Thermal deformation due to temperature change

[Ishihara]

Dear FEAP community,
I am writing this using a translating machine.
I am currently working on an analysis of thermal deformation due to temperature change using FEAP. Reading "manual_86.pdf", I think that thermal deformation due to temperature change corresponds to "Linear elastic models" on p.87, is that correct? I actually entered a variable and got a displacement, but the value was strange, so I asked a question.
I would appreciate it if you could reply.
Ishihara

[Prof. S. Govindjee]

FEAP has thermal (expansion) models for small deformation but not for large deformation.  The large deformation case is something we plan to add soon but have not done so yet.

If you see a problem with the small deformation case, please post an example and we will try to debug it.

[Ishihara]

It will be this file.
This is a hyperboloid model with a hole in the center. It consists of 3906 nodes and 3600 elements. Sorry for the large number of nodes.
I would like to analyze the amount of thermal deformation for the amount of temperature change -85 [K].

[Ishihara]

Specifically, in the output file, it says "TETSHP: Determinant = 0.000000000000000E+000" or "*D4TRI WARNING* Lost at least 7 digits in reducing diagonals of 471 equations."
I would appreciate it if you could reply.

[Prof. R.L. Taylor]

The warning is that the element has no volume. 

What is the analysis, a solid or a shell?

[Ishihara]

I chose SOLID because it was written in SOLID in the manual, but if SHELL can also perform thermal deformation analysis due to temperature change, I would like to use SHELL for analysis.

[Prof. S. Govindjee]

I'm not sure I understand the mesh.  I have attached a zoom in to the mesh.  It seems that you want quads but you have all these crossing edges.  It does not make a lot of sense to me.

[Ishihara]

It's true, I didn't realize that. I want to generate a quadrilateral mesh, so the way to create the mesh is different, right?

[Ishihara]

Is the edge crossing due to the different way elements are created in the file or is it an earlier issue?
I apologize for asking so many questions.

[Prof. R.L. Taylor]

If you change the material type to SHELL it should then plot the mesh correctly.

However, I looked at all the shells and do not see any case where temperature is used.  If you can describe what you want to apply as thermal loading I will try to modify the code to allow you to perform the analysis.

Looking at the input data you specify the nodal temperatures to all be -85. Thus, it appears you just want to uniformly change the temperature by 85 degrees Kelvin/Centigrade.  That should be easy to do by just letting the nodal temperature be 0 and the reference temperature on the material record be +85. 

It is still necessary to modify the shell code where stress is computed for the membrane and bending effects to account for this.  A more general case would be where the top of the shell is one temperature and the bottom another.  This might be a harder case to add at this time.

[Ishihara]

thank you for your reply.
What I want to analyze is how this model made of aluminum alloy deforms against a temperature change of -85.
If you can fix the code, I would appreciate it.

[Prof. R.L. Taylor]

To add the effect of uniform temperature change modify ./elements/shells/shl3ds.f at around line 1300 to read
     call dmat2d(d,d(31),dd,alp)

      thk     = d(14)
      thk3    = thk**3/12.d0

      norm(1) = (dd(1,1)*eps(1) + dd(1,2)*eps(2) + dd(1,4)*eps(3))*thk
      norm(2) = (dd(2,1)*eps(1) + dd(2,2)*eps(2) + dd(2,4)*eps(3))*thk
      norm(3) = (dd(4,1)*eps(1) + dd(4,2)*eps(2) + dd(4,4)*eps(3))*thk
!     Modify in-plane forces by constant temperature change
      norm(1:2) = norm(1:2) - alp(1:2)*d(9)
      temp(1) = norm(1)
      temp(2) = norm(2)
      temp(4) = norm(3)

The change is the line after the comment -- be sure to place exactly as shown so outputs will be correct.

Modify your materials to read

MATErial 1
Shell
ELAStic ISOTropic 7e+04 0.3
THERmal ISOTropic 2.3e-05  85  !  85 is temperature change
THICk,, 0.5, 0.833333333
DENSity 1 2.7e-06

Also if you want the shell to be only 1 part instead of 6 you need a TIE command after the mesh END command to force the shell to be connected.

[Ishihara]

Thank you very much.
I'll think about it.

[Ishihara]

I apologize for the question again.
When I read the manual, it was said that the shell does not support thermal isotropic. Therefore, I would like to perform an analysis on a solid. Is it possible?
In the previous reply, you said that there was no volume, but I think this is probably because the thickness setting was not reflected.
Is it impossible to set it with the thick command?
I would appreciate it if you could reply.

[Ishihara]

I think that the content of the question is a little difficult to understand, so I will ask the question again.

I am currently working on thermal analysis of a hyperboloid-shaped object. Since the coordinates of the object are known, I would like to create an element with "ELEMENT" and analyze the object, but in this case, the volume is 0 and the analysis cannot be performed.
Therefore, I think that it is necessary to give thickness to the element, but I am in trouble because I do not know how to do it.
Please let me know if there is a better way.
(Should I use the BLOCK command?)