View Issue Details
| ID | Project | Category | View Status | Date Submitted | Last Update |
|---|---|---|---|---|---|
| 0000635 | OpenFOAM | Bug | public | 2012-08-27 10:31 | 2012-08-28 17:57 |
| Reporter | hannes | Assigned To | henry | ||
| Priority | high | Severity | major | Reproducibility | always |
| Status | resolved | Resolution | no change required | ||
| Platform | AMD Opteron | OS | CentOS | OS Version | (please specify) |
| Summary | 0000635: LTSInterFoam gives wrong resistance of fully submerged object | ||||
| Description | The LTSInterFoam case runs normal and converges. But the resistance force (X-Force) on the object under consideration is completely wrong (+80%). On the same grid, simpleFoam returns the right result. I have stumbled over this during the simulation of ships with a ducted propeller where the drag of the duct was obviously much too high (more than double of what it should be). The problem occurs when I simulate the duct alone fully submerged with LTSInterFoam (simpleFoam gives better results). Also, Pascal Anschau from SVA Potsdam has reported the same problem some time ago then he simulated a submerged submarine body (with OF1.6). I have adapted his case to OF2.1.x and observed the problem again. I have attached his case, because my geometries are confidential. They can be downloaded here: simpleFoam: http://www.kroegeronline.net/exchange/gen_sub_wo_FreeSurface.tgz LTSInterFoam: http://www.kroegeronline.net/exchange/gen_sub_w_FreeSurface.tgz | ||||
| Steps To Reproduce | *unpack attached cases *run with simpleFoam/LTSInterFoam *simpleFoam case gives Fx=-35N *LTSInterFoam case gives Fx=-63N | ||||
| Tags | No tags attached. | ||||
|
|
Have you tried with interFoam rather than LTSInterFoam? Also is the issue with the pressure distribution or the way in which the force is integrated? How are you evaluating the drag in each case? |
|
|
Personally, I have only used LTSInterFoam. But as I know, Pascal Anschau used interFoam in OF1.6. And the findings were basically the same. The problem is not with the pressure integration. It is rather a different pressure and velocity distribution. I have evaluated the forces using the "forces"-function object. Also integration of the pressure field in paraview gives a consistent result. |
|
|
Last week I pushed a new generalized turbulence framework for the VoF solvers into OpenFOAM-2.1.x which is consistent with the way the models behave for single-phase solvers. Could you test the latest version to see if the problem persists? |
|
|
Okay, I built a fresh clone of commit 0eeb5dd48286 and continued the testcase. The result is different (which is interesting), but still far off (Fx=-58 instead of Fx=-63). |
|
|
OK, that makes sense, I would expect a modest difference. Have you tried running LTSInterFoam without a free-surface, i.e. will the domain with water to make it as similar a possible to the simpleFoam run? |
|
|
Yes, I set up the testcases like this. The whole domain is fully flooded. |
|
|
Are you running laminar or turbulent? If turbulent then as an extra test try running laminar. |
|
|
I have changed the setup of the LTSInterFoam case a bit to make it more similar to the simpleFoam case (pressure given at outlet instead "air" boundary). That removed some artifacts at the upper boundary zMax but did not change the forces. I have updated the case file above. I have also tried running laminar. That reduces the forces sum to Fx=-41. But while the pressure forces in the simpleFoam case are only -7.7N, they have changed from -26N to -34N in the LTSInterFoam case by switching turbulent to laminar. |
|
|
OK, thanks for performing the additional tests, I will investigate further. |
|
|
I am running the simpleFoam case laminar and it has a VERY strongly transient wake rendering the results from simpleFoam meaningless. Does the case converge with kOmegaSST or is the wake also transient? Have you compared simpleFoam results with those from a single-phase transient solver such as pimpleFoam? |
|
|
The simpleFoam case with kOmegaSST converges and I don't remember problems with unsteadiness. The resulting force was -33.7N which is pretty close to the -33.5N from measurements. And no, I didn't try computing unsteady. To my understanding, simulating a turbulent flow time-averaged without reynolds stresses makes the equation system unclosed (probably much too little dissipation) and I would not expect that to give reasonable results. Meanwhile I also tried to solve the flow with an interFoam formulation that uses not the modified pressure p_rgh but the real pressure p. This gives also too high forces (-62N). |
|
|
I also ran the case with pimpleFoam now (maxCo=0.5). The results are pretty much the same as in simpleFoam (Fx=-33.7N). |
|
|
OK, thanks for the additional tests. I improved the outlet BCs and now have a converged simpleFoam solution with kOmegaSST. I will move on to the interFoam tests. |
|
|
I notice that the schemes chosen for the LTSInterFoam run are radically different to those selected for the simpleFoam run; is there any reason for this? Surely it would be more appropriate to chose the same schemes for the same terms. |
|
|
For the LTSInterFoam runs I chose the setup that I normally use for the first step (shall be robust but not most accurate). For the other runs I took over Pascals selection which seems to be more oriented on the tutorials. But he also did interFoam runs with his more accurate setup with the same results in principle. |
|
|
To usefully comprare results from interFoam and simpleFoam I would STRONGLY recommend that the same schemes be use on corresponding terms. I have now setup an interFoam run with compatible schemes and will report the results later today. |
|
|
It appears that the reason for the difference in your results is that the interFoam and simpleFoam cases are setup with different schemes and slightly different BCs. I have run both codes on the case with consistent schemes and BCs and get the following forces: simpleFoam: forces(pressure, viscous)((-5.8721576 370.88298 -0.0072766811) (-26.261384 0.41569413 -0.00035971636)) interFoam (not yet completely converged): forces(pressure, viscous)((-5.89417168805 369.729235118 -0.00430165874276) (-26.4902691499 0.420973088586 0.000348022742271)) |
| Date Modified | Username | Field | Change |
|---|---|---|---|
| 2012-08-27 10:31 | hannes | New Issue | |
| 2012-08-27 10:38 | henry | Note Added: 0001625 | |
| 2012-08-27 10:52 | hannes | Note Added: 0001626 | |
| 2012-08-27 11:11 | henry | Note Added: 0001627 | |
| 2012-08-27 13:11 | hannes | Note Added: 0001628 | |
| 2012-08-27 13:14 | henry | Note Added: 0001629 | |
| 2012-08-27 13:20 | hannes | Note Added: 0001630 | |
| 2012-08-27 13:23 | henry | Note Added: 0001631 | |
| 2012-08-27 14:47 | hannes | Note Added: 0001632 | |
| 2012-08-27 14:52 | henry | Note Added: 0001633 | |
| 2012-08-28 10:53 | henry | Note Added: 0001634 | |
| 2012-08-28 11:46 | hannes | Note Added: 0001635 | |
| 2012-08-28 12:10 | hannes | Note Added: 0001636 | |
| 2012-08-28 13:42 | henry | Note Added: 0001637 | |
| 2012-08-28 14:05 | henry | Note Added: 0001638 | |
| 2012-08-28 14:26 | hannes | Note Added: 0001639 | |
| 2012-08-28 14:32 | henry | Note Added: 0001640 | |
| 2012-08-28 17:57 | henry | Note Added: 0001642 | |
| 2012-08-28 17:57 | henry | Status | new => resolved |
| 2012-08-28 17:57 | henry | Resolution | open => no change required |
| 2012-08-28 17:57 | henry | Assigned To | => henry |
