Stress due to the mismatch of thermal expansion coefficients of two different attached materials in COMSOL

Question

I'm simulating the thermo-electro-mechanical behavior of a copper wire which is surrounded by silicon dioxide. In other words, the wire segments is under mechanical and thermal loads and at the same time an electrical current is flowing in it.

In order to perform the simulation accurately, I think that I should consider an initial stress due to the mismatch of thermal expansion coefficients between copper and oxide. I am using COMSOL to do my simulation. The options that COMSOL provides me with are "body load" and "boundary load". Can anyone advise me which one I should choose? Which one is a more realistic assumption. Thanks.

Answer 1

Thermal stresses are self stresses that arises in two main cases.

1. If one imposes displacement continuity at the interface between two materials with different thermal expansion subjected to a uniform temperature change;
2. if an homogeneous material is subjected to a non uniform temperature change.

(Here with uniform I mean constant with respect to space, i.e. no gradient.)

Being self stresses (equilibrated to vanishing external body forces) you cannot model them as external loads.

Thermal effects are correctly taken into account if you perform a thermo-mechanical simulation, i.e. solving both for the temperature field and stress field. Of course the stress-strain relation should be written taking into account the inelastic strains due to thermal expansion.

A few remarks.

1. Pay great attention to the mechanical boundary conditions: as everyone knows huge stresses may arise in thermally loaded structures subjected to mechanical constraints. So ask your self if the modeled boundary conditions are an accurate representation of your physical prototype.
2. Thermo-mechanical simulations can be uncoupled (first solve for the temperatures, and the for the stresses) or coupled (solve for temperatures and stresses simultaneously). Since you have also electrical behavior to model, accurately analyze how the three field equations are coupled.

Edit

Using FEM thermal stresses are easily incorporated into the model, provided that thermal expansion is correctly modeled. (Every text book on solid mechanics and FE analysis should give you the details.)

The case of $N$ distinct materials each with its own domain $\Omega_i$, $\Omega \equiv \bigcup_{i=1}^{N} \Omega_i$, is simply treated by having continuous displacement and temperatures across the material interfaces (which is always true for a conforming mesh in $\Omega$) and discontinuous thermal expansion and elastic constants (which again is simply obtained by assigning to the elements of each subdomain $\Omega_i$ the corresponding material properties). This will result in the correct (discontinuous) thermal stress fields int the whole $\Omega$.

No extra or ad-hoc assumptions needed.