Ritz Analysis Problem

[mhdhamood]

Dear Engineers;

I had a headache from this problem :

I run analysis in Etabs for a G+4 Project using Ritz so it runs okay. But I wished to convert some
 

columns to shell elements instead of frame elements then I run the etabs but the response spectrum

 

analysis could not start. when I look into "Last analysis Log..." I found the following :
 

 

" The strum sequence check found 5 eigen values below the  shift 
 

Ritz analysis requires All eigen values to be above the shift "



Regards

[mhdhamood]

HELP PLEASE !!!!

[Muneeb Badar]

Dear  I do not know about this error. It did not happen to me before.

 

But why you wished to use shell element instead of frame element?

 

 

Secondly you can try it in SAP. I have assigned some beams and columns as shell element in SAP. It did not gave any error like this. 

 

Thanks

 

Muneeb

[mhdhamood]

Dear ;
I am using auto meshing...... I searched on internet this problem happened but in chinese forums I couldnt translate
Dear Muneeb, I wished to use because of the first mode I got is torsional mode and the columns are 1.5*0.3 m .
I want to reduce the effect of torsion and I got high reinforcement under cores in Mat .

[mhdhamood]

This is another site says about this error 
http://www.construaprende.com/foros/no-corre-el-modal-vt9415.html

[mhdhamood]

NOTE:
Now I removed the P-Delta then the modal analysis is running and it works .... but I want to use the P-delta so what to do ??

[Syed Umair Haider]

This message is indicative of some modelling error in your model as Shift is the centre of cyclic frequency range that is used to limit the modal frequency range i.e to enforce program to neglect modes with frequencies below shift,By default shift is a very small value something like .0001,any mode with eigen value lesser than that of shift means a mode with a very low frequency or a very high modal period that indicates some modelling most probably member connectivity error in your model.

[mhdhamood]

Mr Syed Umair Haider and All engineers;
Thanks for you. But Let us discuss the problem.
Why when I remove the P-delta analysis option then it works ?
Also When it was with frame elements (NOT SHELLS) it was working properly?
I have high sense that the problem coming from auto meshing .why?. That because In many projects I had the same problem then the solution was  changing the size of auto mesh (i.e it was 1 meter , then I changed to 1.2 m) it worked.
But Why, I cant understand.

Regards

[Muneeb Badar]

Dear for this particular error, I think u r the best person who can search for this as u know the problem in details..........

 

But kindly tell me how do u know that by converting to shell element torsion will be reduced and your reinforcement will be reduced. How did u concluded that. 

 

Thanks

 

Muneeb

[Syed Umair Haider]

Auto meshing doesn't ensure adequate connectivity between member to member and is therefore recommended for horizontal area elements enclosed by line elements only (floors), where there is no structural connection between floor and any element in between the panel.

 

In case of vertical elements, connectivity between vertical and horizontal elements is of due importance and is better to be achieved through manual meshing.

 

In case of auto meshing as you indicated, change in size of auto mesh could solve the problem as its possible that connections inadequate (nodes not coinciding) on 1m element size can be adequate for 1.2m size (nodes start coinciding) and so on.

 

For p-delta,a possibility exists that due to any meshing error some connection is modelled with inadequate lateral stiffness i.e when program try to impose lateral deflection due to seismic loads,modes start yielding frequency below shift.

 

If you are interested in studying the problem,then easy approach is to check each mode shape and investigate the member that is going in unrealistically large displacement. Solving this member's connectivity inadequacy will solve your problem.

[mhdhamood]

Amazing interpreting for the problem Mr. Syed Umair Haider
Thanks I will try to solve the problem as you said and told you all what happened.

[mhdhamood]

Dear Engineer Muneeb;
My senior engineer told me that; when converting to shell elements it will attract more forces and help the cores in sharing the forces then the stresses under cores will be reduced.
If you have a comment please share it we will be pleased

[Muneeb Badar]

Dear Mohammad Shaker

 

I do not know about this and also did not hear about this at all  . In my point of view, frame element can be converted to shell elements where there are large transfer of forces at the joints. For example, in case of Transfer Girders (the girders which transfer shear force from shear wall to adjacent columns) must be or can be modeled as shell element as these are directly attached to the member(shearwall) which is transferring heavy shear. The same is the case under Pile Cap. The connection between pile cap and top of pile is critical. You may have seen that the pile near pile cap shows heavily reinforced because we model it node to node so some portion of pile must be inside the pile cap. But when you model frame element it will not catch this effect. So to have this effect we model top portion of pile as shell element.

 

As far as what you are saying is concerned, in my point of view, the absorption/collection of forces is stiffness based. If you model a s column of 300x1500 as frame element then you need to design it as bi axial bending as it will take inplane as well as out of plane bending. The shear reinf. you need to provide must be both sides. But of you provide this 300x1500 member as shell element then you need to skip out of plane bending because we normally neglect the out of plane stiffness of shear wall. 

 

So if shell element with proper modifiers it will not absorb the lateral force in  out of plane direction. But if you use as frame element it will give you inplane as well as out of plane stiffness and then you need to design as for both biaxial bending.

 

I am not sure I make a proper reply to your question or not.........

 

Thanks

 

Muneeb

[mhdhamood]

Firstl I would like to thank you because you are very active and writing in details.

[WR1]

As Muneeb pointed out, the lateral load transfer depends on stiffness of vertical elements.

 

A concrete shell element of the same size of a line frame element has about 4% higher stiffness because of posions ratio.

 

Thats not a big difference but a shell element when meshed has more supports at base adds up to the stiffness as compared to single support frame element.

[mhdhamood]

ooooooh very nice explanation thanks I got more one information