Soil Analysis - Model Not Converging

[scudelari]

Hello Everyone,

I am trying to simulate the pressure expected on the soil caused by the Mats of a Crane during its operation. But I am having problem converging and setting the analysis parameters. 

I am using Autodesk Simulation 2013 SP1.

First, the basics of the simulation environment:

- The simulatiuon type is MES with Nonlinear Material Model. The solver is automatic. Default timestep configuration. 

- The soil is composed of several different layers, as follows. The 3D mesh of the soil is always made using layered mesh with 3 layers. I put fixed surface constraints on all of the four sides of the ground. THE BOTTOM SURFACE IS NOT FIXED.

- The material model for the soil is Duncan-Chang with Small Displacements. The material itself was changed simply to comply with the parameters of the soil.

- The Mats were as follows:

- For the mats the simulated detail is as follows:

I cut in the cad software the surfaces to force that the mesh on the soil and that of the mats be vertically aligned. The contact element (which has a lenght of 20mm) was set to lenght of 20mm and a stiffness of 10e10. They are directly connected to each node underneath of the soil.

The metallic plate is a simple linear material model of a metallic material. Its mesh is of plate elements and the formulation os also of plate.

---------------------------------------------------------------------

The model does not converge. As a matter of fact, the analysis doesn't even start (it tries to reduce the time steps but the error is always very high.

I am looking for suggestions on what may be changed in this model to converge.

I can also give more information if necessary.

Thank you so much for any insight.

[zhuangs]

First of all, for nonlinear analysis types, especially for "Static Stress with NLM" and "MES with NLM", "Large displacement" is always recommended, even though the displacement is small in the model.  Since "Large displacement" controls the updates of global stiffness matrix, resulting from any nonlinearity, such as nonlinear material model, contact, etc..

Second, what's the interaction between neighboring parts, "Bonded" or "Surface contact"?  For the figure, the mesh is uniform for all the neighboring parts, and the nodes match.

-Shoubing

[ipaulson]

Hoping to resurrect this thread, as I am dealing with a very similar problem and have had very limited success in getting models to run to completion. 

The problem setup is similar to the OP, but the soil "block" is only one type of soil, modeled using the Duncan-Chang material model (unfortunately, as far as I can tell, the material model does not support large displacement). The soil block is a solid tet mesh with the panel being a surface mesh. Unlike the OP, I do not have a gap between the soil block and panel.

I originally had Bonded Contact between the soil surface and the metal panel, but bonded contact was creating some inaccuracies, so the next step in model complexity was moving to frictional point-surface (auto choice) contact. Solving with bonded contact was working well numerically, but I've had no end of problems since moving to frictional contact. A MES with NLM will start fine, but then hit a wall 30-60% of the way through (100 timesteps), with residuals diverging with timestep reduction. No errors result (other than autolimiting if left to run until completion), so troubleshooting has been difficult.

Should a gap be introduced between the panel and soil?

Can a few highly stressed soil elements scattered around the perimeter of the contact area be the culprit? These hotspots arise much earlier in the run than the timestep where the solving becomes an issue.

Any pointers on using contact with the Duncan Chang soil model would be greatly appreciated.

Thanks. IP.

[John_Holtz]

Hi @ipaulson

I think the question is whether the slow convergence is due to contact, friction, or the soil part. Any or all three can be problematic in the right (or wrong, depending on your viewpoint) situation.

Perhaps you should try the analyses in this order (easies to converge to more difficult):

1. Change the soil to an isotropic material with the same stiffness as the soil's initial stiffness, and frictionless contact with the other part. Does this run to completion? (Or with the changes needed to get it to run)
2. If that runs, change the contact to include friction. Does this run to completion? (Note: if there is some other way to approximate the friction effects, it might be good to use that. For example, can an applied load approximate the friction?)
3. If that runs, change the material to Duncan Chang.

[ipaulson]

Thanks your breaking down the methodology, @John_Holtz . I was able to get the model started by separating the panel and soil by 3mm, initially suspending the panel with weak springs, using S-S contact, a contact length setting of 1mm and interaction distance of 3mm. However, convergence issues persist.

I think the contact aspect is squarely to blame at this point (I’m moved to frictionless contact with lateral springs to keep the panel from flying sideways).  The particular phenomenon that leads to numerical issues is occurring at the edges of the panels as the panels shift around a bit during loading due to soil deformation. Due to client confidentiality I cannot share the model outright, but the panels are not simply rectangular in cross section – one panel, about 12” wide and several feet long, has several segments of its cross-section that are in contact with the soil (think of a bolded “E” turned so that the cross-section of the three legs are in contact with the soil – one body, but multiple flat contact surfaces).

As the panels/soil shift relative to each other under load, it appears that contact elements are being turned off between timesteps leading to sudden changes in load/displacement of soil nodes. One trouble node can be seen in ts27.png before issues start. In one particularly difficult timestep that MES did manage solve, the soil node moves from about 0.6mm below the plate surface (the blue plate elements) to about 1mm above the plate surface, and non-realistically into the plate, as seen in ts28.png.  I’m assuming that two nodes selected in the images were deemed “in contact” in step 27, but not in contact in step 28. Subsequently, this soil node is forced upward as the result of the low Young’s modulus (Drucker-Prager soil model) and nearby soil nodes remaining in contact with the panel which essentially squeezes this problematic node upward. The vertical displacement plot of both nodes is also attached. Note that this run later crashed due to this phenomenon occurring elsewhere - MES was not able to handle the sudden change.

Do you have suggestions on contact settings or other solver setting to avoid this discontinuity? Is this something that can be avoided by increasing mesh density along the edges of the contact surfaces on the soil block that are initially in contact with panel? I’m not particularly concerned with the soil results, I just need to represent deflection of the support beneath the panel.

Thanks. IP

[John_Holtz]

Hi @ipaulson

I can think of a number of possibilities. Here they are in no particular order ...

1. If the node on the soil is a fraction of a mm beyond the panel, then maybe the node is no longer in contact. This would allow it to "pass through" the panel because there is nothing to stop it. Is it possible to move the panel slightly (in the Z direction?) to ensure the nodes do not squeeze by?
2. There are two types of surface contact: point to surface and surface to surface. Point to surface can allow the nodes on one face to pass through the other face, but surface to surface prevents the nodes on both faces from passing through the other. If point to surface was used, switching to surface to surface could help. (Figure 1 on the page Options in the documentation has a diagram that tries to clarify the differences.)
3. Surface contact are springs between the surfaces. If the stiffness of the springs is too low, the nodes can pass through each other. If the penetration is too large, the software assumes there is a problem and "breaks the spring". Increasing the contact stiffness may help in this type of situation. (The link in the article below describes how to find the current stiffness, etc.)

This article provides some general tips that may be helpful: What are some general tips for setting up surface to surface contact for an MES analysis in Simulati...