Composite Modeling 3

[JPhysics]

I am new to Abaqus and Composites so please bear with me the curve is quite steep and I keep falling down.

A couple of basic questions:
1. The best way to "Model" the composite part. I have a SolidModel from SolidWorks and a Surface Model also from SolidWorks, which one should I use and why?
2. Material Properties: The units, no matter which SolidWorks model I use, it imports as mm. Does this mean that all my material properties have to be in N/mm^2? Resutls are then in MPa?
3. I am interested in the Tsai-Wu failure criteria which the help file says is available, but I cannot figure out how to get my output in this format. Any help here?
4. When creating a layup on a complicated section is there any way to re-orient some of the selected faces while leaving the others alone?

 

[tgrimley]

1. Depends what you're interested in. Surfaces are usually fine and computationally cheap, and easy to mesh.
2. There are no units in ABAQUS. You must only be consistent. That is, your geometry units must match your load units which must match your material properties units. You can use whichever you like. You can also scale geometry when importing to make it appropriate for whichever system you choose. Use the geometry diagnostic and measure distance when importing to be sure it imports at the scale you think it does.
3. I think this is a field output. You must specify all the relevant failure crit before it is selectable, iirc.
4. Yes, each face can be assigned different material orientations based on offset angles and local coordinate systems.

 

[Composites_FEA_Guru]

Hi JPhysics,

I'm going to build on the advice given by tgrimley...

1) If your stresses are primarily in-plane and the out-of-plane stresses (33, 13, and 23) are not of concern, then an imported surface will be easier and quicker to work with.

2) Assuming you apply loads in N and your material properties in MPa, then yes, stress results will be in MPa.

3) TSAIW is the field output for the Tsai-Wu failure criterion. You'll need to specify the Fail Stress values for your material(s) with a *FAIL STRESS keyword in your input file or as a Suboption when defining your material inside Abaqus/CAE. Also note that Tsai-Wu only works for plane-stress formulated elements (shells and continuum shells).

4) You can assign a different orientation to each element if so desired. To do so you'll either need to partition your geometry to have different regions to assign different material orientations to or create element sets on a meshed model to assign material orientations to.

Hope this helps. I'd be interested to hear about your reasoning for choosing Tsai-Wu as your failure criterion. There are more accurate failure criterion available for uni-directional composites than Tsai-Wu. And if you are using woven composites, the Tsai-Wu formulation inside Abaqus isn't appropriate as it is the transversely isotropic material formulation when the 1-2 plane is the plane of isotropy (i.e. uni's only).

 

[ESPcomposites]

Generally speaking, in the aerostructures industry, the FEM is used to first generate loads only (unless it is a "detail" FEM)

From there, you use those loads and apply them to "details" such as a bolted joint, cutout, etc. While some FEM models are appropriate for strength checks, it is less common to use this approach. However, this is just the strategy used for aerostructures and especially when dealing with the FAA, which does not apply to all structures.

The Tsai-Wu/Tsai-Hill failure criteria are more popular in academia than in industry. A few problems:

- I believe it was discovered the testing methods used to validate the failure criterion were not appropriate.
- Even if the test data was validated, it would only be for a lamina. The extrapolation to the laminate level is suspect at best.
- Does not give an indication of failure mode and you don't have the ability to "remove" stress/strain components (i.e. the max strain failure criterion may selectively neglect the matrix or shear failure modes).

Brian

http://www.espcomposites.com

 

[JpPhysics]

WOW... thanks for the replys, I deffinately have a lot to learn about composites and Abaqus.

One quick clairifcation on my composite layup.

So I have a small wing that I am selecting. The wing is made up of several curved surfaces. I have partitioned teh wing so that I can easialy select the areas for the layup. Not all layers go the entire length of the wing.

I notice that when I select a set of faces for a particular layer, each face gets a local "Coordinate System" for lack of a better term but they are not all aligned. That is not even the X or 1 direction, which is along the length of the wing, is aligned. Is it necessary for me to repair this in order to get an accurate result? Of course the follow up question is how because I am not finding an easy way to change the direction on the selected faces individually.

Thanks again.

 

[JpPhysics]

One more thing....

Since this project is my first attempt with composites... may I pick your brains a bit.

Usually when I am running an analysis on a component, typically a machined component, I will run my analsysis then compare the analysis with a test case that is fairly simple to set up. For example, hanging a weight off a simply supported beam. Then I check the deflection in real life with the deflection from the fea and as long as I am within 2~5% I feel pretty good.

I did this same thing with this composite layup and I can get the fea to within about 10% of deflection an a given load, but when I double the load, the fea no longer follows the observed experiment. Is this common for composites or do I have something set up incorrectly?

Thanks again.

 

[ESPcomposites]

Deflections are much easier to correlate than strength predictions. If the reason for this is not obvious, then let me know.

Are you saying that your experimental deflection data is nonlinear or that you are using a nonlinear FEM? One of those has to be true.

In general, there is nothing "special" about composites that would cause this to occur (for typical problems). But there could something specific about your test case that would cause this (i.e. large deflection, etc.). We would need more information to make an assessment.

Brian

http://www.espcomposites.com

 

[Composites_FEA_Guru]

JpPhysics,

By default, the laminate orientations on your model are aligning themselves with the global coordinate system. In addition, if you are using shell elements that have an element normal, the 3 direction of your laminate orientation will align with the element normal. You will definitely need to fix what you see to get accurate results. There are multiple easy and convenient orientation tools available inside Abaqus, the documentation can explain their usage/functions better than I can. I recommend looking into "Discrete" orientations for complex geometry if you are working with Abaqus 6.9-EF1 or later. If not, look into "OFFSET TO NODES" orientations that can only be defined through the input file (not supported by Abaqus/CAE).

Regards
-CompositeModeler

 

[Composites_FEA_Guru]

ESPcomposites,

I'd like to hear more about:

- I believe it was discovered the testing methods used to validate the failure criterion were not appropriate.
- Even if the test data was validated, it would only be for a lamina. The extrapolation to the laminate level is suspect at best.

If you have anything a little more concrete on your Tsai-Wu statement above, I'd be interested in learning more about it. For your second statement, I'd be interested in hearing a defense of your statement and what exactly you mean by "extrapolation" to the laminate level? I have always been leery about Tsai-Wu myself and would love to hear some dissenting opinions about it since for most analysts (definitely not me), it is their go-to failure criterion.

Regards,
CompositeModeler

 

[SWComposites]

see this paper:

A comparison of the predictive capabilities of current failure theories for composite laminates, judged against experimental evidence
M.J. Hinton, A.S. Kaddour, P.D. Sodenc
Composites Science and Technology 62 (2002) 1725–1797

the bottom line conclusion:

"7.3. Predicting final strength of multidirectional
laminates (i.e. ultimate failure)
Once again, the ‘exercise’ has shown that the current theories are not sufficiently robust. In the general case, a designer wishing to estimate the stress levels at which ultimate failure might occur in a multi-directional laminate, can, at best, hope for accuracy of +/-50% in the majority of cases."

And Tsai-Wu was not the best performing theory; not that any of them are much good.

SW

 

[ESPcomposites]

I had a brief look, but need to look a little further into the references (I have over 400 papers). But in general, this is quite a challenging topic to get into.

This is one my favorite papers on failure criteria discussion:

Carl Q. Rousseau
A Range of Practical Failure Criteria for Laminated Composites

Reference: Rousseau, C. Q., "A Range of Practical Failure Criteria for Laminated Composites," Composite Materials: Testing and Design, Fourteenth Volume, ASTM STP 1436, C. E. Bakis, Ed., ASTM International, West Conshohocken, PA, 2003.

Tsai-Wu - In this paper the category labeled "Tsai-Wu" includes all lamina-level interactive, or polynomial curve-fit criteria. While possible to formulate these criteria for solid or beam-column stress states, the vast majority of the derivations and applications are specific to in-plane failure in states of plane stress or plane strain. Beyond the advantages and disadvantages listed in Table 4, it is important to put the development and use of this criterion in proper historical perspective. During the 1960's and 1970's the emphasis was on proper ways to homogenize both the elastic response and the failure physics of laminated advanced composites. Traditional approaches used on glass/epoxy structures in the 1950's were to simply assume that the mildly orthotropic glass/epoxy fabric laminates were isotropic, and use very conservative strength allowables without regard to lay-up. Since this approach was unacceptable for highly orthotropic boron/ and carbon/epoxy, and targeted applications were weight- and fracture-critical primary structure, the two most popular failure theories to emerge in the '60's and '70's were (a) stress-based interactive criteria such as Tsai-Wu, which attempted to capture all fiber and matrix failure modes in one failure index (in order to provide the analyst a work-load comparable to what they were accustomed to on isotropic material); and (b) translaminar fracture-based criteria which attempted to parallel the metallic state-of-the-art at that time in LEFM. Since the 1970's increasingly routine applications of carbon/epoxy advanced composites have lead practitioners to gradually become more concerned with (a) correctly separating and capturing the constituent-level failure physics (in lamina- or laminate-level failure criteria); and (b) applying criteria that are as simple and straightforward as possible, in order to ease allowables-development/application cost and regulatory oversight (i.e., explaining your analysis to the government). Thus, use of interactive criteria such as Tsai-Wu, given the disadvantage noted in Table 4, is on the wane.

The point there being is that in the 60's and 70's there was a lot of hope and guessing that these failure criterion would be true predictors. The truth is that it did not work out like that and we still not have a failure model to predict actual failure (though SIFT seems to be gaining popularity).

For item 2:
The major problem with lamina based failure criteria is that actual failure occurs at the laminate level. The complex state of 3D stress and psuedo-plastic type failure that actually occurs (holes and bolted joints), usually render pure lamina based failure criteria questionable. In addition, free edge delamination in unnotched specimens cannot be accounted for. In fact, when dealing with real failure modes for holes/bolts/impact, all of the lamina based failure criteria start to make less sense. At that point, one starts to consider test data and failure models such as W-N (point stress, etc.), which are semi-empirical and by definition cannot capture the actual failure state.

Like I said, this is quite a complex topic, but those are some general thoughts behind my comments. I also have a good graphic (which I can't locate immediately) which shows the use of the different failure criteria in industry. The max-strain is the most popular, mostly for the reasons Carl mentioned.

Brian

http://www.espcomposites.com

 

[Composites_FEA_Guru]

SWComposites/ESPComposites,

Thank you for the references. I'll have to see if I can find a copy and take a look.