CFD Online Logo CFD Online URL
Home > Forums > Main CFD Forum

Reduction in Residual Norm vs. Mesh Refinement

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

LinkBack Thread Tools Display Modes
Old   January 26, 2004, 17:47
Default Reduction in Residual Norm vs. Mesh Refinement
CFD Rookie
Posts: n/a
Hello everyone, I kinda in trouble again. Let's say that I have an analysis (BC is fixed). I first start with a coarse mesh and reach a converged solution. By looking at the residual norm, I am not satisfied, the residuals still look too big and it is not reducing any further. So the second step is I refine my mesh, especially at those locations where there are hugh pressure and velocity changes (gradients). Then based on this finer mesh, I re-run the analysis (to save time, I use the final result of the 1st run as my re-starting point). So at the end of the second run, should I DEFINITELY expect the norm residuals to be samller than those in the run #1?

Thanks in advance.
  Reply With Quote

Old   January 26, 2004, 19:16
Default Re: Reduction in Residual Norm vs. Mesh Refinement
Jim Park
Posts: n/a
Probably Yes if:

you have numerical approximations that have error terms that shrink as the mesh shrinks [it's not unknown for an 'obvious' difference operator to have unexpected error growth as the mesh is refined - especially if the coarse mesh is uniform and the refined mesh is stretched], and

the code is well tested, and

if you have smoothly varying meshes, and

if you didn't change from a uniform mesh (I'm thinking structured, orthogonal meshes here) to a non-uniform mesh, and ...

Better way to state your question. My residual norms aren't getting smaller - should I be suspecious?

I think so.
  Reply With Quote

Old   January 27, 2004, 02:41
Default Re: Reduction in Residual Norm vs. Mesh Refinement
Lars Ola Liavåg
Posts: n/a
In my experience, coarse meshes often tend to converge better than dense ones. If you're not happy with the convergence of your coarse mesh therefore, I don't think refining it will solve your problem. Try looking for other reasons. One possible reason for oscillating monitoring values and a halt in the reduction of the residuals (or even oscillating residuals) is that your solution is unsteady by nature in spite of the steady BC's. Vortex shedding behind a cylinder in cross flow is one example of such flows.

This has happened to me many times when using second order differencing along with e.g. the RNG k-e turbulence model. If you desperatly want a steady state solution, going to upwind and a standard k-e model might help you. To really find out what's happening however, you should run a transient simulation with your steady BC's (do a restart) and see if a periodic or chaotic flow field evolves.


Lars Ola
  Reply With Quote

Old   January 27, 2004, 10:08
Default Re: Reduction in Residual Norm vs. Mesh Refinement
Hrvoje Jasak
Posts: n/a
Nope. Consider this:

Take a backward-facing step and give it lots of flow - there will be many flow features, shear layers, recirculations, you name it. Now create a mesh for it with 20 cells. You will get a solution and an error norm and all seems fine.

Then you refine the mesh: better resolution allows you to pick up more features of the flow, you see more hing gradients, you capture the sheer layer better etc etc. What happened to the error norm? - It want UP: there is much more going on in your solution now than before.

So, you can expect a smoothly decreasing error only whn the mesh is fine enough to resolve all the features of the solution. In all other circumstances there are (unresolved) surprises waiting for you and I cannto tell what the error will do.

  Reply With Quote

Old   January 27, 2004, 11:17
Default Re: Reduction in Residual Norm vs. Mesh Refinement
CFD Rookie
Posts: n/a
To Jim,

Thanks for the insight. I should have included more info in the first message. The mesh I have initially is unstructured. After the refinement, the overall mesh structure stays the same, and I didn't find any mesh got stretched because of the refinement. By the way, the code I am running is a FE code. If I can remember my CFD professor correctly, in finite element method, everything else being the same, a mesh refinement can only bring approximated solution closer to "theoretical" solution. But I am not seeing one. (so frustrating!)

To Lars,

Based on your reasoning, I tend to agree with you that "coarse meshes often tend to converge better than dense ones", but I am worried that a converged solution at a coarse mesh might be very far off from the true solution. On the other hand, I am pretty sure the problem I am solving in nature is a true steady state problem.

At the end, indeed maybe my mesh is not even fine enough to resolve all flows features. Thanks for enlightening me Hrvoje.

Thank you all guys. I really have learned alot!
  Reply With Quote

Old   January 28, 2004, 11:45
Default Re: Reduction in Residual Norm vs. Mesh Refinement
Abhijit Tilak
Posts: n/a

I did some work on Adaptive Mesh Refinement using FEM. You did not say what norm you are using L-infinity or L2. A lot depends on that. I used AMR (mine was R-Adaptive), I was using L2 norm to compute residuals. In all problems the L2 norm would decrease only slightly. In my test problems the L2 norm would decrease more in the adapted region and would instead increase in the region the mesh became coarse. So overall error or L2 norm remained more or less the same. I also compared L-inf norm. It decreased considerably in refined region and again remained unchanged or worse ... increased in coarse regions.I could not come up with unified way of calculating residual norms. My advisor was of the opinion that L2 norm isn't always a good idea and it depends on the problem and what you want to happen. It may not always work. By the way.... an intresting observation... in most of my problems the regions of large gradient and large error never coincided with each other. I had analytical solutions in those cases... so i knew. you may need to choose a appropriate criteria for adaptation. Hope this helps

  Reply With Quote


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
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM Running, Solving & CFD 8 March 28, 2016 11:08
icoLagrangianFoam OF1.6 myNewParticleSolver heavy_user OpenFOAM 16 February 11, 2012 06:15
Full pipe 3D using icoFoam cyberbrain OpenFOAM 4 March 16, 2011 10:20
Error log OpenFOAM 6 August 7, 2009 05:44
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09

All times are GMT -4. The time now is 07:28.