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

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.

• I originally asked this question here: physics.stackexchange.com/questions/75405/… – alifornia Aug 28 '13 at 2:27
• Cross-posting is usually frowned upon, so could you either remove or modify the question on the physics site? It seems off-topic there in any case. – Godric Seer Aug 28 '13 at 13:47

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.

• Thanks for your advice. I finally added a boundary stress of 100 MPa at their interface due to the thermal expansion mismatch and the result is very close to what I expected. Now, I'm trying to do a more accurate simulation. I'm simulating the coupled thermo-mechanical behavior of my model in COMSOL. In other words, I'm adding the actual insulation (SiO2) around the copper wire and trying to solve the thermo-mech equations for the entire domain (SiO2 and copper). Can I assume that COMSOL will automatically handle the stress due to the material mismatch at their interface? – alifornia Sep 7 '13 at 6:56
• What exactly I've done is: I have a copper wire in the middle of an insulation (SiO2). I added a thermal expansion model (or so-called physics in COMSOL) ONLY to the wire and made the boundaries of the insulation fixed & let the boundaries of the wire be free. Then I solved the stress equations for the entire domain. My questions are: (1)Can I assume that COMSOL will automatically handle the stress due to the material mismatch at their interface? (2)Will the effect of thermal expansion in the wire be propagated correctly to the SiO2? Are my settings correct? (ignore the electric current). – alifornia Sep 7 '13 at 7:06
• (1) Yes, but see the updated answer. (2) Yes: displacement (and total strain) continuity at the interface will cause stresses in both materials. Are your settings correct? It's impossible to answer: please understand that without drawings, dimensions, detailed description of physical constraints no sensible judgment is possible. However some points to think about: why expansion only in copper? What are the physical constraints that corresponds to the fixed boundary of the insulation? – Stefano M Sep 8 '13 at 21:08
• I appreciate your help. I'm still fuzzy how I should set the boundaries in my solid mechanics stress-strain analysis (which ones should be fixed and which ones should be free). I have to configurations in my mind and not sure which one is correct (1) Fixing the boundary of the whole domain (i.e. only surrounding SiO2) (2) Fixing the boundary of each domain separately (i.e. fixing the sides of copper wire as well as the sides of SiO2). I'm solving the stress-strain equation in whole domain and hoping to get correct results as you said displacement (strain) is treated continuously. – alifornia Sep 18 '13 at 1:31
• (1) and (2) correspond to different physical situations. As said above it is impossible for to give you (especially on a comp. science site) sound advice. Try to imagine a physical experiment, with measurable quantities, that could help you to choose the correct b.c. – Stefano M Sep 24 '13 at 6:07