Incorrect Reaction for Unit Displacement 3

[WayneKagawa]

Hi
I am modelling a lumped mass model of the outer shell of a Nuclear Containment Structure given in a research paper.It is a hollow cylinder with a dome placed on top.
To find out the total lateral stiffness, I applied a Unit displacement at the topmost node of the structure and checked the total reaction of the structure which is coming out to be less than the given value. I am doing a linear static general analysis in ABAQUS with concrete as the material.

I can't figure out what is causing the issue. Please help!

 

[bkal]

Is your mesh equivalent to the one used in the paper, including element type etc? What about material properties? You need to give us more information.

 

[WayneKagawa]

The paper just gives the number of meshed elements in the model which I iterated the mesh size to find out. The element type as such is not mentioned so I used the default solid mesh element with hybrid formulation. Also, the paper mentions the young's modulus and the shear modulus which are related in such a way that the poissons ratio is 0. The density is not given but the total mass is so I divided it by its volume to figure the mass density out. Please let me know if more information is needed.
Thank you!

 

[bkal]

This is still insufficient information, could you post a deformed shape with displacement contour plots as well as your mesh. I note that you describe the structure as a "shell" but you use solid elements. Did the original (from the paper) model use solid or shell elements? Could you give the paper reference?

If it is a static model, the density is irrelevant unless you are considering the self weight. Regarding the poisons ratio, assuming that the vessel is concrete, are you trying to model it in a cracked state?

 

[WayneKagawa]

Hi bkal

I appreciate your effort to help me and I apologize for unsatisfactory information. I am new to this forum and I will improve upon this.

By shell, I meant to describe that I am only considering the outer concrete surface and not the internal components of the containment structure. I did not mean it as a shell element.

I am referring to the uncracked state. The paper gives the E as 29.16Gpa and G as 14.58Gpa and says nothing about the poissons ratio so I used the formula E=2G(1+v) to calculate it as 0. I gave it a mesh size of 1.165m and gave an ENCASTRE boundary at the base of the structure and a Unit Displacement boundary condition in the X direction at the top. I checked RF1 at the end of the Static General step which is about 50% less than what it should be. I have attached the input model for your reference.

http://link.springer.com/article/10.1007/s11803-013-0173-1#page-1

is the link of the paper. If needed I can attach the PDF.

Thank you so much for your time.

 

[bkal]

I've run your model and the results (deformed shape) show that your mesh / element type is not appropriate. Have you tried with shell elements, and have you tried with the mesh in the centre of the dome being different. At the moment the aspect ratio of the elements there is quite poor.

 

[WayneKagawa]

Hi Bkal
I haven't tried shell elements as the paper mentions the use of solid elements for the analysis.
I used the tet mesh with a "free" orientation and reduced the mesh size a little more to about 0.9 which did result in a higher reaction than before but still about 25% less than what it should be. I used the C3D4H element in the mesh.

I will try iterating the mesh size to see if the value of RF1 reaches the level I want it to.

Do you have any other suggestion bkal?

Many thanks for your inputs.

 

[GoleGeli]

hi WayneKagawa
if you can use section force(sf) output for whole model in field output
then after run job in visiualization module use cut free body to observe the section force component in each increment.
good luck

 

[WayneKagawa]

Hi guys
I tried iterating the mesh size. I found that as I increase the global mesh seed, the reaction force increases. I suppose this follows from the logic that a larger mesh size makes for a stiffer surface whereas a lower mesh size makes the surface more flexible. Even though now I am getting the reaction RF1 that I wanted but I don't know if I can trust this as when I checked the warnings, it said that there are several elements distorted.

Please help!

 

[bkal]

I still think that the mesh is the issue, and it seems that you have one element only through the thickness. The deformed shape I got what I ran your .inp file showed that all the action (deformation) happens within a few elements adjacent to the displaced node.

 

[Mustaine3]

You use C3D8R-elements with one element through thickness and have bending in your behavior. That means that the reason for the soft behavior is probably Hourglassing. Google it for more details.

Use C3D8I or C3D20R elements or use at least 4 elements through thickness with C3D8R elements.