[chiragsvnit]

Today I was reading the CFX documentation and the following text has raised my eyebrow "The Turbulence Numerics options are First Order and High Resolution. The First Order option uses Upwind advection and the First Order Backward Euler transient scheme. The High Resolution option uses High Resolution advection and the High Resolution transient scheme."
I am trying to find the answers of some questions such as: (1) Even in steady state simulation, CFX solves equations, mainly turbulent, in time domain (using First Order Backward Euler scheme), isn’t it? (2) I am unable to find the formulation (time domain discretized form of turbulent equation) of High Resolution transient scheme. (3) Is there any relation among inner loop iteration numbers generally shown in *’out file of Linear Solution and Physical/Auto Time Scale in CFX?
If anybody knows about it and would like to help me out, I would be thankful.
Thank you in advance.
Chirag.

[highorder_cfd]

Originally Posted by chiragsvnit

Today I was reading the CFX documentation and the following text has raised my eyebrow "The Turbulence Numerics options are First Order and High Resolution. The First Order option uses Upwind advection and the First Order Backward Euler transient scheme. The High Resolution option uses High Resolution advection and the High Resolution transient scheme."
I am trying to find the answers of some questions such as: (1) Even in steady state simulation, CFX solves equations, mainly turbulent, in time domain (using First Order Backward Euler scheme), isn’t it? (2) I am unable to find the formulation (time domain discretized form of turbulent equation) of High Resolution transient scheme. (3) Is there any relation among inner loop iteration numbers generally shown in *’out file of Linear Solution and Physical/Auto Time Scale in CFX?
If anybody knows about it and would like to help me out, I would be thankful.
Thank you in advance.
Chirag.

Hi


(1) Even in steady state simulation, CFX solves equations, mainly turbulent, in time domain (using First Order Backward Euler scheme), isn’t it?

Yes, in CFX the solution is advanced till the steady state condition through a pseudo-transient.

(2) I am unable to find the formulation (time domain discretized form of turbulent equation) of High Resolution transient scheme.

The High Resolution transient scheme uses the second order backward Euler scheme wherever and whenever possible and reverts to the first order backward Euler scheme when required to maintain a bounded solution.

(3) Is there any relation among inner loop iteration numbers generally shown in *’out file of Linear Solution and Physical/Auto Time Scale in CFX?

The time step needs to be representative of the physical phenomena you are simulating, thus it must be of proper size (not too large to ensure accurate solution, not too small...or it will take forever to converge).

Usually, you the time step size should be of size that ensures the iteration to converge in around 5-10 coefficient loops (I read that it is better to reduce the time step size that increasing the coefficient loops more than 10)

[chiragsvnit]

Thank you for your Reply.
Second question is different.
I am looking for the CFX implemented formulation for Turbulence numeric for high resolution scheme. Because I want to understand that.

The reason is:
I have conducted two simulations on hydrofoil with water velocity was 20 m/s. Simulation-1: Turbulence numeric-First order.
simulation-2: Turbulence numeric-High resolution.
The simulation-2 was diverged and failed while simulation-1 was converged perfectly without any trouble. I would like to understand why is it so?

Please do not mix up with Advection schemes. I am not talking about advection scheme.

Third question: I have asked different point. Is there any relation between the numbers generally shown in the column of Linear solution and fluid timescale control option in CFX? I have attached figures for both.

[highorder_cfd]

>I have conducted two simulations on hydrofoil with water velocity was 20 >m/s. Simulation-1: Turbulence numeric-First order.
>simulation-2: Turbulence numeric-High resolution.
>The simulation-2 was diverged and failed while simulation-1 was converged >perfectly without any trouble. I would like to understand why is it so?

>Please do not mix up with Advection schemes. I am not talking about >advection scheme.

This is what CFX does when you set the Turbulence Numerics

20.1.1.2. Turbulence Numerics

The Turbulence Numerics options are First Order and High Resolution. The First Order option uses Upwind advection and the First Order Backward Euler transient scheme. The High Resolution option uses High Resolution advection and the High Resolution transient scheme.

https://www.sharcnet.ca/Software/Ans.../CHDFCJED.html

To sum up

Turb. Num. First Order =Upwind (1st order) for the advection and 1st Order BE for time

Turb. Num. First Order =High resolution (2nd order) for the advection and 2st Order BE for time if possible, otherwise 1st order BE for the time (this is called High Resolution transient scheme)

https://www.sharcnet.ca/Software/Ans....html#i1313650

Lower is the accuracy (higher numerical dissipation), better the robustness of the scheme.


>Third question: I have asked different point. Is there any relation between the numbers generally shown in the column of Linear solution and fluid timescale control >option in CFX? I have attached figures for both.

If you keep the same parameters used to solve the linear system, a smaller time step should ensure a larger drop of the linear residuals/a same drop of the residual should be reached in a lower number of coefficient loops.