molding of plastic can come very close to these numbers.

Size tolerance is largely a function of surface finish, since measuring roughness involves determining the linear deviation of the surface from a reference surface, as does the size measurement.

Get hold of a copy of Machinery's Handbook and take a look at the "Surface Texture" section. There is a chart showing the ranges of surface roughness for all types of cutting, machining, polishing and casting. In my 23rd Edition it's on p. 705.

Good luck!

Don Kansas City

Depends on the size and quality of the machines.

The best way to get this info is to call up your vendors--the question is not what are generic tolerances, but rather, what are the tolerances for the folks you work with?

For instance, I have a machinist that works to a standard tolerance of

+/-.002 in most cases. Anything tighter than that costs extra--anything looser than that is happily accepted, but doesn't really yield any economic benefit. My other machinist (using essentially the same equipment) works to ~+/-.005

Sure, some machinists and welders are more accurate than others, but tolerance is tolerance and they must meet it. A good engineer must know what a reasonable and feasible tolerance is for a given process. I see newly-graduated engineers all the time that try to indicate ridiculous tolerances on their drawings.

I think what James is asking for is a general range of what is normally possible for different methods of machining. You wouldn't, for example, specify a +/-.0001" tolerance on a bolt clearance hole that is to be drilled.

Generally, the tolerance should reflect design intent; the machinist will decide how he wants to get there. If you intend to mount a precision ball bearing in a housing and the bearing manufacturer's specs call for +.0001/+.0007 and a 16 u-in finish in the hole, then that's what it should be, and that's what the drawing should say. The machinist will know whether he needs to mill, bore, ream, hone, or lap the hole to do this. As long as you get the hole you want, who cares how he did it?

They can usually achieve just about any reasonable tolerance that you ask for: it just takes more time and money as the tolerance gets smaller. In general, an engineer should specify the coarsest tolerance that is acceptable (whether for technical or aesthetic reasons) to keep costs down.

Don Kansas City

Don,

You`ve got the idea, yes I appreciate tolerance is a function of cost and vendors ability. But I`m looking for a general range, like you mentioned to avoid the new designers over or under designing products/machines.

James

eromlignod wrote:

It depends on the products, volume, cost ... and many other things. I design professional equipment for IT (printers, check readers,....) that are produced in volume from 500 to 10.000 per year and as a general rule (ISO and mm) : general tolerance Js13 moulded parts Js 11 angles +/- 0.3° roughness N8

when more precision is required for machined parts: shaft h10, h9, h8 holes F10, F9, F8 (or E position)

for molded plastic parts, die casting and sheetmetal stamping and bending we try to use the same

Maybe some Design For Manufacturing books, websites could help you.

Lorenzo

James,

I would have to echo what Don is saying. The tolerance should be the coarsest tolerance that will produce a "servicable" part based on the design intent. The tolerance that makes a servicable part will set the cost. Inexperienced engineers get into trouble because they do not understand what makes a servicable part based on the design intent or they call out processes that are incompatable with the required tolerances. I believe it is the second situation that is your area of concern. So that generates a few questions/answers. Are the parts machined out of house - if so, do not call out the process. Let the outside vendor determine the correct process based on the required tolerance you provde and quote it accordingly. If it's being done in house and your young design engineers are also serving as process or production engineers, then they will need to understand not only what tolerance makes a servicable part but what tolerance each process, particular machine, and operator are capable of holding. Are we getting closer to your question?

Al

OK. But the tolerances must be given as tolerance *grades*, not actual dimensional numbers, since +/-.001" on a .125" dia. shaft means a completely different thing than +/-.001" on a 12.0" dia. shaft, regardless of machining method.

Here is a general guide to IT tolerance grade ranges for some processes (from the M.H.):

Lapping & honing: 4-5 Cylindrical grinding: 5-7 Surface Grinding: 5-8 Diamond turning: 5-7 Diamond boring: 5-7 Broaching: 5-8 Powder metal - sizes: 6-8 Reaming: 6-10 Turning: 7-11 Powder metal - sintered: 7-10 Boring: 7-11 Milling: 7-11 Planing & shaping: 10-11 Drilling: 10-11 Punching: 10-11 Die casting: 11+

This is the tolerance grade number. If you look it up in a standard table that lists the specific allowance (in mm or thousandths) for a given part size, it gives you an idea of what allowances can be expected. This is the "number" part of the tolerance symbol (sans the position letter).

Hope this helps!

Don Kansas City