Use of SECOFFSET command

[Rok1707]

Hello!

I have a question regarding to the use of command SECOFFSET in connection with element SHELL181 that I use for linear structural analysis.

I'm using this element to model shell with few layers, but I need to offset nodes from midplane to the top or bottom of the element.

The problem is that the results of the analysis don't change no matter how much (option USER) or where (TOP or BOT) do I offset nodes.

Does anyone know where problem is. The results should change because moment of inertia changes.

 

[Drej]

Why do you need to offset the section? Which results don't change? What are you doing exactly - type of analysis, type of system being modelled, etc. etc...?

 

[Rok1707]

Oh, I'm sorry for incomplete description.

The reason for offseting the nodes is that this shell, if I can call it like that, is bonded to the part which is modeled with solid (SOLID185) elements.

The geometry is taken from CAD package (and meshed in ICEM CFD), hence, I don't have midplane of that shell. So, that exmple that I mentioned in the first post is just a test, to see how everything goes. I expected some changes in deflection when I changed that SECOFFSET command, but nothing happened.

The problem is sketched in a picture.

Analysis is linear and static, as I mentioned in the first post. And I'm concerned only in deflection, stresses are not that important.

 

[Drej]

Section offsets for shells are used primarily in contact analyses, where you may want to model contact between, say, two shell surfaces in parallel. You might want the contact here to be between the outer surfaces of the shells only - by the use of an offset - whereas by default it will be between mid-surfaces of the shells. Hence why your results don't change.

Cheers,

-- drej --

 

[Rok1707]

OK, so as far as I understand your answer it is not very good idea to use this SECOFFSET in my case at all.

Actually that test that I did was with flat surfaces, not with some irregular shapes. And when I plotted those shell elements, I saw that they were "offset" from the nodes, but the deflection was the same. Unless this command is there only because of visualization, and has no effect on computation.

And what do you think that it would be good solution in my case? How to model this contact between solid and shell? The other problem is, that right now the shells are literally fixed to the nodes od solid elements. The shell and the solid share the same nodes. I did not use any constraint equations or node coupling nor contact elements. I was thinking that maybe this is the problem.

And thank you very much for your answers Drej!

 

[Drej]

No problem. Nice picture by the way, I wish I could insert these sorts of pictures myself.

The "contact" between the shell and the solid can either be modelled with (1) "bonded" contact (i.e. using contact elements) or (2) as you've done with shared nodes, so no worries here. However, a few things to think about in your analysis:

1-- transfer of moments between the shell-solid interface
2-- mesh density

Remember that the shells have 6 DOF (3 translational, 3 rotational) and the solid has 3 DOF (3 trans only). Hence no moment transfer will take place between the shell and the solid. This will only be a problem if (1) your problem is bending dominated and (2) if your mesh density is too coarse around the area of interest. Hence, decide for yourself given your geometry and loading whether your mesh is appropriate. The shared translational DOFs should
be sufficient for the transfer of load. If you're expecting large bending deformations, simply refine the mesh accordingly. As far as visualisation is concerned, the shells, when plotted, should definitely NOT be offset from the solid185 elements. Remove that SECOFFSET command and just recheck making sure with powergraphics both on/off.

Cheers,

-- drej --

 

[Rok1707]

Thank you very much Drej, I think I found the problem.

It is like this. I did tests with both 3 and 6 DOF (with changing KEYOPT(1)). And the first problem was, that normals were not consistent. Some were directed outside and some inside. And I never saw that because I was always doing everything in a batch mode. I plotted mesh there, but the whole picture was simply too small to see the problem.

However, after I oriented normals in the right direction and I did tests again, and the deflection has changed in one case. It seems that this SECOFFSET command has effect only on shells with 6DOF. And this makes sence, since with this option we increase the moment of inertia. But this moment of inertia is connected with bending moment. Hence, if you have shells with 3DOF, there are no moments in nodes and this SECOFFSET has no effect.

Do you think my conclusion is right?

 

[Drej]

I don't understand your logic here. The normals only matter when you have contact, and since you don't have contact the orientation shouldn't affect the results at all. The moment of inertia is only applicable when you have dynamic/rotational loads. On the other hand, the second moment of area (associated with bending) does have an effect on a section under bending. In either case, offsetting the shell section should make no difference, as this is only a mathematical trick for contact - the second moment of area is the same with/without an offset.

 

[Rok1707]

Hmm. My apologies. The expression "moment of inertia" isn't exactly the best. I'm not native english speaker and sometimes I have problems with some expressions. However, I was talking about second moment of area:

We usually call this one moment of inertia, which is not the same as mass moment of inertia.

And about the normals. Actually they do matter, because they define direction in which layers are suppose to be "extruded". So, if you use SECOFFSET and the normals of two neighbour elements do not have the same normal direction, this means than on one element the layers will be extrued up, and on the other one they will be extruded down. And this affects second moment of area. I tried to explain this in this picture, where you can see cross section of a rectangular beam with two different directions of normals.