asdeasoft.net

Hello STKO team,

I am developing a model for a mixed masonry-RC building. The model was initially imported from AutoCAD and only then I modified some details. All the masonry walls are represented by the TC3D damage model including an RC wall. The RC beams and columns are represented by fiber cross-sections.
The issue I am facing is attached below and I would appreciate a closer look on it. I made sure that there is no any geometry with out element/physical assignment, but it didn't appear resolve the issue.
I am happy to send the .scd file of the model (I couldn't attach it with along this message for some reason though).

Looking forward to your response!

If you look at the last line, it says that (line 173) the "domain" object, on which STKO is trying to call the ".elements" property, is None.

This means that you meshed your geometry, but some parts of it could not be merged for some geometry error. In the mesh view, try to identify the geometry (typically a face) that could not be meshes (you will see it as a transparent face), or look into the Terminal messages, there you should find some details

Thank you for your prompt reply. That is exactly what is happening, when I mesh it, I can see that a handful of surfaces are transparent and unable to be meshed. And, yes, they are also indicated in the terminal.
To resolve it, I removed all these surfaces and re-draw them, but the issue persists.
Could you please suggest another approach to help me resolve it. Please note that redrawing the entire building is not an option as it is a large model.

Thank you in advance!

Unfortunately, it's hard to tell what is the issue. Could you share your model here?

Sure, please find the model attached below (I have attached it as image file to be able to upload it, but you still will be able to open it in STKO).

Thank you again for your time!

I managed to identify the faces which cannot be merged, here are some of them: Unfortunately, they are very imprecise, that's why some of them cannot be meshed: This happens very often with users using AutoCAD as a modeling tool. You should avoid as much as you can imprecise O-snap tools such as "near point", "intersection", or "perpendicular". They generate approximate o-snap points which are good for modeling/rendering purposes, but are not accurate enough when you import the geometeries into software that try to mesh them for FEM analysis.

I'm sorry but I think the best solution for you is to draw it directly inside STKO, or you can re-draw it in autocad paying attantion to the tolerance that you use and avoiding imprecise o-snap

Thank you very much for your insights, I completely understand that the O-snap tools can cause such issues.
To get a quick resolution on the issue, I used the 'Repair Fix' command in STKO with 10^-2 tolerance (in this large model it is acceptable). I lost material assignment on some surfaces after doing so, but it was easy to assign them back.
Now that I don't have the meshing issue, I run eigenvalue analysis but I am not able to get modal results.
I would appreciate if you could take a look at it. The model is attached below.

The are some mistakes in the boundary conditions:

• The fix of the floor master nodes is not included in the constraint pattern
• The "perpDir" attribute in the rigidDiaphragm conditions should be "3" because your floor are in the X-Y plane.

Yes, the RepairFix works in most cases (and yes, you lose material and element assignments) but is not magic... The approximations in the AutoCAD o-snap created other imprecisions, in fact, there are some warnings regarding some floor nodes not being in the XY plane. This happens when some nodes are at a Z coordinate which is different from the Z coordinate of the master node.

Another issue is that some of your faces are not attached due to the above-mentioned approximations.
I used the QueryGeometry tool to highlight the free edges. Free edges are edges which are borders of only 1 face. So you should see them only at windows or door openings, bot not in the middle of a wall.
Instead, there are many places where this happens: If you zoom in, you can see that there is a small gap between the faces, this creates a cut in the wall, and that piece of wall is completely detached from the building, therefore your matrix is singular.
You need to fix this issue before running the analysis.

Dear STKO team,

Thank you very much for your insights and comments.
I only returned now to office after a work leave due to a family issue.

I have addressed all the issues of the model and it looks now that I am able to get the modal parameters, but I obtained very low frequencies compared to the expected ones.

Could you please point out any pitfalls on the model that could lead to this situation?

Thank you again for your time.

PS: updated model is attached here.

There are some mistakes that can lead to this.

First, you are using EqualDOF instead of RigidDiaphragm. This will constrain in-plane rotations.

You are running the gravity analysis with a Linear solver. This is not correct because you have non-linear materials. This will give a wrong response after the gravity analysis that will affect the eigen analysis