Fully coupled thermal-stress analysis in Abaqus/Standard- equations

[MPa94]

Hi,

I'm simulating a fully coupled thermal-stress problem with linear elastic material in Abaqus/Standard and comparing the results with my own implementation of the same problem in FEniCSx. The weak form in FEniCSx has been derived using the balance equations mentioned in the paper Farhat et al. (1991) Link, which are:

(Screenshot of the paper)

where

σ=2με+λtr(ε)I−α(3λ+2μ)(θ−θ[sub]0[/sub])I and ε=1/2(grad(u)+grad(u)[sup]T[/sup]). Details on other parameters are fairly standard and can be found in the paper. My FEniCSx results (both temperature and displacement fields) match to those of Abaqus only after I neglect the strain rate term in the heat conduction equation (α(3λ+2μ)θ[sub]0[/sub]tr(ε_dot)) thereby uncoupling the displacement from temperature change. This is in contradiction the Abaqus' analysis description which states that both fields are fully coupled.

Does anyone know which coupled equations does Abaqus/Standard implement for fully coupled thermal-stress analysis? Especially the heat conduction equation? In the Abaqus theory manual I could only find the uncoupled heat conduction equation (link) but no equations on fully coupled thermal-stress analysis. However there is a description of the fully coupled thermal-stress analysis procedure in the Abaqus user manual (link).

I also tried to model a simple linear thermoelastic 2D-"Beam" fixed at left side and "pulled" using displacement-BC on the right side. The initial temperature was defined as a predefined field (value: 20 in Initial Step and the value is calculated in subsequent step). I am not modelling the beam with plasticity.

See Screenshot on deformed and original state. The time dependent deformation is not resulting in any change in temperature.

Anyone has any idea as to what I'm doing wrong? All relevant material parameters and model constants (Absolute temperature and Stefan-Boltzmann constants) are defined. I have attached the inp file.

Thank you for any leads.
MPa

 

[FEA way]

You won't find more information about the theory behind Abaqus procedures than what's available in the documentation. Maybe check the equations used by open-source solver CalculiX which is based on Abaqus.

Heat in this procedure doesn't just automatically come from the deformation, you have to include proper effects leading to heat generation in the model - typically it's inelastic or frictional heat generation.

 

[MPa94]

Thanks for the tip on CalculiX, will check it out.

As per the heat conduction equation, temperature should change due to a non-zero deformation-rate right? I wonder why Abaqus has just included heat generation due to inelastic deformation.

 

[FEA way]

This is just how the perfect elasticity model works. The energy due to the deformation is stored as a strain energy (elastic potential energy) and then, upon unloading, this whole energy is released as the body completely regains its original shape. Of course, pretty much nothing is 100% elastic and in practice, the inelastic (permanent) deformation involves the dissipation of energy in the form of heat. But this has to be included in the simulation as a plasticity model. Same with rate dependence - it can be added to plasticity or elasticity (as viscoelasticity) but is not accounted for by default.

 

[MPa94]

For a purely elastic case, I totally agree with you. But if we include thermoelasticity, then the above mentioned heat conduction equation comes into play. A non-zero strain rate should indeed result in change in temperature, right? This could very well be reversible due to elastic deformation.

 

[MPa94]

Solved the issue. It lied in the fact that I did not scale the units properly. Density had to be in tonne/mm^3 if E-Module is in MPa. Save goes for specific heat capacity and heat conductivity, etc..

 

[FEA way]

Ok, but what do you mean by "solved" - how did the results change ? I still wouldn’t expect any temperature change here.

 

[MPa94]

In Abaqus I really don't see any change in temperature. But in FEniCSx, there is a reduction in temperature in the order of 10^(-2). Which could be due to the couple term. See FEniCSx result:

Since the wrong units were implemented in both Abaqus and FEniCSx, they should have given the same "wrong" results. Therefore I believe that Abaqus is completely neglecting the couple-term in the heat conduction equation.

 

[FEA way]

Yes, Abaqus just doesn’t take this into account by default since it’s usually insignificant. Moreover, there are no built-in ready-made features to model this. You would need a Fortran subroutine like HETVAL. It can be used to define internal heat generation in a material due to various effects accessed usually via state variables. There’s also the UMATHT subroutine but it requires the definition of the constitutive thermal behavior as well.