Modeling tensors

[Onacho]

Hello, I am trying to model tensors in FEMAP with NX Nastran, and I can't figure out how to do it right. The main problem is that I can´t make an element to take tensile loads without taking compression loads as well. I have tried using the property Rod, activating the "cable" option, but it doesn't work. Also, I have been experimenting with the Gap property, but I still can´t achive to make it work properly. I would like to find a solution in the linear field, since my whole model is linear. The only solution I came across with, is runnig an analysis with rod elements and delete all of which are under compression loads, but this model isn't representative for normal modes analysis, so it's useless to me. Any help will be deeply appreciated . Thanks.

Ignacio

 

[Elabbasi]

Dear Ignacio,

There is no linear computational solution to materials that take compressive or tensile loads only. Since there is a change is stiffness (even if between a constant value and zero) the FEA program has to do a nonlinear analysis.

If your loads are such that there is tension everywhere the FEA model should converge easily. If not, then parts in compression may have difficulty converging. You also get convergence difficulties for points that have close to zero load since the program can end up oscillating between two stiffness values. You should use a very small stiffness instead of zero for the compressive stiffness if you can.

The sections under compression will also affect the natural frequencies of the model (compared to removing the elements under compression as you currently do).

Also, one more issue to consider if you are dealing with 2D/3D elements rather than 1D. The difference between a tensile and compressive stress state is harder to define in that case, because it has to be defined based on stress as a tensor quantity. In that case, it's better to use the first stress invariant as a measure of tensile/compression. There is a Nastran material for that, which is MATS1 with TYPE=NLELAST.

I hope this helps.

Nagi Elabbasi
Veryst Engineering

 

[Onacho]

Thank you Nagi, now it's clearer to me that I should run a nonlinear analysis. I will follow your advise and see how this turns out. As soon as I have any result I let you know.

Best regards.

Ignacio Ochoa

 

[ESPcomposites]

In NASTRAN, there is a "linear gap" element as well. This will allow you run a "linear" 101 solution, although I believe it is nonlinear in the background, transparent to you. It may be handy if you want to keep things simple.

I "think", you can reverse it's default direction by modifying the .bdf and setting from a "1" to a "-1" (or something to that effect). I don't know if the pre-processor will support this though. It's been several years since I did this, but thought it was worth mentioning.

Brian

http://www.espcomposites.com