transverse shear stress distribution in composite laminates?? 1

[kevin2002]

Hi,

I have created a 4-ply (30/30)s composite laminated model in Abaqus using layers of 20-noded brick elements and the model was subjected to uniform pressure at the bottom surface. But, the resulting transverse shear stress distribution TaoXZ is not what I'm expecting. The figures below illustrate them where 0 indicates the point of zero stresses.

0 (expected) 0 (resulting)
__
\ /
\__ /_____
\ __/ _____/
/ __/
The material properties is defined using anisotropic type, so the stresses will be plotted in the global direction. I have double checked their definition and there is no problem with this. Also the stresses is plotted at the centre line of the 3D laminated plate and they are many times the width away from discontinuies, e.g fixed end, and sufficiently far away from free edges. So i will expect the stress should decay to what can be determined using lamination theories or equilibrium equations, i.e. the expected stress distribution should be as shown above.

Is that something regarding interlaminar effects that ideal lamination theories have neglected? Any suggestion by someone with expertise in this area is greatly appreciated. Thank you.

Kevin

 

[idly123]

I belive at the simply suppoter boundary condiions along plate edges u have forgotton to make the shear terms to zero. just check back the bondary conditions at x=0, x=a. and at y=a, y=b. where a and b ar e the plate dimensions. (incase u are modelling a full plae)
raj Raj

 

[GJS]

Kevin,

This very problem is discussed in the ABAQUS Benchmark manual, section 1.1.3 of the V. 6.2 documentation. Results for inplane stresses and tranverse shear stresses are compared for solid and shell models..... the same trend that you show in your orignal message is also reflected in these results. I haven't read it fully, but summarising.... You will get better agreement with the solid model if you discretise each layer of material with more elements, but its never going to be a brilliant result - the shell model gives very good agreement with laminate theory for the transverse shear stresses. However, the solid model will give better in-plane stress results than the shell model.

Discussions of the results, with graphs and how the element formulation causes the problems are given, along with the decks used for the examples. Hope this helps.

GJS

 

[kevin2002]

GJS,

I see what you have suggested. But, the laminate thickness is modelled using a stack of brick elements, each of which with different material properties, rather than using the option "*Solid Section, Composite". So the manner of solid modelling is actually different from what is in the ABAQUS Benchmark manual. Isn't it then there will be a difference? Thanks!

Kevin

 

[GJS]

Hi kevin,

I've spent a happy aftenoon running test jobs, as I missed the point of your orignal post slightly! I'm getting the same results as you, so went back to basics, using a three layer composite of isotropic materials, the central layer having a stiffness 1/10 of the outer 'plies'.

If I use a shell element with a shell section of type=composite, I get good results..... the same happens if I use a three layers of solid elements, each with seperate isotropic materials.... however, if I try the same test with a single thickness of solids, of the same type as before, with the same materials propeties, but with the element properties built up using a solid section of type=composite, I get the same spurious result as you describe in your original post. I cant see a good reason why the three nominally similar models should give anything but similar results (accepting the surface shear stresses not disappearing on the solids), especially as the composite shell and the fully isotropic layered solid model are in such good agreement.......

This might be something to pass back to HKS so they can provide an explanation.

Very confused....

GJS

 

[FeaGuru]

I think the problem is in the formulation of the elements. You see, according to classical laminate theory, you assume that the shear strains are zero. Of course that is not true. You have to include additional theory in order to account for this. If you have the composites lecture (can order from ABAQUS) it goes into this. I suspect the latter element you are using does not use a formulation that develops proper shear stresses through the thickness or you are not using enough nodes through the thickness.

 

[vonlueke]

kevin2002: How many layers of brick elements are you using to model your 4-ply laminate? I'd tend to agree with FeaGuru's suggestion. You might not be using enough layers; however, GJS seems to indicate only three layers of bricks for his 3-ply laminate gave good results (?).

Also, based on GJS's research, it sounds like the Abaqus section type=composite feature might be defective for solid elements (?). So perhaps consider avoiding section type=composite when you have solids.

Try more layers of bricks, with orthotropic (anisotropic) material properties assigned. And please let us know the outcome, including how many layers of bricks you had before and after, as several of us are interested to know the best way to model a laminate using bricks. Thanks.

 

[vonlueke]

Also I think we should say, avoid trying to model an entire cross section in bending with only one layer of bricks. I in fact try to have at least four elements through the thickness of any isotropic feature in which I want to capture bending. Any less than this can have difficulty accurately describing the deformation pattern, resulting in errant results.

As for nonhomogeneous cross sections, the above rule of thumb would, if anything, be increased further, not decreased, either by increasing the number of elements through the thickness or perhaps by increasing element order. (And of course try to keep your element aspect ratio down as you increase the number of layers.)

So one of the decisive questions is perhaps, what is the minimum number of brick layers required for kevin2002's 4-ply laminate using 20-node bricks? And same question using 8-node bricks? And does he need to use more than four layers of 20-node bricks if he wants to try to approximate the detailed stress distribution as you approach a lamina interface?

 

[GJS]

All,

I think vonleuke is heading towards the crux of the problem here.....

Using shell elements appears to be fine with type=composite, but the in-plane stresses my be slightly off....

Using solid elements with type=composites gives shear stress representation no better than a hand calc, but the in-plane stress results are likely to be good.....

Hence the only option left is to model each ply with many elements through-the-thickness to capture a complete picture of the response of the structure in one go.

For my test jobs, I've been using 4 elements through the thickness which, as vonleuke is about as low as I would like to go... so for a large 3D compsosite structures with even a moderately thick laminate, the number of elements required will be impractical.

All of this makes me quite worried that the limitations of the type=composite for solid elements aren't discussed in the main ABAQUS manual and is confined to the benchmark manual. The type=composite option for the solid elements will, in most cases, provides the only practical way to run a full 3D model - but the results may not be what the unsupecting user is expecting.

Still confused (and slightly frustrated now!), hence a few more test jobs are required.... but REAL work might get in the way ;-)

GJS

 

[kevin2002]

Hi all,

I'm not sure whether it is something to do with the discretization error. My previous model has two brick elements per layer, so there was altogether 8 elements through the thickness. I refined my model with 3 elements per layer, i.e. 12 elements through the thickness. But the outcome did not differ much.

I'm wondering whether the expecting stress distribution (as shown above) is the ideal case, meaning it is not the exact distribution?

kevin

 

[GJS]

Kevin,

If you are defining the SOLID SECTION with TYPE=COMPOSITE, I dont believe it will make any difference how many elements you put through the thickness. It would appear that ABAQUS applies the TYPE=COMPOSITE according to classical laminate theory, and therfore assumes no shear transfer between plies - the shear stress output for each 'ply' is the shear generated due to the calculated deflection of THAT layer assuming no shear stress transfer from layer to layer (thats my understanding - shoot me down anyone....).

The better way to apply material properties would appear to be to define the 3D elastic properties as separate materials (rotated accoordingly for the relevant ply orientations) then apply these material to the elements representing each layer, bypassing the need for TYPE=COMPOSITE. In this way, increasing discretization through the thickness of each layer should improve results, plus the shear distribution should be more realsitic.

We then go back to vonlueke's query as to many elements will be sufficient for each ply, so if you could test out a few models........

GJS

 

[kevin2002]

GJS,

I was not using type=composite. At all times, I'm using layers of brick elements with differing material properties.

kevin