Weird Results from ETABS 2

[DanAndrews]

I have this 4m x 10m tall wall modelled in ETABS with 4 end nodes restrained and 1kPa area load applied at out-of-plane direction.
I was expecting the the bending moment at mid-span to be around 1*10^2/8 = 12.5kNm/m. However when I went to Moment 22 for piers it shows nearly 0 and M11 for shell objects gives me very small values (less than 2) as well as shown below.
When the weirdest thing is that it gives me multiple reactions at mesh nodes where I didn't assign point restraints to. (which is why I got smaller moments)
Does anyone have this issue as well and what cause this problem? Thank you

 

[MSUK90]

Can you share your etabs model so that I can have a look into the problem??
And would also like to know the actual use of wall, what you are trying to design here?

 

[DanAndrews]

Sure MSUK90. Just uploaded. Thanks.

I am trying to get the out-of-plane moment of wall under wind load but had this kinda of issue in my model so I simplified the model to see what happened.

 

[Agent666]

Looks correct to me based on your boundary conditions, spans horizontally as modelled, M*=1 x 4^2/8 =2kNm vs your etabs 1.8kNm for M11?

You've created a 2 way spanning shell, your question suggests this is not what you wanted? Remove the auto restraints being applied to the vertical edges?

https://engineervsheep.com

 

[MSUK90]

Dear DanAndrews,
I couldn't open your model in my etabs version(v 19.0.1). Can you share the e2k or set file so that I can import your model?

 

[DanAndrews]

Thank you Agent666. Sorry was meant to upload M22 instead of M11. See below.

Yes it is a two way shell but only 4 end nodes are restrained so at the end of the day it will still behave more like a simply supported beam span vertically because there is no restrained along two vertical edges of the walls. M22 should be somewhere around 12kNm.

Do you mean auto edge constraint? If so, I believe this is for shell to shell and shell to line object while I have only one shell here so shouldn't affect it? Anyway. I have changed it and it gives me the same result.

And what happens to these reaction results at node locations where I didnt assign restraints to?

 

[DanAndrews]

Hi MSUK90, e2k uploaded.

 

[DanAndrews]

Okay I found what the problem is now.

I think this is what Agent666 is refer to.
The last box should be uncheck....

Any way that I can keep the horizontal edge restraints only?

 

[MSUK90]

 

[MSUK90]

The last box should be uncheck....

Yes, you needed to uncheck that box.
Now the results are similar to manual calcs I believe.

 

[DanAndrews]

Thank you.
Do you know why the moment 2-2 in the pier results still show 0?

 

[MSUK90]

That's amazing.
I did not check the pier forces and when I check now, there is no moment showing in both the directions(even in the shear wall design result summary).
I tried to check for the error but no success.
Do update if you find the problem.

 

[sticksandtriangles]

Do you know why the moment 2-2 in the pier results still show 0?

You need to subdivide your shell and apply unique wall pier assignments to get bending to show up in your shell.

Something like this:

Wall piers only report forces at the ends of them between levels, so that why it shows 0 moment now.

https://wiki.csiamerica.com/display/etabs/Pier+and+Spandrel+Labeling+and+Design

S&T

 

[DanAndrews]

I see. Thank you very much!

 

[MSUK90]

Wall piers only report forces at the ends of them between levels, so that why it shows 0 moment now.

Does that mean the wall will then be designed only for end moments in case if we don't subdivide it and assign piers as you have specified?

 

[sticksandtriangles]

Does that mean the wall will then be designed only for end moments in case if we don't subdivide it and assign piers as you have specified?

That's correct, the design module for wall only knows the forces associated with the end cuts. For shearwalls, this is typically okay for only reporting forces at levels. For out of plane bending you will miss the moment in the middle of the wall if you do not subdivide.

Now that I am typing this though, I do not think that etabs design for out of plane bending, but you still want to subdivide to retrieve the results you are after.


S&T