the "NX Nastran 10 Advanced Nonlinear Theory and Modeling Guide" says, that it is possible to define different elastic modulus in tension and compression direction for volume elements.
There it says:
3.3 Nonlinear elastic material model
• Advanced Nonlinear Solution supports the nonlinear elastic
material for the rod, 2-D solid, 3-D solid and shell elements. The
nonlinear effect is obtained with a MATS1 entry which has
TYPE = ‘NELAST’. The formulations used for the rod element are
slightly different (and simpler) and are detailed in Section 3.3.1.
• This material uses a nonlinear elastic uniaxial stress-strain data
input in tabular form and shown in Fig. 3.3-1. This material is not
based on the classical theory of finite elasticity, and is not intended
for large strain analysis. However, it is a useful material model
when used appropriately, and with awareness of its limitations.
How and where in NX do I define that?
I think that I know waht are you are looking for:
In FEM file: Menu --> Tools --> Materials --> Manage materials:
Good luck !
thank you for your hint. I got it to work and will post more detailed about this later when I found out more. Right now I have to tell you (and SIEMENS by the way) that this one was hard to find because of serious mistranslation.
PLASTIC in the meaning of nonlinear behaviour of the material would be "plastisch" in German, allthough an "entry" wouldn't have to be translated at all (notice also the change from TYPE to TYP). When PLASTIC was translated, they translated it in the meaning of synthetic material which is "Kunststoff". So when I opened the "Stress-Strain Related Properties", where I was suspecting the things I was looking for, I read "Kunststoff" which I didn't connect to nonlinear behavior right away.
Anyhow, I created a material which has half the modulus in compression than in tension direction. It worked out as you can see in the shiftig of the neutral axis in the bending of a beam.
neutral axis in the middle
neutral axis shifted
I am exploring NX laminates by doing exercises from Mallick Fibre reinforced composites.
Does this also work with orthotropic materials and with different Poisson s ratios under tension and
I can create a stress strain relation, but I don't know to which Youngs modulus this points out to.
I tried to create a table outside the manage material option, with the appropriate values.
But this table does not show up when I want to select an existing field when modifying the Youngs modulus.
It seems that I can only add a temperature dependent field in the manage material options.
In the added figure are the values I want to use in the material/strength definition.
Thanks for your time.
I promised to explain how I got it to work:
1. You need to select NLELAST in the "Type of Nonlinearity (TYPE)"
2. The first positive pair of stress and strain in the Table that you find under "Stress-Strain (H)" has to match the "Young's Modulus (E)". I tried this, if it doesn't match, the Solver won't convergate or has big problems.
3. You have to use a nonlinear Solver at least 106! I didn't try the other yet, but if you use 101 the Solver will only use the "Young's Modulus (E)".
What late for trying, the problem is Laminates are orthotropic.
For the E1 modulus I got:
I want the same for the E2 modulus. But I can not find it.
I played around with the new field ar the E2 modulus, but I can
only selct a temperature dependence
However I find this strange because Carbon fibers or laminates have often different tension/compression
values even for the poisson ratio.
Am i overlooking something??????
Thanks for your time.
There is no way to define a different modulus in tension and in compression for an ortho material.
I would suggest running the simulation twice, once with the tensile properties and then with the compressive ones.
I should clarify my answer.
I would be to create 2 solutions in the same sim, one for each each set of properties. So one solution simulates the structure with the tensile elastic properties, the other with the compressive properties. The actual behavior is in between these two.
I hope this is clear.