CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

how to justify that my numerical predictions are correct

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   November 22, 2010, 02:55
Default how to justify that my numerical predictions are correct
  #1
New Member
 
tushar
Join Date: Aug 2010
Posts: 9
Rep Power: 7
tushar is on a distinguished road
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..
tushar is offline   Reply With Quote

Old   November 22, 2010, 06:44
Default
  #2
Member
 
Dan
Join Date: Oct 2010
Location: UK
Posts: 41
Rep Power: 6
dandalf is on a distinguished road
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.
dandalf is offline   Reply With Quote

Old   November 22, 2010, 07:05
Default
  #3
New Member
 
tushar
Join Date: Aug 2010
Posts: 9
Rep Power: 7
tushar is on a distinguished road
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?
tushar is offline   Reply With Quote

Old   November 22, 2010, 07:23
Default
  #4
Member
 
Dan
Join Date: Oct 2010
Location: UK
Posts: 41
Rep Power: 6
dandalf is on a distinguished road
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 is offline   Reply With Quote

Old   November 22, 2010, 12:19
Default Hi Dan
  #5
New Member
 
saravanakumar
Join Date: Mar 2009
Location: United Kingdom
Posts: 17
Rep Power: 8
sar_mech is on a distinguished road
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 is offline   Reply With Quote

Old   November 22, 2010, 12:20
Default Hi Dan
  #6
New Member
 
saravanakumar
Join Date: Mar 2009
Location: United Kingdom
Posts: 17
Rep Power: 8
sar_mech is on a distinguished road
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 View Post
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 is offline   Reply With Quote

Old   November 22, 2010, 12:49
Default
  #7
Member
 
Dan
Join Date: Oct 2010
Location: UK
Posts: 41
Rep Power: 6
dandalf is on a distinguished road
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

Last edited by dandalf; November 23, 2010 at 05:44.
dandalf is offline   Reply With Quote

Old   November 23, 2010, 02:38
Default
  #8
New Member
 
tushar
Join Date: Aug 2010
Posts: 9
Rep Power: 7
tushar is on a distinguished road
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?
tushar is offline   Reply With Quote

Old   November 23, 2010, 06:05
Default
  #9
Member
 
Dan
Join Date: Oct 2010
Location: UK
Posts: 41
Rep Power: 6
dandalf is on a distinguished road
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,



for each direction.

Of course if you are using a non cartesian mesh then you will have to adjust the equations.
dandalf is offline   Reply With Quote

Old   November 23, 2010, 07:35
Default
  #10
New Member
 
tushar
Join Date: Aug 2010
Posts: 9
Rep Power: 7
tushar is on a distinguished road
Thanks to all..
tushar is offline   Reply With Quote

Old   November 23, 2010, 07:53
Default
  #11
Member
 
Join Date: Oct 2010
Posts: 44
Rep Power: 6
siri is on a distinguished road
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
siri is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Numerical dissipation/difusion in LES Ray FLUENT 2 June 10, 2002 05:15
numerical scheme ado Main CFD Forum 3 October 12, 2000 08:20
Standard for checking and testing numerical schemes? X. Ye Main CFD Forum 7 August 31, 1999 17:05
New Books and Numerical Software Eleuterio TORO Main CFD Forum 0 December 18, 1998 13:41


All times are GMT -4. The time now is 06:20.