I`m trying to build up a training guide for some of my design
engineers. Can anyone help me with listing the typical tolerances for
the following processes:
Plastic Injection Moulding
Metal Injection Moulding
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.
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
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
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
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°
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.
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?
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
Powder metal - sizes: 6-8
Powder metal - sintered: 7-10
Planing & shaping: 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
Hope this helps!