Transient: Domain Timescale Factor
 

Greetings all,
I'm doing a cool down simulation where It takes many days to cool down a geometry (295K down to 4K)
The fluids equations must be solved on a small time scale (~0.01s) where the solids can be solved on much higher timescales (100+ seconds). What I have been doing is freezing the fluids equations, then solving the energy equations @ 100+second timesteps. Using constant properties for the cool down gas. Unfortunately It seems the fluid balancing (there are 98 parallel routes) changes during the cooldown once temperatures start getting low.

So what I'm wondering is:
Can I use the domain solver control: Timescale Factor = 10000 for the solid domains during a transient simulation. The option is there, so I will test it to see what happens, and report back. Documentation seems to hint at Yes, but it is a bit unclear. CFX Pre Users Guide Section 13.4.10.1.
Would this be roughly the same as reducing the specific heat of the solid materials by a factor of 10000? Would Specific Heat reduction of the solids be an alternative option if the timescale factor does not work?
Approximate solution is fine, It should be better than my frozen fluid equations solution, which I can use for comparison.

I think your frozen fluids approach is probably the best one.

You cannot use time scale factors in transient simulations (to my knowledge anyway).

It is effectively changing the thermal capacitance w/o messing around with the material details.

Do you do this manually? Or do you make use of Fortran?

Thanks for the responses all,

So, reporting back, it does seem to work. Yes, the domain timescale factor works for the transient simulations (It is set in each domain). Results track along with with my frozen fluids approach.
It is much less efficient though, after an overnight run on 5 machines, it is only 1.3 equivalent hours into the 130 hour cool down. So It isn't practical in this case, and frozen fluids seems to be the best. (Quickest anyways.)

I do the frozen fluid equations manually: using the expert parameter: solve fluids = f.
What benefit would Fortran offer? I thought about if it would be possible to change this expert parameter every so often to true, to update the fluid field. I would have to change the time steps as well (much shorter) during this time, then increase again when solving only energy equations. I did this a few times on the fly in solver manager manually during the cooldown. Could that be automated?

In CFX-10.0 I had a fortran code which did this automatically. That can help you overnight.
The code was able to switch off fluids for a certain timestep so only energy and scalar were solved using a large timestep.
It was a buoyancy driven flow where the coupling was quite strong. So the allowable timestep increase when fluids were skipped was only a factor 3. Otherwise the flow would deviate too much.
Maybe in your case the coupling is less strong allowing a larger time step increase. I can share the old Fortran. Alternatively ask ANSYS for a more recent version.

That sounds very interesting. My flow won't deviate too much. I would like to take a look at the fortran. I have never used fortran with CFX, so that will be new to me, but could prove very useful. Thank you, I'll PM my email.