Issue with Modal Analysis of a Frame Building

[kolozvari]

Hello,

I am trying to perform modal analysis of a frame building. The model has rigid diaphragms and lumped masses at each floor. When I try to run modal analysis and get the following error.

Modal_issue.JPG (89.71 KiB) Viewed 2875 times

I am not sure what is the issue. I ran modal analyses before with the same computer and STKO and didnt have issue. Can you please let me know how to overcome this? The model is attached for your convenience.

Thank you,

[kolozvari]

Hello, I was wondering if you had a chance to look at this issue. Please let me know.

Thanks

[kolozvari]

Hello, I just wanted to follow up on this issue since it has been ~10 days since I posted this. It would be great if you could provide me with a response or a guideline on how to approach this issue. I tried several things and none of them worked.

Looking forward to hearing from you.

Thank you

[STKO Team]

You are using Timoshenko beams, which require the shear areas (Ay = Area*alphaY and Az = Area*alphaZ), but in all your custom sections the alpha values (shear correction factors) are 0. So the shear areas are zero and the shear stiffness is zero, making the element singular, thus the Arpack error.


Here you have your model were I set all shear factors to 5/6, the typical values for rectangular cross-sections with typical aspect ratios. You may want to adjust those shear factor depending on the shape of your beams/columns

Frame_Building_Modal.zip

(664.89 KiB) Downloaded 200 times

[kolozvari]

Ah, of course, that makes sense. I was wondering where do you define this. I guess I got used to see this parameter being called "k" and didn't catch it. Thank you for fixing it, there was a lot of sections to change. If possible, it would be useful to add description of the section parameters (similarly to other parameters in the model) in future versions.

Thank you again for your continuous help!

[STKO Team]

If possible, it would be useful to add description of the section parameters (similarly to other parameters in the model) in future versions.

Sure! we'll put it in our todo list

[kolozvari]

Hello,

I would like to follow up on the same model discussed here. Per previous communication, the modal analysis works find and gives reasonable results. However, when I try to run dynamic analysis I am running into issues.

In my understanding, penalty analysis method should be used when rigid diaphragm constraint is in the model. Please confirm. If this is the case, how do I determine the suitable penalty coefficients alphaS and alphaM? When I use high value of these coefficients (e.g., 10^10, 10^11, 10^12), the model struggles to converge. When I use lower values (e.g., 10^7, 10^8, 10^9), the model seems to converge better, but I have noticed that the fixed-base boundary condition is not enforced anymore and the entire model has a rigid-body rotation. Therefore, at this point, I feel stuck because I am not sure how to make the model converge and obtain reasonable results.

Can you please advise on how to fix this? The model is attached for your convenience.

Thank you

[STKO Team]

In my understanding, penalty analysis method should be used when rigid diaphragm constraint is in the model. Please confirm.

Not necessarily. Rigid diaphragms are fine with Transformation. The transformation has issues when you have overlapping (conflicting) constraints: i.e. when the retained (master) node of a constraint is also a constrained (slave) node in another constraint.
The penalty method can handle that.

If this is the case, how do I determine the suitable penalty coefficients alphaS and alphaM?

Estimate the typical stiffness of your model: Ktypical = EA/L
Compute its order or magnitude: OOM = round(log10(Ktypical))
Penalty values = 10^(OOM + X), where X is something from 4 to 8 (no more than 8!)
If you are not sure about the OOM of your model, use the customTcl script calling "puts[EleStiffnessOOM]".
This function will show that your model has a OOM min = 4, OOM max = 10, OOM avg = 8.
So you can take the 8 and add 6 to use a penalty = 1.0e14.

Finally, never use NormUnbalance with penalty. Since penalty introduce huge forces to enforce the constraint, you will have to use large tolerances for the norm unbalance.
Use the normDispIncr instead.

[kolozvari]

Thank you! I figured it is related to the settings. The model is too simple to have any real issues.

Can you please remove the model from the forum?

Thanks

[STKO Team]

done