asdeasoft.net

Hello,

I am building a 3D model of a shaft structure in STKO, which consists of side walls and a base slab. The base slab is modeled using brick elements (solid), while the side walls are modeled using ASDShellQ4 elements (shell). These two parts are connected using the beam-solid coupling constraint.

For the material, I have assigned Concrete01 to the structure. However, I still have some confusion regarding the definition of the structural mass and the application of gravity loads. I would appreciate your advice on this matter.

Finally, I attempted to run a simple static analysis but was unsuccessful. I have attached my model file and would be grateful for some suggestions to help identify the issue.

Thank you for your time and help. I look forward to your reply.

There are some conceptual errors in your model.

The main one is that you are modeling the tube as a shell model, but assigned a beam cross section.
If you want to model it as a shell, then you need to use 3D material models inside a layered cross section, not 1D models inside a fiber cross section (this is for beam elements)

Regarding mass and loads: It really depends on what are you modeling. For example, for mass and self weight of shells, you can assign a Face mass (rho * thickness) and face foce (rho * g * thickness)

STKO Team wrote: ↑

Mon Oct 06, 2025 7:41 am

There are some conceptual errors in your model.

The main one is that you are modeling the tube as a shell model, but assigned a beam cross section.
If you want to model it as a shell, then you need to use 3D material models inside a layered cross section, not 1D models inside a fiber cross section (this is for beam elements)

Regarding mass and loads: It really depends on what are you modeling. For example, for mass and self weight of shells, you can assign a Face mass (rho * thickness) and face foce (rho * g * thickness)

Hello STKO Team,

Thank you very much for your previous reply. It has been truly helpful.

I still have some additional questions that I would like to consult with you about:

1. When modeling the tube using shell elements, I understand a 3D material should be used. I've reviewed some discussions where ASDConcrete3D with LayerShell elements were used for modeling concrete structures. However, those examples all involved solid sections. Would this approach also be suitable for modeling a tube structure like mine?

2. Regarding mass and load application for the shell model: I noticed that the surface mass definition doesn't appear to be reflected in the analysis steps. Therefore, would it be appropriate to directly apply a face force to the shell elements to represent the self-weight? Additionally, for the base slab modeled with brick elements where body force can be custom-defined in the element parameters, does this mean we don't need to apply additional volumeForce to this part?

3. Concerning the connection between the tube (modeled with shell elements) and the base slab (modeled with brick elements): To integrate them into a unified structure, I encountered the "incompatible degrees of freedom at the same node" issue at their interface. Is using the EqualDOF method a reasonable approach to resolve this?

4. When modeling the base slab with brick elements and directly assigning the ASDConcrete3D material, I receive a "failed to create material" error. This occurred when I created a solid model where both the tube and base slab used brick elements during static analysis. I haven't been able to identify the cause of this error.

Thank you once again for your assistance. I would be truly grateful for your further help with these current difficulties.
I look forward to your reply.

1. When modeling the tube using shell elements, I understand a 3D material should be used. I've reviewed some discussions where ASDConcrete3D with LayerShell elements were used for modeling concrete structures. However, those examples all involved solid sections. Would this approach also be suitable for modeling a tube structure like mine?

Sure, if you look at the first webinar where we presented the ASDConcrete3D, it was used in the shell-model of a RC shear wall

2. Regarding mass and load application for the shell model: I noticed that the surface mass definition doesn't appear to be reflected in the analysis steps. Therefore, would it be appropriate to directly apply a face force to the shell elements to represent the self-weight?

In OpenSees loads and masses are not directly connected. If you are doing simply a static analysis, you just need the force.
While if you are doing a dynamic analysis, both are needed (the mass for the inertia effects, and the force for the mechanical effect)

Additionally, for the base slab modeled with brick elements, where body force can be custom-defined in the element parameters, does this mean we don't need to apply additional volumeForce to this part?

For solid elements, you can use both approaches.
But if you use the body force in the element property, it will be applied instantaneously. So it can create problems in dynamic or highly nonlinear problems.
If instead you add it as a volume force, you can put it inside a load pattern with any time series you want. For example, if you use a linear time series, you will apply the body force incrementally.

3. Concerning the connection between the tube (modeled with shell elements) and the base slab (modeled with brick elements): To integrate them into a unified structure, I encountered the "incompatible degrees of freedom at the same node" issue at their interface. Is using the EqualDOF method a reasonable approach to resolve this?

Equal DOF is fine, but it will link only displacements, not rotations. So you will create a hinge at the bottom.
The most accurate way is to define a cut in the solid, so that there is a ring surface under the intersection with the shell mid-plane, whose thickness is equal to the wall thickness.
Then you can use this surface as slave in the master-slave link for the beam-solid-coupling

4. When modeling the base slab with brick elements and directly assigning the ASDConcrete3D material, I receive a "failed to create material" error. This occurred when I created a solid model where both the tube and base slab used brick elements during static analysis. I haven't been able to identify the cause of this error.

This is not clear to me. Could you share the full error message? or the model that generates this error?

Hello STKO team,

Thank you very much for being able to receive your reply again. I would like to express my gratitude to you once more.

Sure, if you look at the first webinar where we presented the ASDConcrete3D, it was used in the shell-model of a RC shear wall

Regarding the content related to the ASDConcrete3D material, I will study it in the webinar.

If instead you add it as a volume force, you can put it inside a load pattern with any time series you want. For example, if you use a linear time series, you will apply the body force incrementally.

I believe I have understood the principle. During dynamic analysis, to better run this model, I should apply volume force (for brick elements) or face force (for shell elements) in the conditions module to represent the self-weight. However, does this approach face a particular issue? This problem mainly arises in the base slab structure because the mesh for this part of the model is not completely uniform. Would the application of volume force (rho * g * V) become complicated in this case? I will attach the cross-section diagram and mesh configuration of the base slab for your reference. (Fig 1 and Fig 2)

The most accurate way is to define a cut in the solid, so that there is a ring surface under the intersection with the shell mid-plane, whose thickness is equal to the wall thickness.
Then you can use this surface as slave in the master-slave link for the beam-solid-coupling

Regarding the connection between the shell and solid models, I am not entirely sure if my understanding is correct. Therefore, I plan to attach a cross-sectional diagram later (Fig 3). The outer and inner rings shown in the diagram represent the solid model below, while the middle ring represents the shell. I intend to apply the beam-solid coupling to the line (shell) - surface (brick) where the two models contact.

This is not clear to me. Could you share the full error message? or the model that generates this error?

There is the issue of my failed attempt to create the ASDConcrete3D material. I still need to learn how to establish the 3D model for the shell element. Therefore, I built a complete solid model and planned to assign the material directly to the solid elements. However, during the run, it showed that this material could not be created. This time, I have attached my model to help you better understand the problems I encountered.

Thank you once again. I look forward to your reply.

I believe I have understood the principle. During dynamic analysis, to better run this model, I should apply volume force (for brick elements) or face force (for shell elements) in the conditions module to represent the self-weight. However, does this approach face a particular issue? This problem mainly arises in the base slab structure because the mesh for this part of the model is not completely uniform. Would the application of volume force (rho * g * V) become complicated in this case? I will attach the cross-section diagram and mesh configuration of the base slab for your reference. (Fig 1 and Fig 2)

Hello STKO team,

Regarding the application of body force (for solid elements) or surface force (for shell elements), I believe I have understood the underlying principle. The set parameters are not applied to each individual element but are automatically distributed to the nodes of the structure. Therefore, I only need to calculate the total mass or self-weight load of the entire structure. I would appreciate it if you could confirm whether my understanding is correct.

However, I still have not found good solutions to the other questions I raised previously and would be grateful for your further assistance.

Thank you once again. I look forward to your reply.

Regarding the application of body force (for solid elements) or surface force (for shell elements), I believe I have understood the underlying principle. The set parameters are not applied to each individual element but are automatically distributed to the nodes of the structure. Therefore, I only need to calculate the total mass or self-weight load of the entire structure. I would appreciate it if you could confirm whether my understanding is correct.

Correct

However, I still have not found good solutions to the other questions I raised previously and would be grateful for your further assistance.

Here are 2 models, one for full solid, and one for solid shell. You can see the way I applied the interaction. Note: that interaction requires a penalty constraint handler. I use the Auto handler (recently developed by us to automate the calculation of penalty coefficients)

Regarding the error about the ASDConcrete3D, make sure to have the latest version of OpenSees.

Hello STKO team,

Thank you very much for your continued support. I would like to express my sincere gratitude once again. I'm truly glad to have your assistance in resolving the difficulties I've encountered. Whether it's about applying structural loads or implementing connection methods, I believe that through continued practice, I will be able to master these techniques in the near future.

For the structure we previously discussed, I plan to analyze its response when embedded underground. This inevitably requires modeling the interaction between the structure and the surrounding soil. Currently, I'm using the zeroLengthContactASDimplex element for the soil-structure interaction, and I intend to apply this approach to both the model containing shell elements and the fully solid model. I would like to know if this method requires any further adjustments or improvements.

Regarding the error about the ASDConcrete3D, make sure to have the latest version of OpenSees.

I plan to update my OpenSees version. Based on my understanding, I should be able to download the latest version directly from the STKO website. However, I seem to be unable to download OpenSees option 1. Could you please provide a relevant link to assist me with this?

Thank you once again for your help. I look forward to your reply.

Hello STKO team,

My apologies for disturbing you again.

I plan to update my OpenSees version. Based on my understanding, I should be able to download the latest version directly from the STKO website. However, I seem to be unable to download OpenSees option 1. Could you please provide a relevant link to assist me with this?

I have resolved the previous issue and found the method to download the latest version of OpenSees solvers.

Recently, I have built an integrated model that includes both the soil and the solid structural model. The connection between them is still established using the zeroLengthContactASDimplex method. However, I encountered certain issues during the execution. I will attach the model file and would be extremely grateful if you could help analyze the potential problems.

Thank you once again. I look forward to your reply.

Dear STKO Team,

I hope this message finds you well.

I am writing to follow up on my previous communication regarding some challenges I've encountered while building an integrated soil-structure model. I understand you are very busy, so I truly appreciate you taking the time to read this.

Recently, I have built an integrated model that includes both the soil and the solid structural model. The connection between them is still established using the zeroLengthContactASDimplex method. However, I encountered certain issues during the execution. I will attach the model file and would be extremely grateful if you could help analyze the potential problems.

The issue has persisted for some time now, and despite my continued efforts, I have been unable to identify a solution on my own.

While awaiting your reply, I have been actively exploring alternative approaches. I attempted to build a shell model, but unfortunately, the analysis still did not run successfully. As this is my first time working with shell models, there may have been operational errors in the process, and I would greatly appreciate your guidance to help refine this model.

Additionally, during the construction of the shell model, I used the beam-solid coupling method to connect the structural components. However, when I created the 3D soil element, the coupling markers unexpectedly disappeared from the view. I am uncertain whether this was caused by an operational mistake on my part.

To summarize, during this period I have experimented with two different approaches - a solid model and a shell model - but unfortunately, neither has yielded successful results. These issues have indeed been troubling me for quite some time, and I sincerely hope I can resolve them with your assistance.

I have attached the shell model file for your reference.

Thank you for your time and consideration. Any advice you could offer would be greatly appreciated.