Hi all, I model cooled turbine blade. There are two fluid domains (flows inside and outside blade) and solid domain with heat conductivity. When I solve steady-state problem I use three time scales (individual for every domain) and have a good convergence and calculation time. When I model transient I obligated to use only one time step for all domains and I choose smallest time step (estimated for fast flow outside blade). Solid domain is slow heated so time duration is big enough. Therefore total amount of time steps is enormous and calculation time is huge! Has CFX any ways to set different time steps for various domains? Do you know any approaches to reduce calculation time? May be submodeling or FSI (CFX for outside flow and ANSYS Thermal for solid and outside flow)? Thanks a lot for your advices.

Hi,

Yes, CFX can do different timesteps for different domains in steady-state simulations. You want to set the "solid timescale factor" CCL object. This is a standard trick to accelerate CHT simulations.

Glenn Horrocks

Thanks Glenn. But I need accelerate Transient simulation (please see first post)

Hi,

Some comments:

1) In the solid the only equation to be solved is temperature and it much easier than fluid domains as the equation is linear and there is only one variable (fluid domains usually have 7 variables of more). This means that unless you have a huge amount of mesh points the solid domain does not add much computational load to the simulation.

2) Can the simulation be decoupled somehow? Maybe get heat transfer coefficients from a fluid simulation and put them as boundaries for a heat transfer simulation?

3) I guess the fluid flow sorts itself out quickly but the solid stuff takes much longer. You can solve the coupled thing until the fluid has reached steady state, then turn the fluids solver off and just continue with the heat solver. This will evolve the fluid/solid system in temperature but will not couple back to the fluid system. If the coupling is weak you could just turn the fluids solver on for just a short time and off for a while. Use the expert parameter "solve fluids = t or f" to do this.

Glenn Horrocks

Hi Georg! What kind of interface (for fluid-solid surface) do you use in your model?