
[Sponsors] 
March 1, 2004, 17:00 
stagged grid solution is high of numer viscosity?

#1 
Guest
Posts: n/a

Do you have similar experience as follows?
For an unsteady 1D tube flow, two runs are made (Re=0, almost imcompressible, central difference, no artificial viscosity): 1) regular uniform mesh 2) stagged grid (u is defined at i, p is defined at i+1/2) It seems that it is hard for 2) to give unstaedy soluiton; its soluiton monotonically tends to a steady state. Whereas, in 1) some oscillations are observed Does this imply stagged grid gives solutions with very high artficial viscosity? Thanks TTT 

March 1, 2004, 22:34 
Re: stagged grid solution is high of numer viscosi

#2 
Guest
Posts: n/a

A lot of information is missing here. And the devil is in the details.
Are you using the same algorithm in each case? Explicit or implicit? If implicit (all spatial derivitives evalutated at time n+1) how are the equations solved? Simultaneously or sequentially? Are linearized equations used? If so, how are they linearized? Is the same solution scheme used for both formulations? Did you use the same mesh spacings to compare the two schemes (or two solutions)? Finally, you imply (but don't actually say) that you're using an artifical viscosity scheme for the staggered arrangement. How much artifical viscosity do you use (relative to the natural viscosity)? How did you decide what the value should be? Is it a constant in space and time or is it kept to the minimum necessary for stability in each equation? In any case, the answer to your question is "not always". 

March 2, 2004, 10:05 
Re: stagged grid solution is high of numer viscosi

#3 
Guest
Posts: n/a

Thank Jim.
The details are simple and straightforward: Predictioncorrection is used to march in time (4th RungaKutta also tried). Schemes (central difference) and grid spacings are same in the two cases. No artificial viscosity term is used. constant time step and grid spacing. How the answer can be then? what's your experience? Thanks HT 

March 2, 2004, 16:09 
Re: stagged grid solution is high of numer viscosi

#4 
Guest
Posts: n/a

Do you expect your exact solution for this case to be unsteady for large time? i.e., not just unsteady while the transient due to the initial conditions dies down. If you expect your exact solution to be unsteady for large time, does the unsteadiness arise from a forcing boundary condition (such as a moving wall, or unsteady wall temperature), or does it arise from confinement/reflection of transient due to the initial conditions. In the former case, you should check the boundary condition numerical treatment, i.e., does the interior scheme on the staggered mesh perceive an appropriate numerical boundary condition that adequately represents the physics of the boundary condition? In the latter case (of the transient), you should be aware that even though you are dealing with the subsonic Euler equations, numerical dissipation of any scheme will usually cause the transient generated by the initial conditions to eventually die out. Of course, in this case, schemes with larger numerical dissipation (either inherent in the scheme, or explicitly added by the user) will damp out the initial transient faster than those with smaller numerical dissipation.
Another possibility to bear in mind is the difference between collocated and staggered mesh discretizations. In case your exact solution happens to be asymptotically (large time) a steady solution, then the following is a possibility. The scheme written on the collocated mesh may be suffering from oddeven decoupling (which can be verified by a von Neumann stability analysis, but this is painful work unless you use a computer algebra program). This oddeven decoupling could be holding back the convergence to steady state. Check to see whether your oscillation is flipping and flopping between two states, which is typical of unsteadiness caused by oddeven decoupling, in my experience. The staggered mesh scheme, on the other hand, probably has no such decoupling, and therefore is able to converge smoothly to the steady state. There is a considerable amount of work reported in the CFD literature of the '70s and '80s (though I lack the time to look up any references for you) that analyzes oddeven decoupling in collocated meshes for incompressible flow, and the need for pressure variable staggering relative to the velocities to remove this oddeven decoupling. Most of this analysis is for steadystate solvers, where the oddeven decoupling shows up as sawtooth or staircase patterns in the solution during any given iteration. Check the spatial distribution of your collocated mesh solution during any time step towards the end of your run. Does it show sawtooth type oscillations? (by sawtooth, i really just mean alternating, like a train of square pulses). 

March 2, 2004, 18:03 
Is the unsteadiness physical?

#5 
Guest
Posts: n/a

Thanks a lot for Ananda's points of insight.
It conjectured that staggered grid gives a solution with too much artificial dissipation. By collocated grids without any artificial dissipaiton, the solution oscillates, locally, at begining, then then turns into oldeven form of oscillations (losing stability). After adding right amount of artificial dissipation, the solution has undulations (locally, at few nodes), which seem not to be oddeven decoupling (pressure at neighboor nodes go up or down together). Although the amptitude is small (0.5%), the undulation is lasting and won't die away. Actually, it is expected that unsteadiness is going to happen. Notice that the boundary condition is pressure is fixed at the both ends (1D). So, the question becomes how to justify that the undulation (with artificial diss added) is physical? Thanks for any of opinons. HT 

March 2, 2004, 18:11 
Viscous equations or Euler equations?

#6 
Guest
Posts: n/a

HT doesn't mention solving Euler equations. He just says he hasn't included any artificial viscosity. The lack of artificial viscosity doesn't lead to Euler equations. However, the neglect of the actual viscous terms (mu*d^2 u / dy^2 for example) changes the character of the solution and results in Euler equations  first derivatives (advective terms, etc) only.
Also, collocation is a mathematical approximation technique. Do a Google search on "collocation approximation" for more detail. Colocation is a mesh/differencing scheme in which the pressure and velocities are all located at cell centers. HT is using colocation. 

March 3, 2004, 01:56 
Re: Viscous equations or Euler equations?

#7 
Guest
Posts: n/a

Thanks Jim, for the correction. Yes, I meant "colocation", not "collocation". I was aware of collocation method being the term for Galerkin schemes where the resultant discretization looks like a pointwise difference approximation. I misremembered the spelling of "colocation", because the basic english meaning of both words is the same.
As to the Euler/NS question, I was merely pointing out that even in the Euler case, which is the most likely to have an exact solution in which the initial unsteadiness bounces around forever, one cannot expect the solution of a numerically stable scheme to do this forever, because of the numerical dissipation. Laminar NavierStokes solutions with steady boundary conditions will eventually dissipate the initial unsteadiness, and reach a steady state. So, with viscous equations, HT should have some feel based on the geometry and Re as to whether the flow could be turbulent or in the transition regime. This would account for physical largetime unsteadiness in a flow with steady bcs. HT, I am unable to judge whether the unsteadiness you see with the colocated scheme with larger numerical dissipation is physical or not. The presence of oddeven decoupling when the numerical dissipation is reduced makes me suspect that the unsteadiness may be numerical rather than physical. One possible test is to refine the mesh for both schemes, but particularly for the staggered mesh scheme. See if the solution of the latter goes unsteady on the finer mesh (where there is less numerical dissipation). I would also reduce the Courant number (not just the time step size), because the unsteadiness may also be caused by underresolution in the time direction. Of course, a negative finding in such a test proves nothing because it may be that the mesh would still not be fine enough. 

March 3, 2004, 02:12 
Re: Viscous equations or Euler equations?

#8 
Guest
Posts: n/a

HT, I forgot to mention that if you refine the staggered mesh sufficiently (to achieve low numerical dissipation) and you see the same sort of unsteadiness that you see in the colocated mesh case, that would be a strong indicator that the unsteadiness is physical rather than a numerical artifact, and would support your hypothesis that the scheme on the coarser staggered mesh has enough numerical dissipation to damp out the physical unsteadiness. If no amount of mesh refinement of the staggered mesh scheme produced this sort of unsteadiness, then that would be a strong indicator that the unsteadiness seen with the colocated scheme is numerical rather than physical.


March 3, 2004, 02:41 
Re: Viscous equations or Euler equations?

#9 
Guest
Posts: n/a

Some further thought reveals that my earlier post about the Euler/NS equations was based on fuzzy thinking, and is incorrect. What I wrote earlier is true for some geometries and steady bcs. However, there are other cases, such as crossflow past a circular cylinder, where the exact Euler solution with slip bcs may be steady, while the low Re NS solution with nonslip bcs may exhibit laminar vortex shedding forming a von Karman vortex street. So I am forced to retract my statement that initial unsteadiness is more likely to persist forever in the Euler case than in the NS case. There are unsteady laminar viscous flows with steady bcs, where the unsteadiness is caused by an instability related to the velocity profile, rather than by a persistence of initial unsteadiness. The Euler solution for the same geometry with the nonslip velocity bcs replaced by slip bcs may be steady. So, if HT is solving the NS equations, the question remains as to whether his physical flow exhibits laminar unsteadiness or turbulent unsteadiness or transitional unsteadiness. Apologies for my somewhat confused earlier post.


March 3, 2004, 10:47 
Re: stagged grid solution is high of numer viscosi

#10 
Guest
Posts: n/a

"Predictioncorrection is used to march in time (4th RungaKutta also tried).
"Schemes (central difference) and grid spacings are same in the two cases. No artificial viscosity term is used. constant time step and grid spacing. "How the answer can be then? what's your experience?" HT, I really haven't used RungKutta time marching in this context, so have no experience. My experience with predictorcorrector schemes is checkered; I've usually found the semiimplicit schemes (explicit estimate with a continuity [pressure] based implicit correction) to be the most reliable. These are generally those originally developed by Harlow et al at Los Alamos in the 50's and 60's. Hardly modern but very useful! Your question really opens a 'can of worms' for this kind of a forum. And Amanda's posts raise the question of how the walls of your tube are modeled. How do you account for the wall drag? Depending on your purpose in doing the calculation, the drag might be ignored or described as (for example) some function of the Reynolds number. If you ignore the wall drag, that would appear to be a 1d Euler equation. Are you interested in the transients or just a steady state? I'm probably safe in sticking with my original conclusion: You really can't generalize that a staggeredmesh scheme is always more dissipative than a colocated scheme. 

March 3, 2004, 11:36 
Compressible NS and ...

#11 
Guest
Posts: n/a

Thanks much for your interests in the problem.
I should have given more details earlier: the equtation is of 1D, compressible, NS (continuity + momentum). The fluid (polymer) is very viscous and the viscous term is about balanced by pressure gradient. Also, the compressibility is small (drho/rho =10^{6}). The system is stiff, with very large coeficients. HT 

March 3, 2004, 17:09 
Re: Compressible NS and ...

#12 
Guest
Posts: n/a

HT, you are welcome to the thoughts I set down earlier. I have not studied anything about the highly viscous slightly compressible 1D flow that you mention. So I am unable to say whether you should expect true unsteadiness or not. Your best bet would seem to be to refine the staggered mesh sufficiently to check whether the same unsteadiness shows up that you see with the colocated mesh. Good luck.


March 3, 2004, 20:23 
Re: Compressible NS and ...

#13 
Guest
Posts: n/a

HT,
Your one dimension would be z, the direction along the axis of your tube? Call the velocity in that direction w. And then t (for time of course) is added. I haven't worked with huge viscosity fluids either. Unless it's very different in character as well as magnitude from 'normal' fluids, it would make its influence known along the boundaries of the tube. Normally the axial (shearing) force would enter in the term d[mu*d(w*r)/dr]/(r*dr), where r is the radial dimension. Since you've excluded variation in r, shouldn't this term be modeled some way? I think the axial viscous term, d[mu*(dw/dz]/dz, is very small relative to the shear term and can be neglected. What am I missing? 

March 4, 2004, 13:26 
Re: Compressible NS and ...

#14 
Guest
Posts: n/a

Thanks to both Jim and Annada.
I think mesh refinement test using staggered grid is a good idea. Experiements suggest unsteadiness may happen. Also, the shear stress term is modeled by an integral in r direction, and the nomral stresses are ignored. I'll post interesting results if they turn out. HS 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
grid dependancy  gueynard a.  Main CFD Forum  19  June 27, 2014 21:22 
convergence problem with high viscosity  Jan  CFX  0  February 29, 2008 05:01 
High turbulent viscosity, problem with BC  Narmin  FLUENT  2  May 8, 2007 03:17 
problem: very high turbulent viscosity ratio  Christine Sindelar  FLUENT  2  November 9, 2005 08:23 
Grid Quality and the Solution  Faraz  Main CFD Forum  4  January 10, 2000 19:18 