Modeling thin plates with solid elements

[ThetaJC]

Hello,

I have a question about modeling thin plates with Solid elements. We typically deal w/ structures which have constituents of the geometry that are flat plates which transition into more traditional 3-D elements (not FE). An example would be a circuit card with a bonded stiffner/heatsink structure. To be competitive we need to quickly access performance and move forward. The need for 3D elements are a must for the heatsink structures. They don't lend themselves to anything but solid elements. However, the circuit card portion of the assembly is for all intents and purposes a flat plate. Due to time constraints, an automatic meshing operations using tetrahedral elements is an attractive approach. However, our FEA guys have warned us to maintain a minimum of 3 element layers across the thickness of the plates if we are going to use Solid elements. I am using Ansys v7.1 w/ Solid 92 elements (element contains midside nodes). My question is, how large of an accuracy hit can I expect modeling the structure if the characteristic element length determined by the automatic mesher creates a mesh that is only 1 element layer thick in the plate portion of the structure if I am performing:

A. A PSD spectrum analyis (g^2/Hz) or
B. A structural analysis with transverse loading (circuit card will bend)

My hope is that since the Solid 92 elements are non-linear, they will have a shot at characterizing the bending. I know that shell elements are preferable, however, I do not have the time to write constraint equations to tie them to the solid elements.

Would appreciate any help,

Thank you,
Courtney

 

[Drej]

One solid92 through thickness with bending will result in your solution being nonsense. If you're only interested in displacement, however, you may get away with it (I wouldn't want to defend it, though!). These tets are very, very stiff, and although excellent to model complicated geometry (and in numbers), in low numbers they will massively overstiffen your structure, in particular if it is subjected to bending.

If it is a PCB you are modelling, there is specialist software available known as FEAP (pronounced "feep&quot. This software is fantastic for modelling PCBs with electrical components - it should be, as this is its primary purpose. Take a look at:

http://www.emrc.com/webpages/feap/feap_4.htm

I understand that time constraints may be vital to you here, hence you may want to think about modelling that PCB with shells. I have carried out PSD analyses before on PCBs using shells. I had to use first order shells (shell63) since with solids (higher order tets solid92) the DOF was ridiculous. For the PSD analysis, I lumped masses (mass21) onto the board where the principal components were. You could also manually modify the density locally to achieve the same effect. If you're not limited so much by DOF, use higher order shells (shell93) or even look at one of the shell18x family (which are very good).

(As a test, you could mesh the board with (1) tets92 and (2) shells63. Check to see how stiff your boards are by running an Eigenvalue analysis and comparing the results. If your frequencies are close together in the range you are interested in (<10% difference), then you should have confidence in the tet mesh. I'll say it again, though, don't use one tet through thickness - use at least three).

On the other hand, if you really have to use shell to solid, you don't have to write the constraint equations manually. This is an automated feature within ANSYS 7.1, and it works beautifully: see the CEINTF command or look at:

Main Menu>Preprocessor>Coupling / Ceqn>Adjacent Regions

which will set it all up for you.

The best of luck,

-- drej --