Orthotropic Solid Modeling

kennethfugate

I'm playing around with orthotropic solids and made a simple test model to see where the material constants map into Engineering Constants in the CCX input file. They appear where expected except that the nu12 is mapped twice (nu12 and nu13) and the value for nu13 does not appear. Is this a bug or am I missing something? I've attached the model, the CCX .inp file and the material input dialog.

Victor

There's a difference in the definitions. The Poisson's ratios in CCX are

nu12, nu13, nu23

whereas in Mecway they are

nu12, nu23, nu31

For exporting to .inp, Mecway converts nu31 to nu13 using the formula

nu13 = nu31 * E1 / E3

It's just a surprising coincidence that nu13 = 0.3 * 1/3 = 0.1= nu12 in your test!

Directions 1, 2, 3 correspond to U, V, W as you'd expect.

disla

Hi Victor , Ken

I have read one paper about Poisson's ratio in orthotropic materials which exposes some constrains in between their values.
Now I understand better why there is sometimes a warning when introducing certain combinations of Poisson values. The warning says : “Material Stiffness Matrix is not positive definite. Poisson’s ratios might be too large”.

That paper shows a different relationship between the corresponding symmetric terms.

nu13 = nu31 * E3 / E1

By other hand I do not understand yet which of the criterias are checked. I have found some combinations that should warn the user, but it doesn’t .
Find example.

kennethfugate

Thanks. I was just using numbers to track where they go in the input file. I knew the order was different because of the way the indices are incremented, i.e. 12->13->23 vs. 12->23->31. What I forgot about was the conversion between the mirrored nu values.

Victor

Easy to not notice with such an incredible coincidence occurring! The same thing confused me while I was checking it.

@disla You've run into an even more insidious problem in that there are two different conventions that both use the same name and same notation but transpose the values! Your document and its source use the other convention in which ν_ij = ν_ji in Mecway's convention.

The popularity of each convention seems to have reversed sometime around the 1980s for some reason. The paper your document cites is from 1968 and uses the older convention.

The test Mecway uses for that error message looks at the material stiffness matrix itself, not the individual Poisson's ratios.

kennethfugate

I've been working on modeling honeycomb panels. I've made a comparison model using a detailed core model and one with orthotropic hex elements. I've also included a spreadsheet to compare with an empirical method from the Hexcel report attached. The spreadsheet interpolates the deflection coefficient between all of the 12 curves. I'm sharing this in case anyone is interested in modeling honeycomb and can benefit from the work I've done.

The core modeled is the first on listed for 5056 aluminum in appendix 1. It has a cell size of 1/4 inch and a ribbon thickness of 0.001 inch with a thickness of 0.002 for elements aligned with the ribbon direction from the manufacturing bonding process. The solid hex8 core is modeled using the method in the second pdf. The two FEM models and the empirical calculation give results close to one another.

This work is out of interest and now that I'm retired, I have time to go down these rabbit holes. When I was a stress analyst for F/A-18 aircraft, the model from the late 1970's was very coarse and used a proprietary McDonnell Douglas FEM program named CGSA that ran on a MicroVAX. The honeycomb parts were modeled using membranes and rods for the skins and were around 2 inch square. The shear panels for the core were attached to the skin element nodes and ran in the ribbon and perpendicular directions. The thickness of the shear panels was average of the distance to the next shear panels and had shear properties from the core shear modulus. I knew there had to be a better way to model honeycomb parts given the advances in computers and FEM software. It is amazing how I can run such large models in a few minutes on my laptop where it took many hours to run smaller models back then.

Ken

JohnM

Nice work Ken! I've had to do similar things for simulating the stiffness of fin packs in heat exchangers. It's why it's worth understanding how this stuff actually works :-)
Young engineers today can't imagine that you started your model one line at a time: node, x, y, z (repeat a few hundred times).
My first job was with Lockheed and we used punch cards. Computers were big, processors weak, memory small, run times enormous. Tools like Mecway and Calculix make quick work out of things that would take an order of magnitude longer in the old days!

disla

Thanks for sharing, Ken.
Really nice post.

disla

Hi,

I recently realized that applying symmetry boundary conditions to Orthotropic or Laminated elements couldn’t be safe as it changes the fibers direction, and it is not correct ¿isn't it?.
¿How do we manage this?.

prop_design

My understanding is, for solids, the element orientation is always the global coordinates. So solids are not very useful for composites. For shells, I believe the element orientation is applied by the original definition. Interesting catch on the mirror or rotate etc. I can see that messing things up. You may have to redo your element orientation, after you manipulate the mesh. I don't know that there is a right or wrong way to handle this. If it holds what you originally defined, that would make sense to me. I think it would be a lot harder for the software to know what you had in mind, after you changed the mesh.

disla

Oppps, of course, Cyclic symmetry would show this mess too.
I guess it could be solved orienting the properties orthogonal to the axis of symmetry, but I,m working on some examples with laminates at 0º/+45º/-45º/0º and weird combinations. That’s what remind me this Ken post but his example is and orthotropic core with U V properties being the same, so I think here it’s safe.

prop_design

Experimenting with the laminate orientation is the funnest part of doing composite analysis. The sad thing is, you can't get a good view of the internal layers. So it makes it a bit harder. Sometimes, the open cracks option allows you to see the inner layers a little bit. I have been using 0/+45/90/-45/0 for the most part. My loads are pretty much in the 0 direction. Then I experiment with how many element layers of each. So about two element layers of each works for what I try. I'm not building anything though. It's just FEA for the fun of it. The thing to check is how the weak axis of the composites hold up. They usually pass in the strong direction and fail miserably in the weak direction. There is usually no fatigue data for the weak direction either. So they make the material seem fantastic in the specs, when really, it's awful in actual use. The load direction versus laminate direction is a critical part of making these types of parts work. When fillets are involved, it's impossible to keep loads out of the weak direction. That's where I see these fail all of the time. They usually bond in a metal part in the fillet region as a work around.

Victor

Everything is reflected at symmetry boundary conditions, so fibers at an angle would have a kink along the symmetry line/plane. Yea, probably not useful for general laminates.

disla

Thanks for your comments prop_design and Victor.
I’m doing some validation before proceeding with Calculix/Mecway so I’m not completely free to choose the configuration.
I have clear now that I will avoid symmetry BC for Laminates or Orthotropic elements just in case.
I’m obtaining a big difference between the quarter, the half, and the full plate. I have found now some warnings on the book I’m following even for othogonal fibers 0/90.