FEA of a complex injection molded part with an orthotropic material?

[renderedchild]

I have a customer who is using a plastic with a sort of carbon fiber fill material in various injection molded parts. The material is well characterized and quite orthotropic (anisotropic). They want to run FEA on these parts, but I don't have experience running FE simulations on orthotropic materials.

I've put calls in with ANSYS and Abaqus to inquire if any of their software tools can do this, but haven't been able to speak with anyone technical with answers yet. We typically use solidworks simulation, but are mostly in the linear / isotropic world. My Solidworks VAR said that their simulation package cannot handle orthotropic materials where the material grain direction is changing across the part in FEA.

Are there any software packages (ANSYS, Abaqus, etc) that can handle complex parts and orthotropic materials? I'm guessing there would first be a plastic moldflow type analysis that predicts the fiber orientation, then that data gets imported into your FE solver. This would be ideal, am I just dreaming?

Beyond a software package that can handle complex parts and orthotropic materials directly, are there common techniques for analyzing this kind of thing? I know there are all kinds of high fill plastics that have been used for ages, so I can't be the first person to ask this. Unfortunately in my early searches I haven't been able to come up with a lot of answers, which suggests to me that it's not an easy problem to solve and it will involve a lot of simplification of parts and testing.

Thanks in advance!
-Chris

 

[Mustaine3]

I'm not familiar with Ansys, but Abaqus can do it.
Tools like Moldflow or Simpoe can generate a file that can be reused by Abaqus to have material data for each element.

 

[FEA way]

I think that both Ansys and Abaqus can handle this. Ansys has ACP (Ansys Composite Prep/Post). However Abaqus is usually considered as the best choice for composite modeling. It has several features dedicated to these materials. Especially Composites Modeler add-on for Abaqus/CAE. Both Ansys and Abaqus support data import from external software (like Moldflow) to define fiber orientation in detail.

If you want to know more about composites modeling in these two programs I recommend the books by E.J. Barbero (Finite Element Analysis of Composite Materials Using Abaqus/Ansys).

 

[ESPcomposites]

Before you get too carried away with the FEA orthotropic modeling, you might want to be sure you are going to meet your objective if you do so (there can be some pitfalls). Lets talk more about this:

DEFLECTION ANALYSIS:
D1. If the primary interest is an accurate deflection analysis (or related), then using a model with an orthotropic material as function of the grain direction will be the most accurate approach. In that case, you can look into various packages that can address this (they do exist).

D2. However, if you are less interested in deflection (or don't need high accuracy), there are a few options. First, just how "orthotropic" is the material? As a first order approach, you might be able to model it as an isotoropic material, where you use the properties from the orthotropic material that contribute to the greatest influence of deflection. For example, a orthotropic beam in bending can be modeled (with very good accuracy) as an isotropic material since there is a primary direction of influence.

D3. Another approach is to partition sections of the model and assign those ortotropic properties. I suspect you *may* be able to do this your program already with your program (there is a difference between applying an orthtotropic material to a bulk section of the model versus as a function of a complex part where the orientation is continuously varying). In other words, if you have large portions (geometry or elements) that have the same coordinate system, you can use that to your advantage. You could then just apply isotropic materials to the more complex sections of the model. Deflection is an overall property (i.e. a summation) so if you get most of right, you will be close.

STRENGTH ANALYSIS:
Often times you will be interested in strength and there are some engineering challenges that the FEA cannot address.

S1. Do you have a 3D failure criterion for this material? The more orthotropic it is, the less likely you are to have something that is valid. The more isotropic it is, the less necessary it is to model it with an orthotropic material. Either way, there will be challenge here that is outside of the FEA's domain.

S2. For injection molds, there can be a lot of scatter for the strength properties. This may be a function of the specific part and how it flows, batch to batch variations, etc. This is especially true at stress concentrations and smaller features, which unfortunately are often the failure locations. It may be difficult to establish a statistically based allowable (A-basis or B-basis) that can be used across the board (unless conservative). In the end, you may find that you have to test the completed parts directly to establish a statistically based allowable load (as opposed to a stress analysis with the FEM).

S3. Because of items S1 and S2 (and D2 and D3) you may find that an accurate ortotrhopic model (using a different software and including the learning curve), may be not have much real value compared to the associated cost. But again, it depends on your goals. One thing you can do is compare finite element models in a relative manner (i.e. look at stress concentrations with different sized features), but that could probably be done with an isotropic model since it is only a relative comparison.

Brian

http://www.espcomposites.com

 

[rickfischer51]

If you want to accurately account for fiber orientation you must begin with a mold filling simulation. Fiber generally aligns with the flow direction at the surface and perpendicular to the flow direction in the middle of the section. Flow direction will vary all around the part and is totally dependent on gate location. This means the following:
1. The mold filling simulation must begin with an optimization of the molding process.
2. Once the process is optimized, the shrinkage, warp and fiber orientation simulation are performed.
3. Based on these results, the customer and molder agree to gate location.
4. The molding simulation must be performed by someone with a strong background in injection molding, polymer science, etc.

Another benefit of this analysis is that you will see where knit lines are located. Keep in mind that fiber will not cross a knit line, so you will not have full strength perpendicular to the knit line. Knit lines can in fact sometimes be "resin poor", meaning that excess fiber has collected at the knit line, replacing resin that is needed to do the knitting. For this reason you must make sure that knit lines do not occur at high stress locations.


Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[renderedchild]

Thanks so much for all the input!

At this point I'm pushing to do some testing on actual parts to see how orthotropic the material really is. I'm hoping that the way the test coupons were shot in the mold, all the fibers are oriented along its length much more so than a real world part would be. Maybe I can get away with analyzing parts as isotropic.

I'm also talking with ANSYS and Abaqus to get more info on their capabilities, they're wanting to do some trials to make sure the software will do what we're asking it.

Again, thanks for the great feedback!

-Chris