How will you know if you got an acceptable result during iteration? Thanks!

# Acceptable Result

- 75 Views
- Last Post 15 April 2018
- Topic Is Solved

If the iteration converges to the final time, that represents an equilibrium solution for static or steady-state models. If the iteration stops before that, there is a clear indication that there is a problem that needs attention in the model.

If the solver converges to the final time, the best practice is to perform a mesh refinement study. Duplicate the system with the initial coarse mesh with element size s3, and refine the mesh with elements that are smaller in size (s2) by a factor of between 1.3 and 2.0 in the areas of high gradient, or in the areas critical for accuracy in the model, and get a second solution. Observe the change in the result quantity. Duplicate the system and repeat the mesh refinement so the element size is s1 and get a third solution. Plot the result quantity of these three systems vs the element size.

Mesh refinement studies are done in both Structural and CFD models. Here is a discussion with more detail. A mesh refinement study tells you if the numerical errors of discretizing and solving the model are acceptable. You might show that the numerical error is reduced to less than 1%, but later learn that one of the material properties was incorrect by a factor of 10! That is where validation needs to be done.

Validation is the process of obtaining a measurement of the physical system to compare with the simulation result.

Thank you! My iterations says:

....

reversed flow in 19 faces on pressure-outlet 8.

195 1.2657e-01 4.4848e-03 3.6785e-03 1.1488e-06 1.1585e-02 1.5845e-02 0:00:00 5

reversed flow in 19 faces on pressure-outlet 8.

196 1.2434e-01 4.4962e-03 3.7319e-03 1.1541e-06 1.1549e-02 1.5610e-02 0:00:00 4

reversed flow in 20 faces on pressure-outlet 8.

197 1.2783e-01 4.4833e-03 3.7615e-03 1.1756e-06 1.1460e-02 1.5387e-02 0:00:01 3

reversed flow in 20 faces on pressure-outlet 8.

198 1.3009e-01 4.4894e-03 3.7951e-03 1.1746e-06 1.1333e-02 1.5115e-02 0:00:00 2

reversed flow in 20 faces on pressure-outlet 8.

iter continuity x-velocity y-velocity energy k epsilon time/iter

199 1.2936e-01 4.5001e-03 3.8368e-03 1.1769e-06 1.1157e-02 1.4724e-02 0:00:00 1

reversed flow in 20 faces on pressure-outlet 8.

Radiosity converged after 3 iterations

Final radiosity residual = 2.954131e-05

200 1.3033e-01 4.4930e-03 3.8676e-03 1.1660e-06 1.0959e-02 1.4360e-02 0:00:00 0

Registering S2s, ("D:\ANSYS\x_files\dp0\FFF\Fluent\FFF.s2s.gz")

Writing data to D:\ANSYS\x_files\dp0\FFF\Fluent\FFF.ip ...

x-coord

y-coord

pressure

x-velocity

y-velocity

temperature

k

epsilon

hyb_init-0

hyb_init-1

Done.

Calculation complete.

....

Attached also is the scaled residual graph.

Any thoughts, I will do the size refinement as you suggests and I will observe changes in the iteration. Thanks you!

And therefore, a converging residual graph indicates a good simulation? Thanks you!

I commend you for your interest in how to use ANSYS to obtain valid results. I recommend you take the free course on edX.org, "A Hands-on Introduction to Engineering Simulations" developed by Cornell University. It takes you through four modules that lay a foundation of understanding and show you techniques to obtain valid results in your models. Module 5 shows you how to simulate the 2D airflow over a wing profile, and the methods used to obtain a converged solution. I have taken this course, and that was my first exposure to CFD.

I believe your model is not sufficiently converged. You should run iterations until the residuals are below 1e-3. In the course, it was recommended to set the residuals even lower to 1e-6. There are also techniques to drive the residuals down using fewer iterations by setting some methods to first order for the initial few hundred iterations, because first order methods are stable while second order methods might lead to divergence. But after some amount of reduction in residual has occurred, change to second order methods because they converge faster than first order methods.

In the example of your roof in the open ground, the reversed flow messages may mean that your outlet boundary is too close to the disturbance in the flow you are trying to model with the roof. Double the distance to the downstream outlet and try again. If you still get the message, double the distance again. If this doesn't apply to the model you are working on, then you should attach the workbench archive file .wbpz so that the CFD experts can take a look.

Thank you so much for your patience in answering my questions. Rest assured that I fully comprehend your suggestions, you've been a great help!

##### Search

##### Change Language

##### Categories

##### This Weeks High Earners

- peteroznewman 59
- abenhadj 41
- kkanade 31
- zypresse91 10
- Francisco Guerra 7
- Raef.Kobeissi 7
- jj77 7
- shaheen wahab 6
- Jamessmp23 6
- Georgiro 6