Non-Linear Plastic Shrink

SolidWorks is a dream for hard parts and plastics with linear shrinks
when you use the cavity feature to create metal cavity parts.

Non-linear shrinks of Polyethylene and Polypropylene can't be handled
inside of SolidWorks "Cavity" function and I accept that. Cost
containment , inertness, and incineration favor some of these very
very simple plastics which essentially consist almost entirely of
carbon and hydrogen for use in medical & food products.

What I am wondering is how mold & product designers reconcile the
differences in the drawings between the actual final parts and actual
tool. Solidworks doesn't allow me to go in and "Edit" a tool insert
to get it correct, except by putting up a note.

It is a non-trivial issue in todays world where the FDA GMPs are
considered.

What do other designers do with non-linear shrink issues?

Bo

 

I have seen people actually model this in. Come to think of it, it was
warp instead of non-linear shrink, but same concept. They made a prototype
tool, measured the warp and then made the production mold with the part
deformed the opposite direction.

SW does have the ability to do different shrink rates in different
directions, which in some cases might serve as an approximation, but the
problem is that the direction of flow is never aligned to the origin in the
real world.

In practice, it's mostly done at the mold builder. Make all your walls
steel safe, then whittle away until you get it right. Very time consuming
and expensive.

Mold process is also important, pack pressure, gating, venting, cooling,
cycle time. As deterministic as we are, injection molding still has a lot
of black science or trial and error involved.

Moldflow software has tools that help you predict anisotropic shrink
effects as well as warp and sink, but I don't think it's possible to go
electronically back to the CAD model to make corrections. You have to take
measurements in Moldflow and take the numbers back to your model to tweek
the shape. http://www.moldflow.com/Products/MPI/modules/shrink.asp

matt


(Bo Clawson) wrote in

 

Snips

SolidDesigner from CoCreate had a pretty good solution for this over 5 years
ago. When you did your differential scaling you could select features that
you wanted to scale isometrically, like round pins. The location would be
scaled differentially, but the pin stayed round. It still didn't get around
the fact that you really need to be able to define the shrinkage directions
locally.

Jerry Steiger
Tripod Data Systems

 

Bo,

In the few instances I've had to deal with non linear shrinkage, I was forced to model the molded part in SWX and
manually shrink the sketched dimensions.

Malcontent

 

Bo:

In 2004 the "Cavity Feature" DOES have "Non Uniform Scaling".

 

Jacob, thanks for the note from SWks 2004, which I am not using yet.

What I see in my medical cylindrical tapered fittings work (like the
ANSI 15mm & 22mm anesthesia/respiratory fittings) where functional
diameters need to be met, is that I can't keep a constant wall and the
thicker the wall, the more shrink in the Polyethylene & Polypropylene
materials. That is different than X,Y, & Z shrink rates being set
differently.

The 3D CAD software may never realistically be able to deal with it.
Obviously there is a disconnect in being able to have the part drawing
directly relate to the tool when the shrink is non-linear. One of the
solids is going to be "wrong". Since the part drawing needs to be
"right" for inspection of finished parts, the tool solids will remain
"wrong" and need the manually noted 'adjustments'.

I suppose a real elaborate FEA program could step in between the part
drawing and the cavity shape, but that would introduce lots of
decisions that would get real sticky in a hurry and probably require
the user to make a lot of judgement choices.

It looks like the solution is manual corrections.

Bo

 

John,

I do much the same process when needed. What I do though is create a new
configuration in the plastic part model for shrinkage. Then adjust all of
the part dimensions for the non-linear shrinkage manually for that
configuration only. I will have 1 configuration showing the original part,
and 1 configuration showing the part with shrinkage allowance added. I just
have to make sure that I have the part set to the correct configuration in
my assembly when doing the cavity feature in you steel, and use 0% shrinkage
in that feature.

The problem like you said is on complex parts as well as imported parts.
Makes it kind of impossible...