CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Verification & Validation (http://www.cfd-online.com/Forums/openfoam-verification-validation/)
-   -   OpenFOAM V&V (http://www.cfd-online.com/Forums/openfoam-verification-validation/89580-openfoam-v-v.html)

Martin Hegedus June 16, 2011 18:14

OpenFOAM V&V
 
I'm interested in finding Verification and Validation data on OpenFOAM for incompressible and compressible external aerodynamics for basic test cases.

The root of this question is a posting I made at Symscape, http://www.symscape.com/blog/new-str...fd-wind-tunnel

I realize that OpenFOAM is used by industry, academia, and hobbyists. There is even a workshop for it.

However, I am having difficulty finding systematic quantitative (i.e. not qualitative pretty colored pictures or top level slides) V&V information for OpenFOAM for simple geometries, i.e., flat plate, bump, forward/backward steps, lidded cavities, airfoils, wings, etc. This includes grid convergence studies.

Examples of what I am referring to, in regards to a NASA code CFL3D, are, http://cfl3d.larc.nasa.gov/Cfl3dv6/c...testcases.html or http://turbmodels.larc.nasa.gov/, or even http://aaac.larc.nasa.gov/tsab/cfdlarc/aiaa-dpw/

Does such information, to the extent one can reproduce the results, exist for OpenFOAM? Or is it up to each individual/group to work through V&V cases from scratch on their own?

wyldckat June 19, 2011 16:24

Greetings Martin,

I just saw this blog post and remembered about your thread: http://cfdtoy.blogspot.com/2011/05/m...ification.html

Best regards,
Bruno

santiagomarquezd June 21, 2011 16:53

Quote:

Originally Posted by Martin Hegedus (Post 312344)
I'm interested in finding Verification and Validation data on OpenFOAM for incompressible and compressible external aerodynamics for basic test cases.

However, I am having difficulty finding systematic quantitative (i.e. not qualitative pretty colored pictures or top level slides) V&V information for OpenFOAM for simple geometries, i.e., flat plate, bump, forward/backward steps, lidded cavities, airfoils, wings, etc. This includes grid convergence studies.

Does such information, to the extent one can reproduce the results, exist for OpenFOAM? Or is it up to each individual/group to work through V&V cases from scratch on their own?

We did some of this work (and we continue to do it, but the extra part isn't not published yet) and is published here:

COMPARISON OF SINGLE PHASE LAMINAR AND LARGE EDDY SIMULATION (LES) SOLVERS USING THE OPENFOAM(R) SUITE

VOLUME OF FLUID SIMULATION OF BORDA MOUTHPIECES

Results are checked against experiments and Fluent.

Hope this help

Martin Hegedus June 21, 2011 17:33

Thanks, it's a start.

In general, I've seen others raise the issue about grid convergence. (Lid-Driven Cavity from first paper).

Did you figure out why the lid driven cavity did not converge?

The fact that the residuals do not converge to machine zero is a little scary.

santiagomarquezd June 21, 2011 17:42

Hi, Do you refer to the problem of p residuals?

Regards.

Martin Hegedus June 21, 2011 17:49

Yes, that is correct.

santiagomarquezd June 21, 2011 18:00

Martin, this problem was reported several times, but I couldn't find a cure at that time. This is related to PISO loop and tolerances and type in p solver (I never played enough time with GAMG solver for example), I'm working in that now. If you could find a set of parameters that perform better It would be nice to share it with the community, particularly avoiding the plateau at ~1E-6.

Regards.

Martin Hegedus June 21, 2011 19:49

I don't use OpenFOAM that much. I get very frustrated with it. The vast majority of my cases are steady state external aero, both compressible and incompressible. In general I haven't had much luck with OpenFOAM. I figure it is my own personal issue since so many others use the code. So, instead, I wrote my own solver from scratch (compressible with equations coupled). That's been a lot of work. Especially the V&V stuff. However, at some point it would be nice to have more confidence in OpenFOAM and use it more.

If I come up with something that works for the lidded cavity, I'll share it here on this forum. BTW, is there a better place to share cases and solutions for OpenFOAM? http://www.cfd-online.com/Wiki/Valid...and_test_cases seems sparse and www.openfoam.com doesn't seem to be very, well, open in the sense of supplying a place for the OpenFOAM community to go to.

santiagomarquezd June 21, 2011 22:44

Quote:

Originally Posted by Martin Hegedus (Post 312986)
So, instead, I wrote my own solver from scratch (compressible with equations coupled). That's been a lot of work. Especially the V&V stuff. However, at some point it would be nice to have more confidence in OpenFOAM and use it more.

Well you're the kind of person which is essential as a user/developer in OpenFOAM, you have a lot of experience and a very critical vision of a code. I'm working with FOAM to write customized solvers and re-implementing some of them in Matlab (my advisor is working on that since he works with it the most), this task is very instructive but a bit slow.

Quote:

If I come up with something that works for the lidded cavity, I'll share it here on this forum. BTW, is there a better place to share cases and solutions for OpenFOAM? http://www.cfd-online.com/Wiki/Valid...and_test_cases seems sparse and www.openfoam.com doesn't seem to be very, well, open in the sense of supplying a place for the OpenFOAM community to go to.
Well, some vendors as ANSYS, etc. show a lot of benchmarks in their slide-shows, etc. but the real validation is ever spread in a lot of papers, since the validations are usually connected to a specific application.

Regards.

Martin Hegedus June 22, 2011 00:21

Quote:

Originally Posted by santiagomarquezd (Post 313003)
Well, some vendors as ANSYS, etc. show a lot of benchmarks in their slide-shows, etc. but the real validation is ever spread in a lot of papers, since the validations are usually connected to a specific application.

Regards.

Papers are an important part of the process, but I'm also hoping there is a web resource where one can place grids, input decks, and results and "blog" (i.e. informally write) about the results. Another nice feature would be if others could comment on the results and contribute their own results. Something similar to these forum threads, but more focused on results than questions.

I haven't found one yet. A wiki (such as the V&V here at CFD Online), in my opinion, may not be appropriate. Wiki's are very formal and polished.

pbohorquez June 22, 2011 08:45

At low Reynolds numbers (i.e. incompressible and laminar flow) we have reported successful comparison between OpenFOAM and wind tunnel experiments for external flows both for steady and unsteady regime. You could find more information in the following paper:

Bohorquez, P., Sanmiguel-Rojas, E., Sevilla, A., Jiménez-González, J., Martínez-Bazán, C. Stability and dynamics of the laminar wake past a slender blunt-based axisymmetric body. Journal of Fluid Mechanics, 676: 110-144 (2011) http://dx.doi.org/10.1017/s0022112011000358

Quote:

Originally Posted by Martin Hegedus (Post 312986)
I don't use OpenFOAM that much. I get very frustrated with it. The vast majority of my cases are steady state external aero, both compressible and incompressible. In general I haven't had much luck with OpenFOAM. I figure it is my own personal issue since so many others use the code. So, instead, I wrote my own solver from scratch (compressible with equations coupled). That's been a lot of work. Especially the V&V stuff. However, at some point it would be nice to have more confidence in OpenFOAM and use it more.

If I come up with something that works for the lidded cavity, I'll share it here on this forum. BTW, is there a better place to share cases and solutions for OpenFOAM? http://www.cfd-online.com/Wiki/Valid...and_test_cases seems sparse and www.openfoam.com doesn't seem to be very, well, open in the sense of supplying a place for the OpenFOAM community to go to.


santiagomarquezd June 22, 2011 09:52

Another ref. for my thesis!! Thanks for it and the downloading link.

Regards.

Martin Hegedus June 22, 2011 12:55

Quote:

Originally Posted by pbohorquez (Post 313071)
At low Reynolds numbers (i.e. incompressible and laminar flow) we have reported successful comparison between OpenFOAM and wind tunnel experiments for external flows both for steady and unsteady regime. You could find more information in the following paper:

Bohorquez, P., Sanmiguel-Rojas, E., Sevilla, A., Jiménez-González, J., Martínez-Bazán, C. Stability and dynamics of the laminar wake past a slender blunt-based axisymmetric body. Journal of Fluid Mechanics, 676: 110-144 (2011) http://dx.doi.org/10.1017/s0022112011000358

Clearly a lot of work went into the paper and I found the results and topic interesting. I found the shift from steady axisymmetric, to steady non-axisymmetric, to unsteady cool. And I believe in the real world this transition exists. However, something usually sets off the transition, i.e. transitioning from steady axisymmetric to steady non-axisymmetric. In the case of the wind tunnel results I assume it is the sting which comes out the side of the model, i.e. the plane of symmetry for the non-axisymmetric, but symmetric, result is aligned with the side sting. But what transitions it for the axisymmetric CFD geometry? I assume it is the non-axisymmetric grid that was used. But was it? Where the results converged all the way? How was convergence measured? Depending on the solution algorithm and the case, I expect the results sometimes to converge non-axisymmetricly on a non-axisymmetric grid, at least until the residual has died down a lot. And the process is very non linear. The solution sits for a while and then moves rapidly to a new location, i.e. the axis. The flow is on the verge of being unstable, so all the perturbations (solution, grid, numerics, etc.) must be removed to the extent possible to get a true answer. Otherwise things get masked, i.e. the effects of the wind tunnel and sting. Or, bugs in the code.

Martin Hegedus June 22, 2011 13:16

Quote:

Originally Posted by Martin Hegedus (Post 313135)
The solution sits for a while and then moves rapidly to a new location, i.e. the axis.

Let me rephrase, The solution state sits for a while and then moves rapidly to a new state location, i.e. axisymmetric.

pbohorquez June 22, 2011 14:25

Yes, you are right. On the numerical side there are lots of parameters that affect the solution of any problem because they introduce errors: the topology of the mesh, cell elements, the implementation (segregated/coupled), the order of consistency, etc. And they affect the results because the mesh is always coarser than we want in the absence of exceptional numerical facilities.

But this happens with any numerical solver, not just with OpenFOAM. There are suitable problems that can be solved if you know how to drive the tool, otherwise the numericist wont succeed. Numerical algorithms are designed for specific purpose and, consequently, they continue growing. OpenFOAM implements a classical FVM formulations, it is not the Panacea.

Martin Hegedus June 22, 2011 14:57

Quote:

Originally Posted by pbohorquez (Post 313144)
But this happens with any numerical solver, not just with OpenFOAM. There are suitable problems that can be solved if you know how to drive the tool, otherwise the numericist wont succeed. Numerical algorithms are designed for specific purpose and, consequently, they continue growing. OpenFOAM implements a classical FVM formulations, it is not the Panacea.

Very true, and I definitely agree with "know how to drive the tool, otherwise the numericist wont succeed" That's the frustrating part. I'm not confident that I know how to drive OpenFOAM. Therefore, my personal chance of numerical success with the code is low. And sometimes I feel like I'm driving blind. Even with my experience writing and driving various research codes.

A question then. Were you able to converge the residuals for your steady results to machine zero, or at least to the point where you were very confident the residuals were heading there? I assume you did, but I'm looking for data points not based on my assumptions.

pbohorquez June 22, 2011 15:27

In the case described in the paper, if the boundary condition of the body is set to slip, then the pressure and velocity residual drop to zero. When using 'no slip' the pressure residual may reach an asymptotic value (usually between 10^{-6} and 10^{-4}). However, I cannot ensure that it is due to the boundary condition. Why can you use a different interpolation and discretization scheme for each differential operator in each equation? Is there an optimal choice to guarantee the "well balanced" property and drop the residuals to machine accuracy?

Anyway, we are very happy with OpenFOAM results for incompressible flows. They converge as the mesh is refined and it is able to reproduce many non-linear transitions for a wide range of physical problems, even in the presence of the pressure plateau.

Martin Hegedus June 22, 2011 16:11

Quote:

Originally Posted by pbohorquez (Post 313154)
In the case described in the paper, if the boundary condition of the body is set to slip, then the pressure and velocity residual drop to zero. When using 'no slip' the pressure residual may reach an asymptotic value (usually between 10^{-6} and 10^{-4}). However, I cannot ensure that it is due to the boundary condition. Why can you use a different interpolation and discretization scheme for each differential operator in each equation? Is there an optimal choice to guarantee the "well balanced" property and drop the residuals to machine accuracy?

Interesting. You mention boundary condition, or could it be the shear stress in the cell? For example the ratio of shear stress vs. delta pressure. You mentioned a range of asymptotic values. Is this a function of Reynolds number? An increase in the viscosity has the effect of dropping the Reynolds number. So, as the Reynolds number drops, does OpenFOAM have a harder time to converge? (sorry, asking the question doesn't mean I know the remedy. I don't.)

One of the reasons this is interesting is that eddy viscosity in the RANS equation basically lowers the local Reynolds number, i.e. viscosity goes up. Thus there is somewhat of a connection between the flows I usually deal with, and your low Reynolds number shapes.

This seems to match with santiagomarquezd.

Has anyone done a flat plate analysis with OpenFOAM and converged it to machine zero? (Edit: Oh, at low to high reynolds numbers)

pbohorquez June 22, 2011 17:03

Nice thoughts. The flat plane analysis is a good suggestion. If someone knows the answer please share it.

With respect to the shear stress in the cell, figure 16 in Alves, Oliveira & Pinho (2003), www.fe.up.pt/~fpinho/pdfs/ijnmf1.pdf, came to my mind. I don't know if it is a crazy idea but iterations in SIMPLE are analogous to "pseudo-time", so maybe there is some analogy between the asymptotic values for the pressure and for \tau_{xx}.

Martin Hegedus June 22, 2011 17:24

I did I quick internet search and found OpenFOAM results for flat plates, both laminar and turbulent. I have not seen any residual plots and the results I saw are for x stations that have much higher Rex than the reynolds number of interest here. So nothing conclusive.


All times are GMT -4. The time now is 11:20.