Moulded Parts

[cdown]

Sorry for being a little off topic here but a little help is required.

We are looking into doing moulded part for the first time and are
struggling to find what tolerance specs to state on our drawings ie ISO
standards, is there such a thing?

Would anyone be willing to share company standards or drawings with these
specs on?

Any help would be greatly received

Thanks

Colin Down
Mechanical Design Engineer
email: -
tel: +44 1305 208503

The information in this e-mail and any attachments transmitted with it are provided in commercial confidence for the intended recipient(s). If you have received this e-mail in error, please notify the Postmaster by e-mail at -. Any views or opinions expressed are solely those of the author and do not necessarily represent those of DEK.

For local company specific legal information for your country or region and any local contact information for DEK, please refer to:


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[dgschaefer]

I'd defer to your molder's preferences and keep in mind that some parts,
like in any process, are going to be special cases where tolerances are
going to need to be looser. Of course, if you need it tighter in a
certain dimension, your molder may be able to accommodate. Best to
discuss this early in the process, before the mold is made for sure,
early in the design process is better.



Shrinkage plays a part in the tolerances that can be achieved.
Generally plastics have different shrinkage in the direction of flow of
plastic through the mold than across the flow, although it's not usually
a big concern. Some part geometries are going to induce more shrinkage
in one direction versus another, and that can sometimes cause problems.
There are a lot of process variables that can affect shrinkage, final
size, warp and so on. Your molder is going to handle that stuff, but
giving him a well-designed part up front is going to give him more room
to play with. I'd get your molder involved earlier than later to give
you help getting the design optimized. He should be able to look at
your design and know about what's going to happen.



Since some plastics shrink significantly more than others, standard
tolerances will vary based on the material used. More shrinkage, more
tolerance required. With that in mind, a decent rule of thumb we've
used is you can hold 20% of the shrinkage across a given dimension.



For example, a good tolerance on a 10" dimension in PVC with shrinkage
of 0.035"/inch:



Total shrinkage: 0.035" * 10" = 0.350"

Tolerance: 20% of .350" = +/-0.070"



Same dimension in ABS with shrinkage of 0.005"/inch:



Total shrinkage: 0.005" * 10" = 0.050"

Tolerance: 20% of .050" = +/-0.010"



Now, on higher shrinkage materials like PVC, your molder should be able
to do better than the 20% rule, but it's a good starting point for
discussion. Most plastics don't shrink quite that much, more in the
range of 0.001" - 0.015" with a few exceptions. Unfortunately, cheap
stuff like polypropylene and polyethylene are both exceptions at around
0.020".



The good news is that once the tool is final and the process is dialed
in, the parts are generally very repeatable. So, the first articles may
need a generous tolerance, but ongoing production, especially on a per
lot basis, is going to be in a narrow range somewhere in the overall
tolerance band.



I hope that helps,



Doug Schaefer

[mlocascio]

Colin Down,

It seems to me that a committee is required here. Usually tolerances are
determined by the capabilities of various machinery and operations. They are
also a function of cost and operator competency. So you need to consult with
them.

For you to get drawing standards from another company might work. However
these standards might not fit your "mold" ,if you know what I mean.

Michael P. Locascio

[ptc-593619]

This also raises the question of your model intent. If you model at
nominal most tolerances will be plus/minus. However it may be
advantageous to model at maximum condition (blackbox condition) and
tolerance zero plus. Or some applications may require the minimum
condition (maximum clearance) so tolerance accordingly. I usual leave
the shrinkage allowance to the mold maker, they generally know much
better than a lay person what happens in the mold. If all else fails,
you can always "qualify machine" - but at added expense, of course.

Drafting also comes into your tolerance scheme - most mold makers want a
45 degree draft! That raises the point of whether you tolerance at the
top or bottom or neutral of the draft.

I feel your pain in your struggle to apply a standard, Colin; maybe one
doesn't exist to cover all eventualities.



Richard A. Black

Lead Design Engineer

Eaton Corporation

440 Murray Hill Road

Southern Pines

NC 28387 USA



tel: 910 695 2905

fax: 910 695 2901

richardablack@eaton.com

www.eaton.com

[wattsteam]

I agree 100% that early consultation with an experienced moulder and/or mouldmaker is always a good idea when designing plastic parts.

I don't agree with ever modeling parts at max. size. For best results in plastics all features should be modeled at the mean size and have (suitable for size and materials) equal +/- tolerances applied.

A good general guide for draft is to start with 1 degree per side and if need be in specific small areas this may be reduced to 1/2 or 1/4 degree per side if these areas are kept small and depending on the plastic used. The more draft there is the easier the part will eject.

For sealoffs and parting line steps 5 degrees per side is minimum, 10 degrees per side is better, if space permits. Less than that and severe and rapid mould wear will likely result.

There are exceptions of course but the above are general practices established over more than 25 years in the plastics industry.

Planning to machine plastic parts after moulding is not a good idea for several reasons. In most cases where this might be necessary, the machining can often be designed out if the parts are considered as a whole system including all tolerance stackup, prior to detail design.

If there is a particular feature that needs a very close tolerance, the mould can be made 'steel safe' or at mould MMC/part LMC on that feature. The mould is run until process is stable, parts are measured, then mould is machined to bring the part to size. Some people call this "sneaking up" on the size. Again a stable process is critical before final mould adjustments. This may mean running and scrapping quite a few parts until process stability is achieved. Google 'scientific moulding' to find out more.

Best regards Jeff Dayman

[scooke]

Hi Colin

Everyone else has expounded on the specific challenges facing toolmakers and
moulders. All their points are valid and I won't add to that.

There is an old tolerance standard for plastic parts which is now obsolete
and I have been unable to find what has replaced it. It is a German standard
DIN 16 901 and it was really well thought out. It takes into account the
different types of material and applies the tolerances with respect for
their characteristics. (e.g ABS is afforded a much tighter band than PP or
PE). This would be a good starting point to apply to your parts and then
"negotiate" with the moulder/toolmaker where you have to tighten up to meet
your design intent. This way you will keep your tooling cost as low as
possible. I have built these tolerances into tables in ProE which makes it
really easy to see for each dimension what will be applied.

If you want a copy of the standard or my ProE tables contact me off forum,
but bear in mind that we are still on WF2 although tables should come up
without a problem.

If anyone knows of another plastic tolerance standard that might have
replaced DIN 16 901 I would like to know.

Best regards,


Steve

[mlocascio]

I second this motion. All in favor say "Aye."

Michael P. Locascio

[stevei_pe]

See SPI AQ-102. You can purchase a PDF from the SPI online store for US$30, I believe.

This specification has tolerances for27plastics (according to the SPI website). Hope this helps.

Best regards,
Steve Ijams, PE


-----End Original Message-----

[dgallup]

The Rubber Manufactures of America (RMA) also has a table of standard tolerances for molded rubber parts. You can just google them and find the values. They have several classes, A1 is the highest precision.

Material selection will have a big impact on the tolerance that can be achieved. Highly filled engineering thermoplastics can hold very tight tolerances compared to unfilled LDPE. Floppy parts are particularly difficult to tolerance & inspect.

There is an ASME Y14.8 for dimensioning castings, forgings & molded parts. That won't tell you tolerancing but does have a lot of good info on dimensioning schemes.

PTC quality philosophy: We've upped our quality standards. Up yours.