modal analysis error
modal analysis error
I want to make a model with infill walls and waistheight 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 postprocess 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.
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 postprocess 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 (403.09 KiB) Viewed 246 times

 model_inele.zip
 (223.38 KiB) Downloaded 10 times
Re: modal analysis error
There were several errors in your model.
Here is a fixed version, check it after reading what I changed: Errors:
Here is a fixed version, check it after reading what I changed: Errors:
 3 Lines around the infill were missing an ElementProperty, therefore your system was singular (negative eigenvalues)
 Some nodes at the base were missing a fix
 An extra node was wrongly fixed as master of the diaphragm
 Some columns were drawn from toptobottom. 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
 With the abovementioned 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 2.35e5, but this is a specific weight in Nmm (equal to 23.5 kN/m^3). Your mass density should be 2.35e9. So I scaled all your masses by a factor of 1.0e4. Keep in mind that in Nmm 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 1.0e4.
 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
Re: modal analysis error
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?
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 (279.59 KiB) Viewed 237 times

 Posts: 140
 Joined: Fri Nov 13, 2020 1:52 pm
Re: modal analysis error
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 =)
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 =)
Re: modal analysis error
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 infillwall 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 elearning course (June).
If you attach your model we can show you how to use it.
you have only 1 option to solve this issue if you still want to use the automation of the infillwall 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 elearning course (June).
If you attach your model we can show you how to use it.
Re: modal analysis error
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.
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
Re: modal analysis error
Dear gookki,
I just realized that using the ASDEmbeddedNodeElement in this case would require too much work.
Instead I adopted the other solution:
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.

 Posts: 5
 Joined: Mon Apr 12, 2021 8:41 am
Error in Modal Analysis of CFS Building
Dear STKO team,
I want to perform a time history analysis on the Coldformed steel 2story building. The sections are builtup 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 twomode 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!
I want to perform a time history analysis on the Coldformed steel 2story building. The sections are builtup 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 twomode 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 (101.58 KiB) Viewed 183 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.
Re: modal analysis error
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.