Injection Mould Models

[cdown]

Guru's, A bit off total really after advice / standards really. We are currently looking into gonig over to injection moulded parts for some items on our products. How ever the question I am really wanting an answer too is regarding model set up and what are the thought on drawings?

Our current thoughts are either a full dimensioned drawings& models, or aminamal drawing and model.

also what are the views on holes sizes etc on models, ie how do you show tolerances etc, are holes modeled top end, lower end of tolerance or the mean?

Might be simple questions but not had a great deal of experiance of using models to manufacture moulded parts

cheers

Colin Down

Design Engineer

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.

[scooke]

Dear Colin



As a tool room and injection moulder I would prefer models and a minimal
drawing which dimensions only those sizes that are important to you as the
client. A fully dimensioned drawing actually only serves to divert
attention away from what is really important.



Regarding hole sizes (and in fact any features) the key thing to remember is
that in a mould once the steel has been machined away it is more difficult
to correct. You have to add steel back before you can correct the size and
this means either putting in an insert or welding (and welding is not an
acceptable option for a new tool in my opinion). So if a size is important
to you, tolerance it correctly and allow the tool room to adjust accordingly
to leave metal in the mould to hit your tolerance band.



In general plastic mould making is not easy as the shrinkage and warpage
that occurs during the process can cause problems in achieving the desired
final sizes. Many plastic part designers apply steel press tool tolerances
to plastic parts which in most instances are not achievable. (Worse still is
machined tolerances!!) There is an excellent (but now I believe obsolete)
ISO standard for plastic mouldings called ISO16901. It was very well
thought out when it was first introduced and takes into account the type of
polymer being used, the size of the part and the intended grade of accuracy,
and then gives tolerances that are actually achievable with the process.
Like most documents that address a complex process it is not simple to
understand! However if you can get you head round it, it will save pain in
the long run. If you need tolerances that are tighter than the recommended
tolerance then it must be planned into the toolmaking by leaving steel on,
moulding a first trial and then finally adjusting to size. This of course
adds cost to the tool.



Lastly my personal preference is to receive a model without drafts and
rounds especially if your toolmaker is not using Pro|E. If a part has been
drafted and rounded by an inexperienced part designer, the part can require
hours of work before one can even start to design the tooling, because most
part designers I have had to work with do not understand the requirements of
robust mould design, and we are always striving to give our customers the
best quality mould and part.



Our company has 34 years experience in making plastic moulds and injection
moulding and we design and construct complex injection moulds for a wide
variety of industries including automotive. We're still using WF2 including
tool design set, expert mould base extension (EMX) and Pro NC/MFG and there
is nothing we can't design and build with it!



Hope this helps



Best regards



Steve



_____

[rreifsnyder]

I agree with most of what Steve has said, the only proviso being that I have had instances where we needed to include draft. One project in particular, we spent a lot of time working the geometry to get good shutoffs and pass through so that we could end up with a simple open/close tool. Unfortunately, due to corporate policy (this was prior to my coming to Lockheed) we were separated from the vendor. They took our model, stripped out all the drafts and put all sorts of slides and cams into the tool which increased cost while reducing cycle time and reliability. The lesson from that is to work with your vendors. They're usually the experts in what they can do, but don't just take what they say if you really need some aspect. No offense, but sometimes they will push the capabilities THEY have or what makes it easiest for them and not always what YOU NEED.

Rob Reifsnyder
Mechanical Design Engineer/ Pro/E Librarian
L
Mission Systems & Sensors (MS2)
497 Electronics Parkway
Liverpool, NY 13088
EP5-Quad2, Cube 281
work: (315) 456-4307
cell: (315) 317-4304
-<">mailto:->



From: Steve Cooke (C & S) [

[bgruman]

Rob, Steve,

Great feedback! I couldn't agree more.

15 of my 16 years experience has been in the class "A" and other complex
part design of thin wall plastic and cast parts. (for Injection, SMC, Roto,
Blow, Hand laid fiberglass, sand cast, die cast, etc etc.) The other one
year I was designing molds in a tool shop. All of this time has taught me
one main thing... Communication between the Tooler, Molder, and Client is
key. As a Designer/Modeler (usually hired by the client) I find myself
playing middle man in this communication to make sure that the Clients needs
are met, while also establishing parting lines, draft, and incorporating
slides and lifter where necessary to accommodate the Toolers, and Molders
capabilities. In the end, you get a model that is 100% accurate, satisfies
all three parties involved, and can go directly to the Toolers CNC
programmers. Then the Client uses this same model to create a minimal
dimension drawing that calls out only the important features required for
quality and inspection purposes.

As far as Tolerances go, The Client needs to understand the material and
tooling, and molding tolerance capabilities so that "realistic" tolerances
can be applied, but then the Client also needs to fully understand the
"needs" of the end product and needs to tolerance the inspection dimensions
accordingly. Then the Tooler can do whatever they need to for first shot
parts, and can adjust later if needed without weld-up.

Good Luck.
Bernie

Bernie Gruman
Owner / Designer / Builder
www.GrumanCreations.com




On Mon, Jul 11, 2011 at 10:24 AM, Reifsnyder, Robert <
-> wrote:

> I agree with most of what Steve has said, the only proviso being that I
> have had instances where we needed to include draft. One project in
> particular, we spent a lot of time working the geometry to get good shutoffs
> and pass through so that we could end up with a simple open/close tool.
> Unfortunately, due to corporate policy (this was prior to my coming to
> Lockheed) we were separated from the vendor. They took our model, stripped
> out all the drafts and put all sorts of slides and cams into the tool which
> increased cost while reducing cycle time and reliability. The lesson from
> that is to work with your vendors. They’re usually the experts in what they
> can do, but don’t just take what they say if you really need some aspect. No
> offense, but sometimes they will push the capabilities THEY have or wha t
> makes it easiest for them and not always what YOU NEED.****
>
> ** **
>
> *Rob Reifsnyder*****
>
> Mechanical Design Engineer/ Pro/E Librarian****
>
> *L*****
>
> Mission Systems & Sensors (MS2)****
>
> 497 Electronics Parkway****
>
> Liverpool, NY 13088****
>
> EP5-Quad2, Cube 281****
>
> work: (315) 456-4307****
>
> cell: (315) 317-4304****
>
> -****
>
> ****
>
> ** **
>
> ** **
>
> *From:* Steve Cooke (C & S) [

[lylebeidler]

I agree with what Bernie said: communication is the key.



Re: draft vs. no draft: there are times when the part designer must have
draft in the model to accurately reflect the geometry & ensure the good fit
of the finished product. At my previous employer, I was modeling a "tub"
that held hanging file folders; we needed to model the draft to ensure that
the paper would fit at the bottom, while still allowing the metal strips in
the hanging folders to hook over at the top. This is just one example of
where draft is not a byproduct of manufacturing, but an input that you must
account for. This example also goes back to the communication issue - we
actually had to have discussions with the molder regarding the draft angle;
IIRC, we needed to halve their desired draft angle in order to accommodate
the paper fit. This, in turn, required a change in texture on those inner
walls. It's all in the partnership & communication.



--



Lyle Beidler
MGS Inc
178 Muddy Creek Church Rd
Denver PA 17517
717-336-7528
Fax 717-336-0514
<">mailto:-> -
<">http://www.mgsincorporated.com>

[BrentDrysdale]

Hi Colin
Is see you got a comprehensive reply from Steve Cooke from the
toolroom/molder side of things and some nice comments too from Robert,
Bernie and Lyle; makes my comments easier.

I started as a toolmaking apprentice and did a couple of years post that as
a toolmaker meanwhile doing study in plastics engineering. Graduating from
there I have since worked in the area of Mechanical Design (last 16 with
ProE). Total span is 35 years. Most of my life and I am still learning and
improving.

Basically I think Bernie has the best encapsulation but I do appreciate
Steve's comments on having to do a lot of rework on parts that are poorly
designed with respect to the toolmaking aspects. They all talk about
communication and I heartily endorse this.

Design in plastics is a minefield for the unwary. Most assume you can just
port over some design that has been made by some other process and this is
so often wrong you can just say it is wrong.

What your parts need to do includes the geometrical form but also the
strength (static, impact and creep), durability in handling/use conditions
(such as chemical or UV resistance), regulatory requirements (e.g. UL), end
cost (combination of tooling cost/efficiency plus material cost/weight and
handling), number of parts you are planning to make (different decisions for
a total part life of 1000, 10000, 100000 and 1000000 parts). The list goes
on and on.

As you start down this path I recommend registering with
IDES

For you I would say that one of the easiest ways to get into this is to work
with suppliers who have ProE so that you can share files back and forth so
they can look at an early model from you without any draft or fillet rounds
and give you feedback on what they recommend for these things.


We use Moldfl...

[ikamster]

Colin,

In my experience,I have always included all draft and fillets inmy models, and the models are always constructed to nominal dimensions. You need to include things such as draft 7 radii, to check for clearences between mating parts, and to watch out for die-lock conditions, material flow, and possible sink marks. Our drawing usually have minimal dimensions. We include overalls, and dims to locate any holes and locators. Include a general note on your drawing that says to refer to cad data for any dimensions not shown.

[Tundra]

My 2 cts...

RE: "Shrinkage"

Designed a thin-wall (.020") trigger sprayer housing for a snap fit. Basically created the Pro/E model geometry such that the front end was actually splayed out 10 degrees more than the required finished part. This was "Kentucky windage" on the Pro/E geometry for the mold such that after injection and cooling, the part front end shrunk back to its design intent...

[wattsteam]

Hope you bought a lotto ticket afterward - cause you were lucky.

JD

[wattsteam]

A note I frequently use when the part accuracy is not so critical is " All undimensioned features to be per CAD data file (filename-revX-date) within +/-0.3mm."

JD

[scooke]

For ABS, where the shrinkage is most consistent across a wide range of
geometries and wall thicknesses, applying a general tolerance of +/- 0.3 mm
to any dimension over 40 mm on your model exceeds the limits set in ISO
16901. You are therefore specifying a tolerance that is tighter than what
is readily achievable in injection moulding on the first mould trial. A
competent tool maker will factor this in to his quotation and it will
increase the cost of the tool as he plans to adjust the size after first
trial and this may be completely unnecessary.



In my original post I stated that I thought ISO 16901 was now obsolete, does
anyone know what might have replaced it?





Steve

_____

[wattsteam]

I did not mean to say that 0.3 is the number to use for all parts of all sizes, I should have said "+/-x.x (actual number to suit process and material)".

These days I refer to SPI's tolerance guide data rather than ISO's.

JD