mesh type related error

[Rania. Ah]

Dear STKO team,
An error happens while creating input files, this error is related to mesh type.
The model consists of line elements for building and solid elements for soil domain and foundation.
I would be most grateful if you could illustrate how to fix this error.
Regards,
Rania

[STKO Team]

It means that you assigned a wrong Element Property (with 5 nodes, what element is that?) to an Edge (mesh with 2 nodes).
This happens when you use the sub-selection and erroneously select the boundary edges of a face or of a solid.

Can your share your SCD file? (Zipped)

[Rania. Ah]

Dear STKO team,
The file is attached.
I would be most grateful if you could resolve the issue.
Yours Faithfully,
Rania

[STKO Team]

The error means that you assigned an element property that expects 5 nodes to a mesh that has 2 nodes.
The SimpleContact3D required 5 nodes, 4 from the face of an hexaedron, and 1 that should be in contact with it. So your interaction should have been a node-to-element, not a node-to-node. The node-to-node is always a 2-node link.

In order to keep the interaction as is, I changed the element type to ZeroLengthImplexContact. It is a new contact element that we recently added (and it is available in your OpenSees if you downloaded the OpenSees-Solvers from prof.Tarques website, otherwise you can use the standard ZeroLength Contact)

The advantage of the implex one is that, if you choose the -implex option, the contact element will be always convergent, but requires small time-step.

Another problem that I've seen is that you are using a linear system. This is fine only with linear model, not in your case

Rania_ItalyBuilding_Soil_03062021.zip

(3.35 MiB) Downloaded 305 times

[Rania. Ah]

Dear STKO Team,
That’s great, thank you very much for your prompt reply and help.
Please, could I ask you some questions?
1. Which type of these two interfaces is faster to analyze?
2. For the small time-step, dt of earthquake has been used for the last transient analysis. However, very large time steps have been used for gravity analyses which are conducted as transient. Should I change the type of gravity analyses from transient to static?
3. Mumps system and Krylov-Newton algorithm have been used for all analyses, is that right? (openseesmp solver will be used).
4. EqualDOF or rigidLink constraint should be used to connect the top and bottom faces of mat foundation? The lateral faces of mat are connected using EqualDOFs, is that right?
5. What is the correct order of Analysis steps for using InitialStateAnalysis and updateMaterialStage together?
6. Should any masses be assigned to the soil and structure? Loads are assigned to frames by eleLoad_beamUniform, and by body force b3 in the SSPbrick elements definition for soil and foundation in addition to mass density for material definitions.
7. For the force time history applied to the base of the soil, is it correct to use a unit area of the soil column to calculate damping coefficient regardless of mesh size? (biased mesh is used).
8. Is rayleigh damping necessary in my case? If it is necessary, is rayleigh damping of soil enough (using frequencies 0.2 and 20 Hz)? Or should I enter it separately for both the building and the soil using region command?
There is an ERROR: the analysis did not converge.
The file that contains modifications to the analyses is attached.
Regards,
Rania

[STKO Team]

2. For the small time-step, dt of earthquake has been used for the last transient analysis. However, very large time steps have been used for gravity analyses which are conducted as transient. Should I change the type of gravity analysis from transient to static?

You can turn them to static. But sometimes you can't, for example when you use U-P mixed elements for soils. In case you use transient analysis for quasi-static problems, you can use very large time steps so that inertia effects are negligible.

3. Mumps system and Krylov-Newton algorithm have been used for all analyses, is that right? (openseesmp solver will be used).

Krylov-Newton is just more stable than standard Newton. Mumps is much faster than other solvers, but it is available only in OpenSeesMP/SP, that's why I used it.

4. EqualDOF or rigidLink constraint should be used to connect the top and bottom faces of mat foundation? The lateral faces of mat are connected using EqualDOFs, is that right?

No.
You have to use beamToSolidCoupling to connect the columns to the foundation.
You don't need EquaDOF at the link foundation-soil, otherwise you are simulating a perfect adherence. I noticed that you are using both contact and equalDOF at the interaction between foundation-sides and soil. Doing so your foundation will be attached to the soil, and the contact will be useless. Using only contact is more realistic.
However, you should also do the same at the interaction between the bottom-face of the foundation, otherwise, your structure will penetrate the soil.

5. What is the correct order of Analysis steps for using InitialStateAnalysis and updateMaterialStage together?

There is not a unique way.. It really depends on what you want to simulate. Typically you do:
1) initial state on
2) gravity elastic
3) turn to plastic
3) initia state off
4) dynamic analysis
So that you will see displacements relative to the gravitational ones.

6. Should any masses be assigned to the soil and structure? Loads are assigned to frames by eleLoad_beamUniform, and by body force b3 in the SSPbrick elements definition for soil and foundation in addition to mass density for material definitions.

Yes, you need to assign mass-per-unit-length to the beams, either in the beam element property or using the condition.EdgeMass

7. For the force time history applied to the base of the soil, is it correct to use a unit area of the soil column to calculate damping coefficient regardless of mesh size? (biased mesh is used).

Yes, if you use a FaceForce, it is supposed to be a force-per-unit-area (Pressure), and STKO will take care of converting it into equivalent nodal loads.

8. Is rayleigh damping necessary in my case? If it is necessary, is rayleigh damping of soil enough (using frequencies 0.2 and 20 Hz)? Or should I enter it separately for both the building and the soil using region command?

It depends... since you never model all the physical nonlinearities, you may need artificial damping. And you should do it with regions if the damping coefficients are different for soil and structure.

here is an ERROR: the analysis did not converge.

Try to do the changes I suggested for the connection between foundation and soil, and let's see what happens

[Rania. Ah]

Dear STKO Team,
I would like to thank you for your assistance and guidance, and to tell you that analysis run and complete successfully after doing the modifications.
Please, could I ask you about the penetration between lateral sides of foundation and surrounding soil? When the magnitude of acceleration is displayed together with displacement for deformation, there is no penetration. However, the left side of foundation penetrate the soil when acceleration is used for deformation. Illustrated figures are attached. Therefore, is there any penetration or not?

No.
You have to use beamToSolidCoupling to connect the columns to the foundation.
You don't need EquaDOF at the link foundation-soil, otherwise you are simulating a perfect adherence. I noticed that you are using both contact and equalDOF at the interaction between foundation-sides and soil. Doing so your foundation will be attached to the soil, and the contact will be useless. Using only contact is more realistic.
However, you should also do the same at the interaction between the bottom-face of the foundation, otherwise, your structure will penetrate the soil.

That’s what I did exactly; I used beamToSolidCoupling to connect the bases of columns to the top faces of foundation.
I did not use EquaDOF at the link foundation-soil, I used it only between all the faces of foundation to confirm the rigid behavior of mat foundation. Anyway, I have deleted them and the foundation behaved more realistic.
You are right, I missed to connect between the bottom-face of the foundation and soil! I have fixed this error.

It depends... since you never model all the physical nonlinearities, you may need artificial damping. And you should do it with regions if the damping coefficients are different for soil and structure.

I have used the frequencies (f1, f4) of the first two modes in the X direction of the fixed structure (using ETABS) to calculate Rayleigh damping for structure and foundation.
I have used the frequencies 0.2 and 20 Hz to calculate Rayleigh damping for soil.
Please, could you tell me if you have any notice or correction for these chosen frequencies? Could you suggest a reference to get a benefit?

Thank you again. I really appreciate your guidance and efforts.
Yours Faithfully,
Rania

[STKO Team]

I would like to thank you for your assistance and guidance, and to tell you that analysis run and complete successfully after doing the modifications.

You're welcome

Please, could I ask you about the penetration between lateral sides of foundation and surrounding soil? When the magnitude of acceleration is displayed together with displacement for deformation, there is no penetration. However, the left side of foundation penetrate the soil when acceleration is used for deformation.

It makes perfect sense. Penetration is related to displacement (not velocity nor acceleration). A simple example is a contact between 2 nodes: Node_1 (at position X = 0) is fixed, so its displacement Ux(t) = Ux(t+dt) = 0, and therefore its first and second derivatives with respect to time are both 0 (velocity and acceleration). Node_2 (at position X = 1) has Ux(t) = 0 and Ux(t+dt) = -1 (displacement at which contact happens), so its velocity is not zero, but -1/dt.

have used the frequencies (f1, f4) of the first two modes in the X direction of the fixed structure (using ETABS) to calculate Rayleigh damping for structure and foundation.
I have used the frequencies 0.2 and 20 Hz to calculate Rayleigh damping for soil.
Please, could you tell me if you have any notice or correction for these chosen frequencies? Could you suggest a reference to get a benefit?

Here is a reference about damping (rayleigh and numerical damping) for soils:
https://geotechsimulation.com/2018/04/0 ... -analysis/

[[email protected]]

Dear STKO,

I have had the same issue with one of my models a few weeks ago (since abandoned). But now that I see this post I would like to do some forensics on this model to learn from my mistakes. I tried to double check my mesh and element assignments today but I still couldn't get this issue to go away. My message says I need 8 nodes (as I assigned sspBrick) but I have 4 nodes (which would mean a quad element I suppose). However, my mesh is supposed to consist of solids only.
I'd be grateful if you could pinpoint the mistake in the model for me. I have attached the scd file.

Thank you in advance!
Bence

[marafini.f]

Dear bence,
you assigned you element to all the subgeometries in your solids, faces, edges and nodes. You can simply unassign it and re-assign it by selecting only the solids. You can use the quick toolbar selection tools to operate a restrincted selections or open the specific geometry tree, right click on the solids, select.
Best,
Francesca