modal analysis error

Post Reply
gookki
Posts: 13
Joined: Wed May 19, 2021 8:24 am

modal analysis error

Post by gookki » Thu May 20, 2021 8:20 am

I want to make a model with infill walls and waist-height wall.
I have some problems with the infill wall element tool because of the interaction between the surface and truss element.
So, I just test one infill wall that don't interact with the truss. I make the model then merge the whole element. Then I have a minus value with eigen command. also, the post-process graphic that I got was horrible. I want to find what's wrong with it.


One more problem: During modeling, whenever truss or wall is merged, columns or beams disappeared. So I need to draw it again. I also want to know why this is so.
Attachments
analysis_postprocess_error.png
analysis_postprocess_error.png (403.09 KiB) Viewed 247 times
model_inele.zip
(223.38 KiB) Downloaded 10 times

STKO Team
Posts: 660
Joined: Tue Oct 29, 2019 8:45 am

Re: modal analysis error

Post by STKO Team » Thu May 20, 2021 2:39 pm

There were several errors in your model.
Here is a fixed version, check it after reading what I changed:
model_inele.zip
(223.03 KiB) Downloaded 9 times
Errors:
  • 3 Lines around the infill were missing an ElementProperty, therefore your system was singular (negative eigenvalues)
    3_lines_with_no_elem.png
    3_lines_with_no_elem.png (75.74 KiB) Viewed 239 times
  • Some nodes at the base were missing a fix
    2 cols no fix.png
    2 cols no fix.png (87.62 KiB) Viewed 239 times
  • An extra node was wrongly fixed as master of the diaphragm
    extra_node_fixed.png
    extra_node_fixed.png (91.89 KiB) Viewed 239 times
  • Some columns were drawn from top-to-bottom. You declared the column load in local coordinates, so the Wx would follow the dir_x of the lines. But on those wrongly oriented columns, the load will point upward. I just changed the load from local to global
    wrong_col_orient.png
    wrong_col_orient.png (315.07 KiB) Viewed 239 times
  • With the above-mentioned fixed, your model runs, but it will have periods of 30 seconds... There is an error in the mass. You assume a mass density for concrete of about 2.35e-5, but this is a specific weight in N-mm (equal to 23.5 kN/m^3). Your mass density should be 2.35e-9. So I scaled all your masses by a factor of 1.0e-4. Keep in mind that in N-mm the acceleration of gravity is 9806 mm/s^2.
    With this, your periods lower to about 0.3 secs.
  • Same for loads, I think they where 1e4 time larger.. so I scaled them by 1.0e-4.
  • On trusses you cannot use eleLoad, I changed it to EdgeForce
  • I replaced the old TCL script for modal analysis to the new modalProperties command that we added recently to OpenSees

gookki
Posts: 13
Joined: Wed May 19, 2021 8:24 am

Re: modal analysis error

Post by gookki » Thu May 20, 2021 3:17 pm

Thanks for you help, a lot of progress has been made.
but I have still one more problem.
I want to make infill wall element inside of model.
when I draw the wall with interaction as shown in the figure, it will be triangle even I set quadra.

Is there a modeling method for this situation? Or should I add the tcl code myself?
Attachments
infill interaction.png
infill interaction.png (279.59 KiB) Viewed 238 times

marafini.f
Posts: 140
Joined: Fri Nov 13, 2020 1:52 pm

Re: modal analysis error

Post by marafini.f » Mon May 24, 2021 7:23 am

Dear gokki,
The faces at the ground level of your structure are quadrangular but with 5 edges, and 5 vertices. If you assign size 1 to the edge seed you will never have a quadrangular mesh, because that additional node needs to be considered by your mesh.
If you want to model your infill as a truss, we made a webinar about it, number #11 https://asdeasoft.net/?webinar, you can check it out to learn how to use such elements. However, you will need to have square faces to apply the truss to simulate the infill walls, so you will need to either remove the diagonal element or divide your faces in two parts.
Let us know how it goes.
Best,
Francesca =)

STKO Team
Posts: 660
Joined: Tue Oct 29, 2019 8:45 am

Re: modal analysis error

Post by STKO Team » Mon May 24, 2021 12:56 pm

Adding to what Francesca already said,
you have only 1 option to solve this issue if you still want to use the automation of the infill-wall element.

We recently added the ASDEmbeddedNodeElement under the Condition->MP models.

This condition can be used to force a node to be attached to an element, even if the two are not physically connected. It will be the topic of our next e-learning course (June).

If you attach your model we can show you how to use it.

gookki
Posts: 13
Joined: Wed May 19, 2021 8:24 am

Re: modal analysis error

Post by gookki » Tue May 25, 2021 5:06 am

Thank you for your answer.
In fact, I was considering adding elements directly to the code. However, I wonder how to use ASDembeddedNodeElement.
so I want you to briefly show me how the function is applied.
Thank you very much for your help.
Attachments
test.zip
(238.35 KiB) Downloaded 8 times

STKO Team
Posts: 660
Joined: Tue Oct 29, 2019 8:45 am

Re: modal analysis error

Post by STKO Team » Tue May 25, 2021 1:47 pm

Dear gookki,
I just realized that using the ASDEmbeddedNodeElement in this case would require too much work.
Instead I adopted the other solution:
  • I detached the walls (Faces) from the frame (Edges). In this way the walls do not intersect with the diagonal low trusses, and therefore they can be meshed with a single quad element.
  • I added an EDOF condition between the Frame and the Walls in all 6 DOFs to restore continuity
  • I had to change the constraint handler to Penalty, because now the EDOF will be in conflict with the rigid diaphragm using the transformation method.
  • For the same reason, I had to put a fake analysis (0 steps, without the wipeAnalysis) before the eigen, otherwise the eigen (by default) will choose the transformation method.
Please make sure I re-applied all masses and loads correctly after changing your model
test.zip
(259.28 KiB) Downloaded 7 times

nparag@iitg.ac.in
Posts: 5
Joined: Mon Apr 12, 2021 8:41 am

Error in Modal Analysis of CFS Building

Post by nparag@iitg.ac.in » Wed May 26, 2021 10:06 am

Dear STKO team,
I want to perform a time history analysis on the Cold-formed steel 2-story building. The sections are built-up sections that are modeled as section fiber. The acceleration is applied and analysis is carried out in STKO but the results that I got from SAP2000 are not at all matching with STKO analysis.
To rectify the problem I tried to perform the Modal Analysis but, the first two-mode themselves are showing wrong results. The natural frequencies are as shown in the attachment which is wrong.
I am attaching the .scd file kindly help me through this.

Thank you!
Attachments
Modal Analysis Error.JPG
Modal Analysis Error.JPG (101.58 KiB) Viewed 184 times
trail_4.rar
(146.52 KiB) Downloaded 9 times
Last edited by nparag@iitg.ac.in on Wed May 26, 2021 1:20 pm, edited 1 time in total.

STKO Team
Posts: 660
Joined: Tue Oct 29, 2019 8:45 am

Re: modal analysis error

Post by STKO Team » Wed May 26, 2021 12:53 pm

There were 2 errors that lead to invalid eiegvalues (NAN):
  • All your fiberSection have GJ = 0. This makes your model singular (almost because they add a very small value). I solved it by assigning to each section , GJ = G(steel)*J(of your cross sections)
  • Since you split your rigid diaphragm in 3 per floor, there are some nodes that belong to multiple rigidDiaphragm, and this is not supported by the Transformation constraint handler. Since the eigen analysis by default uses the Transformation, I had to add a "fake" analysis (0 steps) with the Penalty method, and without the "wipeAnalysis" at the end.
  • I moved the eigen command at the beginning, but feel free to put it back at the end.
trail_4.zip
(267.24 KiB) Downloaded 8 times

Post Reply