equation and domain dependent timescale
hi there
i'm simulating a cht + fluid case and i need to be able to set three different timescales: one for the solids, one for the mom. and continuity eqs in the fluid and one for the energy equation in the fluid. now, how do i define the timescale for the energy equation in the fluid only? i know that such a thing can be done, according to the manual, but it has to be done by editing the ccl file. unfortunately the manual doesn't specify as to what the cclcode is supposed to look like. any ideas would be greatly appreciated. cheers 
Of course this only applies to steady state simulations.
The command you are looking for is "Solid Timescale factor". 
Thanks for the reply glenn. I'm afraid that doesn't do the trick. Specifying a timescale for the energy equation overwrites anything i set for solid timescales. I need to be able to set the energy timescale for the fluid domain only.

I do not think you can set separate timescales for the momentum and energy equations in a fluid domain. At least I do not know a way of doing it. Once the momentum equations are converging you can usually massively increase the time scale (factors of 1000 or more are possible) and that means you accelerate the energy equation.
I have done many CHT simulations and the way I always do it is using a smallish time step in the fluid to start off, and increasing the time scale as the flow converges; and a large solid time scale factor so the solid converges quickly. This works pretty well for me. 
According to the manual there is a way, for this exact situation in fact. It just doesn't specify how to do it :) i'll ask support. Thanks for your answers!

Quote:
Did you found a solution for this problem? Kyriakos 
Quote:
I have the same question too, do you find cel to do the domain dependent timescale? Qu 
you can basically just copy the structure from the actual solver control: add a "solver control" item in your domain. a subitem could then be "convergence control" to set domain specific time scales. (this can be done in cfx pre already by activating beta features).
if you want to specify equation classes directly then simply add a subitem to your "solver control" item called "equation class: energy" (for example) and then add another "convergence control" item into that one. the structure basically looks like this: domain > solver control > convergence control > timescale control etc. > equation class: energy > convergence control > timescale control etc. 
Quote:

if you are looking for a steadystate solution, then you can use as many and as different timescales as you want. they only help or hinder your convergence, but at convergence the solution should always be the same. if it's not, then there's something else wrong. make sure you check whether your simulations are actually converged. also make sure you check the imbalances of your energy equation since it's proper convergence can take forever when using small timescales ...

Quote:
To my knowledge, all the simulations had been converged, I had checked RMS, imbalances and monitors. All the RMS were nearly below 1e5, the imbalances of T,P,and V were extremely closed to zero, and the T, V of monitors were unchanged for many time steps before the solver stopped. I doubt if the improper boundary condition caused the different results. My case is mainly about a natural convection heat transfer in a infinite space. I had set all surrounding boundary to opening boundary and opening pressure. someone told me all pressure boundary may cause a initial value dependent result. However, in may case, The initial value did not influence the result, but the timescales did,just as I described in last message. Have you ever did a similar simulation about a natural convection heat transfer in a infinite space? Could you give me some advise? Thank you for discussion. 
It is a known issue that steady state simulations in general can have problems converging with small time steps and converge better when the time step is increased. When the time step is significantly smaller than the turbulent fluctuations in the physical flow then the solver starts to resolve these fluctuations and the simulation is no longer steady state  and hence your difficulties in convergence.

All times are GMT 4. The time now is 20:47. 