Themomechanical Analysis

[alexzive]

Hello there,

I have a problem understanding some results from Thermomechanical Analysis with Abaqus . I performed some simple tests on a 2D plate (all in the zip file). UNits: Kg, mm, J, s, N. Each simulation consists of 2 steps:

Step-1: heating up the plate homogenuosly with the same heat flux applied at the 4 sides of the plate. The flux follows a tabular amplitude (linear increase, plateu, linear decrease). No mechanical constraints. No external forces.

Step-2: once the flux has been decreased to zero from the previous step, step-2 is just a relaxation to a certain time with no flux applied. The heat remains inside the plate because the whole process is supposed to be adiabatic. No mechanical constraints. No external forces.

I used temperature dependent material data for tungsten: a simple thermoelastoplastic model with the plastic part of the stress/strain curve as horizontal line. Expansion coefficients for Tungsten are also given. (see .inp files)

I expect the plate expands the same in all direction because of the heating, without stress inside.
I got following results for both sequentially coupled and fully coupled thermomechanical analysis:

a. with expansion coefficients -> expansion + overall non zero stress ~ 800 Mpa!
b. without expansion coefficients -> no expansion + overall zero stress

Case b is fine.
Case a: it seems that in case I allow thermally induce expansion, the abaqus solver associates some internal stress to the pure thermal strain for some reason. But pure thermal expansion without mechanical constraints nor external forces should produce an overall zero internal stress, isn't it?

To sum up:
I expect for both case a&b: ?(total) = ?(elastic) + ?(plastic) + ? (thermal) = ? (thermal) but ?(total) = f(?(elastic) + ?(plastic)) -> ?(total) = 0 even if ? (thermal) >0;

What I actually get is:

?(total) = 0 overall only if I don´t activate thermal expansion

WHY it doesn't do the same with pure thermal expansion????
What I did wrong??

many thanks for any help!
Alex

********************************
List of attached files:

test5reg_T_smoothFlux.inp -> thermal part of sequentially coupled analysis
test5reg_T_smoothFlux.odb -> results of thermal part (needed for mechanical part)
HTtestreg_S.inp -> mechanical part of sequentially coupled analysis
HTtestreg_S_noExp.inp -> mechanical part of sequentially coupled analysis without thermal expansion
HTtestreg_TMFC.inp -> fully coupled TM analysis
HTtestreg_TMFC_noExp.inp -> fully coupled TM analysis without thermal expansion

 

[corus]

Thermal stresses are produced by differential thermal expansion, just as if you heat something up uniformaly and restrain all edges from expanding then you'll induce a stress. The same thing will apply if part of a structure is at a different temperature to another. The cooler region will be expanded further than it should, and the hotter region will be contracted by the cooler region, producing tensile and compressice stresses respectively.
Looking at the odb file there is a slight difference in temperature, but not enough to cause any significant stress (thought the stresses aren;t output). In the .inp file, though, you appear to have no restraints so I'm a little surpised that it actually managed to run at all, if it did.

corus

 

[alexzive]

Hello Corus,

you are absolutely right about thermal stresses..that´s the reason why I am very dubious about my results: I have no thermal gradient inside the plate but non zero stress too!!. Probably I have done some mistake somewhere, I don´t know where.

all the simulations converge despite the fact there are no mech. constraints (pure heating, plate free to expand). I am doing this because I am actually looking at pure thermal expansion in more complex geometries and how this is managed in the abaqus TM solver. But first I started with a simple one.

In the zip file I put the second odb (mechanical part) for the sequentially coupled analysis including expansion (you can see the non zero S distrib. as result of the simulation). Unfortunately the fully coupled odb is too big to upload. You can run the sim. by yourselfes from the inp file in the previous attachment, it'll only take some minutes to converge.
Alex

 

[MrMyers]

Tried using plane stress elements?

Otherwise plot your stress vectors which might indicate where the stresses are coming from?

Do you have any yielding? There could be residual stresses.

 

[alexzive]

Hello MrMayers!

thank you very much for your very useful suggestions!!!

I changed to plane stress element and the anomalous stress field disappeared!!
So the issue seems to be related to the choice of the elements, between plane stress and plane strain.
I also checked the components of the S tensor (my mistake not have done it before!) and noticed that the dramatic high values were only for the S33 component which exits the plane in the z direction. It seems that "isotropic" heat flux is responsible for such stress in the z direction.

Now what is the most consistent result for the real case? does this S33 >>0 really exist in case we heat up a plate free to expand? Or the result with plane stress (S33=0) is the more realistic one?
And what about if we´d consider the plate as 2D cross section of a 3D cube?

I have to think a bit about it, but any input is welcome!

Thank you so much again!
AZ

 

[corus]

In plane strain you are effectively preventing thermal expansion in the out of plane direction as the strain is set to zero, and hence produce stresses. You should use generalised plane strain elements if your model represents a thick plate and restrain only the rotational freedoms to keep the section plane as it expands in the Z direction (constant strain). The stresses you'll get (for an arbitrary temperature distribution) will represent the stresses in the centre of the plate. Plane stress will represent stresses at the free surface of the plate.

corus

 

[alexzive]

Dear Corus,
thank you very much for your help,
I am trying to compare results also with gener. plane strain, but for the case of more complicated 2D geometries I am experiencing convergence problem (the simullations simply don´t converge).
Once I am done with this problem I will start a new thread for the interpretation of the results of my TM simulations in the real case..(not the simple plate, but complex 2D crossections of a 3D model)..
Hope to still get your help, many thanks, Alex