Learning Forum

[Joerg]

Hello,

I am using LS Dyna Workbench 2024R1. I have a 35m deep soil column, modelled with 35 x 1m solid elements, which I want to initialize for gravity load. The screenshot for the MAT_079 command snippet is below. I have calibrated the pressure dependency parameters b, a0, a1, a2 based on a target Vs profile and friction angle. I have run a gravity load analysis of the same column with a linear material model, and am using the stresses and strains from that as initial condition for the nonlinear gravity run. For some reason it appears that the program does not adjust the stiffness and strength properties with increasing pressure. The results I am getting are aligned with what I would expect based on the reference input shear stress vs shear strain curve (which is at 3.5m depth). When I assign a separate material to each element (35 separate parts) and give every material the stress strain curve as input that I calculate by hand based on my input parameters (b,a0,a1,a2), then the model works as I would expect. I also tried varying the PINIT parameter to vary between pressure and vertical stress (my model is restrained in both horizontal directions, only vertical strains), but it made no difference. I did consider this in my hand calculations.

Hoping anybody can help me find out why the pressure dependency doesn't seem to work. I thought the strains that I give with the *INITIAL STRAIN card should determine the pressure, based on which the shear stress - strain curve is adjusted automatically.

Thanks.

 

[Joerg]

Here is the screenshot

[Pedram Samadian]

Hi Joerg,

When using pressure-dependent properties (e.g. A2>0 and/or B>0) in *MAT_79, you need to define the initial stresses. The soil stresses can be initialized using *INITIAL_STRESS_DEPTH or by doing a pre-analysis to obtain the *INITIAL_STRESS_SOLID cards in a dynain file. The pre-analysis would have gravity ramped up slowly from zero to its full value. 

I hope this information helps.

Pedram

[Joerg]

Hello Pedram and thanks for the response. I am using the *INITIAL_STRESS_SOLID and *INITIAL_STRAIN_SOLID out of a dynain filr from a gravity analysis of the same model with linear material. What seems to happen based on the results I get is that the program takes the initial strain (converts to shear strain) and looks up the corresponding shear stress from the reference input curve, but does not scale it first. In my example I have given the reference shear strain vs stress curve for a shallow element (3.5m depth). At the bottom element (35m depth) I still only get the maximum shear stress per input reference curve. The vertical stress is correct, but it seems to adjust the horizontal stresses such that the shear stress is satisfied (I can confirm this by hand calculating the stress based on the formulas given in the manual for MAT_079). When I switch the reference input curve to the values I calculate by hand for the 35m deep element, then I get the correct stress distribution (vertical, horizontal, shear).

Any idea what the reason could be that the program does not seem to scale the reference shear stress-strain curve based on the initial pressure (given by *INITIAL_STRAIN_SOLID) ?

[Pedram Samadian]

Hi Joerg,

You are welcome. I contacted one of the developers about this and he said "Doing the initial analysis using elastic material is not a good idea as it would not capture the relevant history variable values. Also, recommended practice is to use separate material properties for different layers, and not use B etc."

I hope this addresses your concern.

Thanks,

Pedram

[Joerg]

Thanks for the follow up Pedram. I switched to using separate layers as recommended.

[Pedram Samadian]

No problem. Good luck.