What to expect from CFX
 

Hello fellow CFD engineers,

I am in the process of modeling a water submreged impinging jet with D= 6.35 mm and inlet velocity of 2.01. I already have experimental data obtained from PIV.

My question is:

how close should my Ansys data can get to the real experiment. so far I am getting the same trend but the velocities has 0.1 difference and it gets more near the wall close to0.3 m/s difference.

should i keep trying to get more accurate results or this amount of error is expected in computer modeling??

I will appreciate any imput.... thank you in advance...

Fahad

Hi -

How close you get depends on too many factors to list here. Your simulation seems manageable - a CFD platform should be able to accurately predict the flow.

The Journal of Fluids Engineering provides a good explanation of predicting discretization errors (skip to page 3):
http://journaltool.asme.org/Template...umAccuracy.pdf

Discretization errors are the greatest concern (if terms of errors) to a CFD modeler. Discretization errors are those that occur as a result of modeling the governing flow equations as algebraic expressions in a discrete space-time domain. Discretization errors should approach zero as the grid is resolved (i.e., as more grid points are generated and the solution becomes grid-independent). However, discretization errors also depend on grid quality (e.g., aspect ratio, orthogonality, skew). A well-refined grid is not necessarily a high quality grid.

Other errors:

Physical approximation errors (e.g., simplification of the fluid as an ideal gas).
Computer round-off errors (i.e., what accuracy does your computer store floating point numbers at - this is usually negligible if you run the simulation in Double Precision mode).
Iterative convergence error (i.e., the simulation has to stop eventually - how many iterations did you run and was it long enough to establish the flow - this can be decreased by running the simulation until it stops converging monotonically and the residuals fluctuate periodically for a reasonable amount of time).
Usage errors (i.e., running a turbulent simulation as laminar).

Hope this helps.

Also, do a sensitivity analysis on the grid, convergence residual, domain size, turbulence model, timestep (if applicable), and other factors important to your simulation (e.g., freestream turbulence intensity).

In its most basic form, a sensitivity analysis involves tweaking one thing (e.g., turbulence model) while keeping everything else constant and observing the effect on solution accuracy (for example, a skin friction graph) and time.

Thank you Very much
 

Dear Josh,

Thank you very much for your thorough answer. it did shed the light on a lot of ideas for me to consider.

I think i should tackle the results error step by step.

I am using tetrahedral mesh with high relevance to center and 30 angular resolution and it look pretty uniform with not a lot of skewness. i have 1.5 million nodes for the entire geometry concentrated mostly around the center.

I am not sure how to run double precision on CFX I know fluent has an option at start up. I should look that up on the manual.

I am currently running 130 iterations and it seem that the residuals get close to 10E4 , I think i should set it up to 200 and let it stop by itself.

the turbulence model that I have tried are K-e and K-w ( both with automatic values) and SST

my least accurate data are from the near wall line when when it is close to the stagnation point ( 0.35 m/s below the experimental). the other lines are reasonably close ( 0.1 m/s ) higher than the experimental data.

I will try to build a report with my finding and do a sensitivity analysis as you suggested.

Thank you again for your quick and thorough feedback :)

Fahad

You're very welcome for the response. The people on this forum have been extremely helpful to me and I feel obligated to help others to the best of my abilities.

1) A tetrahedral mesh is nice because it is quick and robust. However, it's best to use a structured hexahedral mesh in the boundary layers of the wall as an unstructured mesh can cause large discretization errors in the boundary layer. Your geometry looks relatively simple - do you know how to use ICEM-CFD? It can generate very nice structured meshes. If not, CFX's mesh program can create a structured boundary layer (inflation error).

2) ICEM-CFD has the capabilities to provide histograms of your mesh quality. If you're not using ICEM, Post has a mesh calculator that has a good amount of mesh quality factors to export.

3) To run double precision, when you define your run in Solver, there's a little check box reading "Double Precision".

4) If you're doing a quantitative study, you're going to want to converge to a lower residual than 10E-4. Converge the RMS residuals to at least 1E-5 (10^-5). Or, better yet, set the residual very low (say, 1E-10) and let the solution converge monotonically (i.e., in a straight, downward line). Eventually, the line will begin fluctuating at a lower residual. Let it continue to fluctuate for some time until you notice it's somewhat periodic, then stop the simulation manually.

5) Two-equation turbulence models are a good choice, but what do you expect the flow to do? Is there a lot of swirl? Do you expect vortices? You should read the Help file section on turbulence models for a good introduction to each of those models. k-e is popular, but requires sufficient refinement for accurate boundary layer capturing. k-w is good for near-wall treatment, but suffers from sensitivity to freestream turbulence and inlet conditions. SST is popular, but also has the usual deficiencies common to all RANS turbulence models.

6) What's your maximum y+ value at the wall? Which turbulence model gives you the best results?

Good luck!

Hi Josh,

You have some good answers here. I have been meaning to write a FAQ for the question "My simulation is not very accurate" and your posts is a pretty good start. It would be great if you could write a FAQ - http://www.cfd-online.com/Wiki/Ansys_FAQ

Thanks, Glenn. That means a lot coming from a CFD expert. I'll get to it ASAP.

School is in session
 

Thank you Josh you are giving me pearls here. I am , as you can tell , new to CFD.

1) I have not tried structural mesh yet but I will implement your meshing ideas ASAP

2) I have not paid attention to the The double precision box on CFX I used to see it on fluent. I will make sure to check it this time on CFX Solver. I stopped using Fluent because of the element number limitation MAX 1/2 a million node for academic version. CFX gives 2 milllions.

3) I will diffidently run it with very low residual I will try 1E-10 and stop the solution after it stabilizes

4) I took Glen's Advice from 2 days ago and used SST model and it gave me the best results so far I am attaching a picture with last night results. Thank you Glen.

5) I have not paid attention to my y+ value i will give you some feedback on that next time.

Thank you again Josh for your valuable comments. you really added some significant ideas to my CFD experience. :)

Fahad

You're very welcome. I, too, am a fan of the SST model. I use it for external aerodynamics applications and find it predicts separation very well.

Good luck.