
[Sponsors] 
August 22, 2010, 07:47 
Artificial dissipation for NS equations, flow in a pipe

#1 
Member

Hi all,
I am trying to simulate compressible flow through a pipe. I am using FVM with Grid in Cylindrical coordinate system. I am adding artificial dissipation which is of the order of 1e6, for a certain number of control volumes. Code is working fine and I see convergence. But If I change the number of control volumes then the code diverges. I am trying to solve full unsteady compressible NS equations. My question is 1) do we need to add artificial dissipation for NS equations similar to that of Euler equations? 2)how do we determine what amount of dissipation to be added even in Euler equations. 3) upwind schemes has inherent dissipation is this correct or wrong? 

August 25, 2010, 23:02 

#2 
New Member
Join Date: Jun 2010
Posts: 16
Rep Power: 7 
Hi Ramesh,
1) Yes for unstructured grids, but maybe unnecessary for nonskewed structured grids with the centraldifference scheme. For viscous discretizations, a recent paper by Nisikawa (AIAA 20105093) can be useful. He calls it a damping (rather than dissipation) term that is required for robust viscous schemes. Beyond Interface Gradient: A General Principle for Constructing Diffusion Schemes http://www.hiroakinishikawa.com/My_p...20105093.pdf Presentation slides http://www.hiroakinishikawa.com/My_p...093_slides.pdf 2) It can be very difficult. For the Euler, the amount of dissipation depends on the local flow. 3) Correct. Upwind methods are very useful in that you don't need to tune the amount of dissipation by yourself as in 2). Use the Roe solver, fluxvector splitting method like VanLeer or AUSM. These upwind fluxes provide dissipation. Good luck. Bjohn 

August 30, 2010, 07:18 
Thanks

#3 
Member

Hi
Thank you, for u prompt reply. I understood, the concept and am going through the paper. But for the problem I am trying to work on, I have a pipe with the grid in cylindrical system meaning that I have concentric circles and radial lines and am stacking it, I see that my grid at the axis has triangular prisms and as I go away from the axis I get quads in 3d hexahedras, only one or two layers of the grid are skewed. I see that my code diverges if I don't add artificial dissipation. I am solving full compressible NS equations, the solution evolves and suddenly diverges I am not understanding why and what is making it to diverge, I fixed the cfl to 0.1 and my typical time step is of the order of 1e7. the viscosity calculated with sutherlands law is of the order of 1.86e5. How do I know that I need artificial viscosity for this problem, those cells at the axis do they really trouble the code. I am using FVM to solve this problem. 

August 30, 2010, 15:26 

#4 
New Member
Join Date: Jun 2010
Posts: 16
Rep Power: 7 
What is you FVM?
1. Cellcentered or nodecentered? 2. What Euler flux are you using? (Roe, Van Leer, Jameson?) 3. What is your viscous discretization? (centraldifference?) 4. Is the timestepping explicit or implicit? The more details you provide, the more response may be expected. 

August 31, 2010, 05:14 

#5  
Member

Quote:
Q= [rho,rho*v1,rho*v2,rho*v3,rho*Et] with Et total energy 2. Flux is evaluated by taking average of Q on the face to be average of Q of neighbouring cells corresponding to the face. 3. Viscous discretization is also done in the similar manner, first find the gradients at cell centre and then get the average gradients on the face. 4. I am using Explicit scheme and time step is found by specifying CFL=0.1 and use RangeKutta 4th order method for time integration. The discretization I use is central difference as i use the summation of the fluxes on each face for a given cell. The observation made by me in the results obtained. Till 6600 time steps the v3 component of velocity gradually increases and I can see pressure wave travelling till some distance but then suddenly the pressure in the some cells increase and causing the code to diverge. 

August 31, 2010, 05:44 

#6 
New Member
Join Date: Jun 2010
Posts: 16
Rep Power: 7 
>2. Flux is evaluated by taking average of Q on the face to be average of Q of >neighbouring cells corresponding to the face.
Inviscid flux needs dissipation. Use upwind flux: Roe flux, Van Leer FVS, AUSM, etc. >3. Viscous discretization is also done in the similar manner, first find the gradients >at cell centre and then get the average gradients on the face. This scheme can also be a cause of instability. The above mentioned Nishikawa's paper shows that the averagegradient scheme needs a damping term. See his paper which has a cellcentered viscous discretization scheme with a damping term. Good luck. bjohn 

August 31, 2010, 09:24 

#7 
Member

[QUOTE=bjohn;273448]>2. Flux is evaluated by taking average of Q on the face to be average of Q of >neighbouring cells corresponding to the face.
Inviscid flux needs dissipation. Use upwind flux: Roe flux, Van Leer FVS, AUSM, etc. >3. Viscous discretization is also done in the similar manner, first find the gradients >at cell centre and then get the average gradients on the face. This scheme can also be a cause of instability. The above mentioned Nishikawa's paper shows that the averagegradient scheme needs a damping term. See his paper which has a cellcentered viscous discretization scheme with a damping term. But Upwind flux is first order and it has inherent dissipation in it. How ever I am solving NS equations which has natural viscosity, why is the need to add more dissipation to the scheme. I am looking at higher order schemes for solving a DNS problem. so using upwinding will reduce my order. Can u suggest any thing on this 

August 31, 2010, 11:17 

#8 
New Member
Join Date: Jun 2010
Posts: 16
Rep Power: 7 
I'm not familier with DNS.
You should look for papers to see how other people do. Upwind flux does not determine the accuracy. It is actually used in highorder methods. It is the left and right states (and quadrature) that determines the accuracy. See for example, http://chimeracfd.com/programming/gryphon/muscl.html I write upwind fluxes, not upwind schemes, to make this point. 

November 13, 2011, 11:29 

#9 
New Member
budakjam
Join Date: Nov 2011
Posts: 2
Rep Power: 0 
did someone know, how should i close the artificial viscosity where im developing an ausm scheme.Which scheme should i replace if i close the artificial viscosity..


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
High speed compressible flow through pipe  Munni  Main CFD Forum  6  December 7, 2015 12:33 
Reverse Flow at Rotating Pipe Outlet  vismech  STARCCM+  1  August 11, 2009 10:38 
Domain for Pipe Flow  Swarup  FLUENT  0  September 28, 2005 23:25 
stepped pipe flow  Tom Cloutier  Main CFD Forum  0  April 20, 2003 13:19 
Pipe flow  John Grimm  Main CFD Forum  8  March 11, 2002 13:15 