CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   how to justify that my numerical predictions are correct (http://www.cfd-online.com/Forums/main/82258-how-justify-my-numerical-predictions-correct.html)

tushar November 22, 2010 02:55

how to justify that my numerical predictions are correct
 
how to justify that my numerical predictions are correct when i don't have experimental results. what kind of validation tests can be performed? thanks in advance.. :)

dandalf November 22, 2010 06:44

You could simulate a known flow pattern and compare with bench mark solutions.

Bench mark flow solutins can be found in,

Schafer, et al, "Bench maek computations of laminar flow around a cylinder" Notes on numerical fluid mechanics, 52, 547-566 (1996)

Oosterlee et al, "Benchmark Solutions for teh incompressible Navier-Stokes Equations in general co0ordinates on staggered grids", International Journal for numerical methods in fluids, 17,30-321, (1993)

Or if you are working with compressible flows, I'm sure you can find a similar document that is more appropriate.

tushar November 22, 2010 07:05

thanks Mr. dandalf ..

I did compared my simulation results with some standard benchmark problem. but the original problem which i am trying has no experimental results available in liturature. Is there any other check i can do before publication?

dandalf November 22, 2010 07:23

The only other think I can think of is to double check conservation of mass throughout the simulation, if mass is conserved both locally and globaly throughout the simulation, then the flow must at least be physicaly plausable.

sar_mech November 22, 2010 12:19

Hi Dan
 
In the above query u have metioned verify the conservation of mass,does that mean the mass flow rate value @ inlet and outlet boundaries

sar_mech November 22, 2010 12:20

Hi Dan
 
In the above query u have metioned verify the conservation of mass,does that mean the mass flow rate value @ inlet and outlet boundaries

Quote:

Originally Posted by dandalf (Post 284315)
The only other think I can think of is to double check conservation of mass throughout the simulation, if mass is conserved both locally and globaly throughout the simulation, then the flow must at least be physicaly plausable.


dandalf November 22, 2010 12:49

To varify conservation of mass localy
for each cell the net inflow at any time must equal the net change in mass
\rho\left(\frac{\delta u}{ \delta x}+\frac{\delta v}{ \delta y} +\frac{\delta w}{ \delta z}\right)=V\frac{\delta \rho}{\delta t}
where V is the volume of the cell.

To varify global conservation of mass,
The rate of change at any time step of your total mass must equal the diference between your inflow and your outflow.
\frac{\delta \sum \rho V}{\delta t}=A_{in}\rho U_{In} - A_{out}\rho U_{out}

where A_{in} is your inflow area, A_{out} is your outflow area.

if either of these are not satisfied to within some tollerence then your model, is generating or destroying mass either on a local or global scale, which is clearly impossible... thus evidence of an error.

Hope this helps

tushar November 23, 2010 02:38

but in finite volume method we are inherently solving conservation form of equations. This means if mass residue is sufficiently small, will it automatically satisfy both local and global conservation of mass??

whether mass conservation implies to momentum conservation also?

dandalf November 23, 2010 06:05

If you are working with the compressible form of the conservation equatiosons both should already be satisfied.

My point was mearly that if checks reveal that either are not satisified then the result must be incorrect.

you can double check conservation of momentum for each cell buy confirming,

http://www.cfd-online.com/Forums/vbL...ad0727c2-1.gif

for each direction.

Of course if you are using a non cartesian mesh then you will have to adjust the equations.

tushar November 23, 2010 07:35

Thanks to all..

siri November 23, 2010 07:53

tushar,

One general practice to ensure cfd results are meaningful is - monitoring the residual convergence behavior of a physical variable inside the flow domain to one's satisfaction.
However, the choice of the variable and location for its monitoring varies from problem to problem and so it must be made intelligently; otherwise it may not help.

Futher, it is always advisable to put some extra effort and conduct
i) mesh independence study
ii) analyse turbulence models effectiveness
iii) check numerical diffusion
iv) check in results
- numerical bounds of all variables (should be consistent to specified BCs)
- any gradients in flow correlate to local geometry variations or other natural phenomena
v) re-check if results appeal to commonsense

Having done all this, you will be in a position to publish; but more importantly have the courage to defend and receive critical reviews.

Best luck

S


All times are GMT -4. The time now is 04:07.