Transient Endstate conditions
 

Hello Community,
the CHT-Simulation I am doing needs apparently a very long time to reach the steady state condition. Although physically not very complex, the model has some very fine and some very large regions.
For the flow through tight gaps and a high rotation speed of >2000rpm I need timesteps of around 0.002s at least to reach a convergence lower than 5e-5, which I assume as statisfying.
Problematic is, the simulation time might be more than 200s. With 5 loops per step I would get 500,000 iterations, which would take a tiny little bit too long.

Since I have some good results from my steady state, can I use these results as a final (not initial) codition?

I would expect the transient simulation to converge faster and maybe use timesteps of about 0.1 secs.

Cheers and thank you for your kind help
Marcel

This big range of time scales between the solid and fluid parts of a simulation is common for CHT simulations. That is why the "Solid Timescale Factor" option is added for steady state simulations. It allows you to use a large time step in the solid domains and a small time step in the fluid domains, and should allow you to converge the entire simulation in the same amount of iterations as it takes to converge the fluid domains alone.

My comment is don't be shy when using solid time scale factor. Factors of 100 or 1000 usually work fine. As the equations being modelled the solid domain are simple and linear they are quite numerically stable and can handle aggressively large time steps.

Thank you for your info, indeed, increasing the solid timescale factor was necessary in one of the simulated models (which differ slightly) to converge quickly.

But I don't know if you understood the issue. It's really that I want to temperatures after 10s, 50s, 100s, 200s, but I need tiny timesteps. So is it possible to make advantage of the steady solution in order to speed up my transient?
I know it's possible to use a converged steady state as an initial guess, but I rather want the opposite: as an end guess :)

If you want to model a true transient then your only choice is to model using whatever time step a transient simulation requires.

But often you can be a bit clever about it. Does the flow field fully develop quickly and the only thing which evolves is the fluid thermal field? If so then you can stop the momentum equations and just do the thermal equations. Or can the fluid side be replaced with a convection boundary condition? Hopefully there is some form of simplification which can be done to accelerate things.

A convection simplification is not possible, since the geometry is being optimized to cool the solids.

I guess the flow field doesnt change significantly, after about 0.5s it is a bit unstable and monitored velocity is shifiting in a 10% range, but this could due to convergence issues. Also I wonder if the buoyance is a strong factor.

Yet I don't know how to tell the solver not to solve the momentum equations any further? And would this method help to solve the flow field only every 10th timestep or so?

Cheers

You can use expert parameters to turn the momentum, turbulence or any other equation off. The effect of this is that the equation you turn off is not solved and the solution field of that variable remains fixed. So if your fluid field has established a steady state flow (in the momentum equations, but not thermal steady state) then turn the momentum equations off and the solver will proceed MUCH quicker.

Thank you for the useful advice.
Since I see only the possibility to switch between true and false, is there an easy way to set the parameters depending on the timestep?
Then I would be able to update the flowfield every 0.1s or so, or do you think the every ongoing changes because of increasing heat and buoyancy changes are neglectable? It is not really comfortable to sit and watch the Monitor and do it manually every now and then.


Cheers
Marcel

? You do not use controls like turning whole equations on and off for fine-control of simulations. Is the flow field evolving with time of not? If it is evolving then you cannot use the approach I described to turn equations off. If it is not evolving then you can.

I understand your concerns about my dirty approach, but I'm interested in a practical, time efficient solution.

The flowfield is changing, at least to some extent, since the solid body is warming up and the heatflux to the fluid is increasing. But maybe this is negligible.
When observing the solver monitor, I see a slight sinusodial change in velocity. my monitored mass changes about 1/10,000 of the inflow, even thought the standard Pmass Imbalance is fluctuating between +10 and -10% (really no clue how that is calculated).

I just thought it made sense to solve to flow field every second or so for maybe 10 timesteps.

Is the velocity field changing at all? Your comment suggests it is changing about 0.01% which can probably be ignored. If the temperature does not affect your material properties (a viscosity or density a function of temperature) then you can probably turn the fluids equations off. No need to run them again every now and again as nothing changes.

But note you do not turn the thermal equations off. This means the temperature in the fluid can change even though the fluid field (velocity and pressure) is frozen.

Well the userpoint massFlow()@Opening suggest a round about zero change, but that doesn't mean the velocity or vectors in the fluid aren't changing.
I was thinking that with buoyancy model, the density of air must be changing and therefore move differently with increasing temperature. As a result I suppose the flow field would never be constant until steady state conditions are reached.

You seem to be confused about what steady state means. Steady state means that the conditions at any point in space do not change with time. There might be a flow velocity at a point, but if it is not changing then the flow is steady state. It does not matter if the flow is driven by buoyancy, forced convection or any other thing which pushes flow along. If it does not change it is steady state.

My point is - the fact there is buoyancy driven flow is irrelevant. It is whether it is changing with time at any location which is important.

Actually I hope I at least understood this basic concept when it comes to numerical fluid simulations :>

So my point is: Let's say I will reach steady state after about 300 s, which would take days since I need timesteps of about 0.001 s. This is I guess due to the fact, that heat spreads slowly in solids.
So it's an simplification with an error, to assume the flowfield won't change anymore, after about 1s simulation time. Of course it won't change much, the flow developed due to the roation of the solid, but the body is heating up, and every second a tiny bit more heat is transferred into the flow due to conduction, which should as a consequence, have effects on the flow (convection).
By updating the flowfield every now and then, I assume to reduce this error. However, the change in the flowfield from 62.001s to 62.003s and it's effect on the temperature of the solid is not visible. Am I making sense? :)

I see what you are saying now, and I understand why you are saying the flow will slowly evolve as the heat increases and the buoyant effects slowly increase.

So you could turn the fluids solver off and on to capture this, but it is a bit of a kludge. An alternative is the increasing heat transfer as the temperature increases is probably well described by a combination of convection and/or radiation. You might be able to model the solid in one simulation and the fluids as a separate simulation. The interface between the solid and fluid could be replaced with a convection and/or radiation boundary.

Thank you for the advice, but since I have many bodies with many fluid/solid interfaces I doubt it's a quick solution.
I guess the only way is to write a user function, if in fact, I want to turn the equations on and off automatically?

No, you can't do it with a user function. You need to change the CCL. The official way of doing this is by stopping and restarting the simulation or using "edit run in progress" in the solver manager. But you might be able to work out the command line to do it so you can automate it as I think it is just a command line thing to do it - but not a documented one.