Different time step for heat transfer and fluid flow possible ?
 

Hello,
i have trouble with the conjugate heat transfer.
My analysis of a gas-turbine is time dependent. For the time step i choose manually 0.0001s and after 100 iterations (0.01s) the fluid flow converged.
But the temperatures of the solid parts change only a little bit.
Start condition: 300 K for the solid parts.

Example: The temperature of the fluid is 900 K and the temperature of the turbine-blade is only 320 K.

Problem: One iteration (0.0001s) takes about 11 minutes.
So the calculations can take "weeks" until the steady temperatures established.

How can i manage the problem of different time steps for the fluid flow and the temperature of solid parts until established ?

I can set initial conditions for the solid start temperatures but only speculative values.

For the result i need accurate temperature distributions in the solid parts.

Any ideas ?

Hi, You might want:

Set the higher value of time step after 0.01s. It is possible to set it as a variable.

Another thing you can use Flow Freezing after your 100 iterations. That means it will freeze the fluid flow (it's convenged anyways) and calculate heat transfer. This will be quicker because fluid is freezed. You can specify how many iterations it's freezed and unfreezed.

Hi Sven,

sesq is right, that should speed up your solver time. May I ask why you want to calculate fully transient?
You can also start steady state and then switch to transient with steady state results as initial conditions. This is usefull if you consider the initial flow development to be very quick and not of high interest for your calculation. Then the longer initial flow development in a transient calculation can be shortened to the main task you look into in the transient calculation.
For example if you are looking at the transient heating up of the blades as your ultimate goal of the simulation. Then a steady state calculation for an initial condition is wise as the initial flow development will probably not take more than 1-2 seconds until the flow is established around the blades but calculating 1-2 seconds in 0.01 second steps or smaller takes quite some time. You can reset the initial solid temperatures to your 320K and calculate from there with established flow from the beginning, larger time steps and the use of flow freezing.

I hope this helps,
Boris

Hi guys,

thanks for your answers. They will be very helpful.

The magic word seems: "flow freezing" and set higher time steps after flow is established.

For my understanding:

With flow freezing you stop the calculations for the flow like velocity, pressure mass flow and so on BUT NOT for the existing HEAT in the system right ?
So with a higher time step the parts have enough time to heat up
(heat capacity).

Hopefully i can change the time step in the solver settings after a complete transient analyses and set "flow freezing" to calculate on for heat transfer.

I set initial conditions for temperatures but only rough estimations.

For the turbine wheel i set 700 K but it can be 200 K more or less.
Especially the distribution at the blade tips is important.


marginal note:

36 hours for one transient simulation with around 1.900.000 cells until flow established. Running on a 64-Bit CPU Intel i5 2,8 GHz and 8 GB main memory :eek: That's a horror.


P.S.
I set total pressure for the inlet and environment pressure for the outlet as a boundary condition. Also a mass flow for the fuel in the combustor.

Goals for the convergence are mass flow rate at the inlet and outlet.

Perhaps that's the reason for the very long calculation time.
I read in the forum the best way is to set a mass flow or volume flow rate at the inlet, but that's not possible for my analyses.
No estimations of values are available for the new parts.
That's the reason why i use FloEFD.


Best regards and thanks

Sven

Hi Sven,
yes, flow freezing really freezes the flow beeing recalculated each iteration but the heat transfer into the flow and out of the system is assumed to be the same for each time step as it is at the moment of the freezing. So the solids get cooled or heated (depending on the fluid temperature. Now if you start and stop the freezing periodically then the flow gets updated every now and then for more accuracy.

Yes, you can change the settings for flow freezing and manual time step during the solver run in the calculation control options in the solver monitor.

Well 36 hours is not that bad. I had once a calculation running for a week in transient where the task was 2 hours in real time but the time steps cannot be too big of course and there was a lot happening in the flow.
Which CPU generation is the i5? I know it is not always possible but the latest CPU generation can often give a 20% speed increase compared to 1-2 generations before.

The goals are not the reason for the long calculation time as they are not important in a transient analysis. The transient goal is usually to see the transient behavior not a converged simulation.
Well it can come to instabilities with two pressure openings if you use rotation but that's hard to tell from what you described.

But why are you using transient? Is there any information you are trying to get out of the simulation that needs a transient calculation?

Boris

Hey Boris,
thanks for your answer.
The reason for choose a transient analyses is simple.
I try to validate a "half" tutorial from the following link:
Micro-Turbine in FloEFD

But until now it is impossible for me to validate these example.
Until fourty iterations all values looks good but after fourty iterations the values run away to the basement... :confused:
I need these example for my own construction.

Greatest problem: No contact informations for the authors are available and no helpful informations from mentor graphics.

Only these "half" article. To validate i need exact informations for the boundary conditions, initial conditions and the solver settings.



Greetings
Sven

Hi Sven,

you are lucky, the author is a colleague of mine and I am from Mentor Graphics.
Please write me a private message with information to what product you use exactly and who you have contacted at Mentor Graphics. If you send me your email address I should be able to provide you with the model as it was setup by my colleague.

Boris

Hello Boris,
thanks for your answer. You have a private message.

Sven