Solid-Shell Coupling in Heat Transfer Analysis
Solid-Shell Coupling in Heat Transfer Analysis
(OP)
Hi All
I was wndering if anybody could answer the following. I am performing a transient heat transfer analysis, and wish to include the influence of a thin film surface coating on the thermal conduction which has a significantly lower conductivity. I am modelling the heat transfer via a surface convection, and wish to model the coating with axisymmetric shells and the bulk material as a 2D axisymmetric body. Therefore I 'tie' a shell surface to a solid surface. However, I have discovered that for a heat conduction problem, this only works of there is 1 integration point specified through the shell thickiness. If this is the case, there is no conductivity through the shell, and therefore no temperature gradient through the shell, resulting in a step change at the shell solid interface proprotional only to the convection, and not the shell conductivity as well. I summise the requirement for 1 intgration point is such that ABAQUS knows which nodal temperature value to 'tie' to the solid (as the number of nodal temps that are possible through a heat transfer shell is equal to the number of integration points). Does anybody know how to get around this problem without modelling the coating with continuum elements.
Thanks
Brent Fillery
I was wndering if anybody could answer the following. I am performing a transient heat transfer analysis, and wish to include the influence of a thin film surface coating on the thermal conduction which has a significantly lower conductivity. I am modelling the heat transfer via a surface convection, and wish to model the coating with axisymmetric shells and the bulk material as a 2D axisymmetric body. Therefore I 'tie' a shell surface to a solid surface. However, I have discovered that for a heat conduction problem, this only works of there is 1 integration point specified through the shell thickiness. If this is the case, there is no conductivity through the shell, and therefore no temperature gradient through the shell, resulting in a step change at the shell solid interface proprotional only to the convection, and not the shell conductivity as well. I summise the requirement for 1 intgration point is such that ABAQUS knows which nodal temperature value to 'tie' to the solid (as the number of nodal temps that are possible through a heat transfer shell is equal to the number of integration points). Does anybody know how to get around this problem without modelling the coating with continuum elements.
Thanks
Brent Fillery





RE: Solid-Shell Coupling in Heat Transfer Analysis
I have done some extensive reading and believe that the above can be achieved by ensuring the bottom shell surface is adjacent to the solid surface i.e. NT11.
Can anybody confirm this?
However, I am still trying without success to prescribed an initial temperature field to the shell such that all shells sections have the same inital temperature. If I just issue a predefined field that is constant throughout the section, only the NT11 section sees this definition. Anybody know how to attempt to change this?
Regards
bfillery
RE: Solid-Shell Coupling in Heat Transfer Analysis
"There are a few workarounds:
1) Use a single integration point through thickness. The downside being that you will not pick up on any through thickness variation in temperature
2) Use *EQUATION to link all the appropriate degrees of freedom. The downside being that you need a matching mesh.
3) You could try using a *GAP CONDUCTANCE. With this option you define conductance against distance between surfaces. If you use a high conductance this would simulate perfect heat transfer between the shell and solid."
If you have problems then just use 2D axisymetric elements everywhere, even for the thin shell region you had.
corus
RE: Solid-Shell Coupling in Heat Transfer Analysis
Any idea on how to specify a uniform initial temperature through the shell section. If I issue the predefined field + temperature + constant through thickness, it only specifies the initial condition to NT11, not any other sections that arise due to the integration scheme (i.e. NT12,NT13...)?
bfillery
RE: Solid-Shell Coupling in Heat Transfer Analysis
As I said if you use 2D hex elements everywhere then this problem won't arise. If the elements will be very thin then don't worry about aspect ratios or any crap like that. Try and make a smooth transition in your mesh though away from the thin elements. If you have a severe transient then you'd need thinner elements at the face where major changes in dT/dt occur anyway.
corus
RE: Solid-Shell Coupling in Heat Transfer Analysis
I have found away to correctly model heat transfer within shell elements, at least in 6-6.
Firstly, in the section information for the shell, set in the advanced options that the temperature is to have a piece wise linear variation over a number of values corresponding to the number of section points in each layer. Secondly, when defining initial temperature, the section variation is defined as being at beam or shell temperature points, with the number again corresponding to the number in each layer etc.
Hope this helps for the future
bfillery