Copying Part of the Model from One Model to Another

[kolozvari]

Hello,

I have a model of the soil with a simplified superstructure in one model and a detailed model of a superstructure in another model. I was wondering if there is an easy way to copy/import model of the superstructure from one model to another model with the soil domain? If yes, is there any good example on how to do this.

Please let me know.

Thank you

[STKO Team]

Dear Kristijan,

Merging 2 STKO's files completely (geometries, materials, elements and so on) is not yet supported, even though we are working on it.

What you can do now is to Export the geometry of one file and import it to another. However, this works only for the CAD Geometry itself. You lose the physical and element property assignments and the conditions as well.
So, I would recommend you to:

• pick the least complex model (in terms of materials/sections/boundary conditions) (probably is the soil model)
• Select only the geometries you want to export
• Click the "Export" command in the Geometry Tab. Choose BRep or Step as output format
• Open the most complex model
• Click the "Import" command to import the previously generate CAD file
• Re-create the materials/elements/conditions of the imported geometry

[kolozvari]

Thank you for quick response. This worked pretty easily.

Now that I have imported my model of the structure and the soil, I have 2 follow up questions:
1) Please see first screenshot. I believe I need to split geometries of the foundation block to connect the core walls. Please confirm. If so, how do I do this in the most effective way? I would like to try to avoid splitting the entire sol domain. Is there any constraints that can be applied so I only need to split the foundation block as indicated?
2) please see second screenshot. There is a number of gravity columns around on the perimeter of the foundation. They all need to have beam to solid interaction to be connected to the foundation, in my understanding. Is there any issues with constraining so many columns to one solid geometry, i.e., with creating many beam-solid interaction that have all the same master solid? I currently have defined only one in the middle of the building as indicated in the screenshot.

Looking forward to hearing from you. Thank you.

[STKO Team]

1) Please see first screenshot. I believe I need to split geometries of the foundation block to connect the core walls. Please confirm. If so, how do I do this in the most effective way? I would like to try to avoid splitting the entire sol domain. Is there any constraints that can be applied so I only need to split the foundation block as indicated?

If you don't want to split your soil or foundation geometry, please see the answer to the next question

2) please see second screenshot. There is a number of gravity columns around on the perimeter of the foundation. They all need to have beam to solid interaction to be connected to the foundation, in my understanding. Is there any issues with constraining so many columns to one solid geometry, i.e., with creating many beam-solid interaction that have all the same master solid? I currently have defined only one in the middle of the building as indicated in the screenshot.

The beam-to-solid coupling has the beam as master and the face of the soild as slave. So it makes the face of the solid fully rigid (as the "fictitious" cross section of the beam). This is fine if you split the foundation in many sub-faces, so that each column has a small sub-face under its master node, that coincides with the cross-section.
Otherwise, as in your case, the full foundation will be a rigid block.

An alternative is to use the ASDEmbeddedNodeElement. It's typically used to "embed" a node inside an element (as rebars inside concrete volumes). But the same theory can be used to create a "tie" condition between two incompatible meshes.

The difference is that now the beams' end-node and the walls' base-edge are the SLAVE, and the foundation Solid is the MASTER. Therefore you don't add any stiffness to the foundation, while the slave nodes are constrained to move "as if they were attached to the master element".

Look at this example file:

Embed-tie-example.zip

(126.04 KiB) Downloaded 208 times

This is the node-to-element condition for the Embed constraint:

embed-tie-1.png (114.3 KiB) Viewed 4682 times

And this is what you can obtain. As you can see, even if the meshes are incompatible, they move as if they were connected.

embed-tie.png (184.97 KiB) Viewed 4682 times

Note: pay attantion to the stiffness parameter of the ASDEmbeddedNodeElement (read the description)

[kolozvari]

Thank you for the information.

I have added the ASDEmbeddedNodeElement to connect my walls and a column to the foundation block, but after doing so the model doesn't converge for the gravity load. Please note that I have also added rigid diaphragm at all floors that connect the central dummy column that has masses to the RC core wall elements. I have spent a couple of hours checking the model, but I cant find anything that is off. I was wondering if you can please take a look at the model and let me know what needs to be fixed (model is attached).

Another question on a separate note, can you please verify that I connected the coupling beams and the walls correctly? I am not sure if there is a drill DOF at the wall elements so I am not sure if the moment from the coupling beams will be transferred into the walls.

Thank you very much.

[STKO Team]

There were few issues that were giving the singularity of the model:

• When you created the interaction for the embed condition, you erroneously selected some entities from the soil domain

  

  CK_embed_err_1.png (394.74 KiB) Viewed 4610 times

• I understand that the central dummy column is used for generating the Central node (with mass) for each floor. These nodes are used in the RigidDiaphragms. You used a dummy column section to put some stiffness to the 3 DOFs not involved in the Rigid Diaphragm (Uz, Rx, Ry).
  This is fine to give inter-element stiffness, but the whole stick still has 3 rigid body modes (Uz, Rx, Ry) as a whole body, because it is not connected to anything in these DOFs.
  I simply removed the "Stick" physical property and element property. In this way, STKO will only generate the Nodes, but NOT THE DUMMY ELEMENTS (you don't need them). Now you have to fix the 3 out of plane DOFs with a simple FIX

  

  CK_floor_master_nodes.png (88.3 KiB) Viewed 4610 times

• The layout of the diaphragm is wrong.
  The stick nodes should be the masters, and the wall edges should be the slaves (note: all the edges, not only the 2 corner vertices, otherwise the wall will be connected to the diaphragm only at the corner nodes)

  

  CK_diaphragm_error.png (168.29 KiB) Viewed 4610 times

• Some walls were missing physical and element properties, so STKO did not generate elements for them, thus the singularity

  

  CK_missing_elements.png (124.76 KiB) Viewed 4610 times

• Finally the contact local axes in the -Y direction did not have the local-Z axis pointing to the -Y global direction

  

  CK_local_axes_Y-.png (113.94 KiB) Viewed 4610 times

With these fixes, the model runs fine. Now you may want to use the concept of staged-analysis and using the initial state analysis to first apply the self-weight of the soil, then reset the displacements to zero keeping the stresses at the solid elements (initial state analysis).
Then you can add the superstructure and go on with the analysis, otherwise, you will see this delta displacement which is not real, since the structure is built when the soil is already settled.

CK_out.png (181.95 KiB) Viewed 4610 times

[kolozvari]

Thank you very much! Can you please remove the file you uploaded from the forum?

I will study your explanations and try to learn from it.

Best regards.

[STKO Team]

You're welcome

[kolozvari]

Hello, I have a follow up question on this thread. After running the model and observing the deformed shape (see screenshot), it appears that beams do not transfer any moments into the walls, i.e., they are pin-connected to the walls. I didn't do any detailed force-based check, but according to the deformed shape, beams don't bend at all.

Do I need to do anything extra to enable transfer of the moments? In my understanding ShellDKGQ elements used for walls have the drill DOFs, so there must be something with the beam-to-wall connectivity.

Please let me know your thoughts.

Thank you.

[STKO Team]

Do I need to do anything extra to enable transfer of the moments? In my understanding ShellDKGQ elements used for walls have the drill DOFs, so there must be something with the beam-to-wall connectivity.

The fact that the Drilling DOF can be used to successfully link a beam to a shell is something that I've seen a lot in literature, but it is not completely true.

For sure it avoids a singularity (in old-school shell elements without Drilling DOF). But the Drilling stiffness is not sufficient to give the exact result of a beam connected to a shell.
This happens for 2 main reasons:

• The drilling DOF is somehow related to the Cosserat theory in a simplified fashion. The Drilling stiffness is a measure of how much the independent rotation field (rotation about the local Z axis of the shell in this case) can differ from the rigid body rotation of the element (SKEW(GRAD(U)). So it does not coincide with the rigid rotation of the edge to which the beam is attached
• The beam is connected to a single point, while the real beam should be attached to a zone that has the true physical size of the beam cross-section, so that this entire zone is rigid, exactly as the beam section following the assumption of planar sections

Here's a simple file that explains this:

model.zip

(170.55 KiB) Downloaded 216 times

This is the result you obtain:
Solid (LEFT), Shell+Beam+RigidLink (Center), Shell+Beam Only (Right)

drilling_1.png (81.05 KiB) Viewed 4587 times

As you can see, the beam seems pinned but it's not:
it can transfer the moment to the shell, but It's the shell which is too soft in that area, because the beam is concentrating all its forces to a single point, and that point of the shell is overly deformed

drilling_2.png (62.96 KiB) Viewed 4587 times