View Issue Details
| ID | Project | Category | View Status | Date Submitted | Last Update |
|---|---|---|---|---|---|
| 0001073 | OpenFOAM | Bug | public | 2013-11-05 07:32 | 2015-07-29 12:02 |
| Reporter | Assigned To | administrator | |||
| Priority | normal | Severity | trivial | Reproducibility | always |
| Status | closed | Resolution | no change required | ||
| Platform | Unix | OS | Other | OS Version | (please specify) |
| Summary | 0001073: Incorrect injected mass with sprayFoam on 2D axis-symmetric case | ||||
| Description | Hi, I suspect that the calculated mass injected in sprayFoam for 2D axissymetric case is incorrect. The input injected mass is 6.0e-6. Wedge angle 2.86degree one side. So total wedge angle for front and back should be 5.72degree. Calculated injected mass should be 6.0e-6 X 5.72degree/360degree giving somewhere around 9.53e-8. Half of that value is 4.76e-8 assuming that sprayFoam wrongly makes it's calculation based on just one side of the wedge. Log file attached comes close to that value. Please let me know if i'm wrong or had the case setup wrongly. Regards RJ | ||||
| Steps To Reproduce | Just hit ./Allrun. | ||||
| Tags | axisymmetric | ||||
|
2013-11-05 07:35
|
|
|
|
From your log file, I see your OpenFOAM installation is at git commit 596b07255a53. I would suggest you upgraded your installation to e41a7e821f5fabfefb4f9703da8e96cd329f0dae or later, prior to that are just too many (critical) bugs related to the sprayFoam solver. It's likely, you are hitting this bug: http://www.openfoam.org/mantisbt/view.php?id=1036 But probably also one of these ones: http://www.openfoam.org/mantisbt/view_all_set.php?type=1&temporary=n&reporter_id=294&hide_status=90 |
|
|
I'm new to OpenFOAM. It maybe a stupid question to ask, how do you know which commit I'm using? And is it just git pull in terminal will update my OpenFOAM to later commit? Its frustrating to know that the solver is broken after having such a hard time trying to have my simulation validated. Well, it's better late than never. Do you think other version has the same problem? Is there any recommended OpenFOAM version to model diesel spray? |
|
|
In the beginning of your log file it reads: Build : 2.2.x-596b07255a53 As you have already a working OpenFOAM git installation, most likely a 'git pull' and './Allwmake' will do. Detailed instructions on how to install OpenFOAM from git are given here: http://www.openfoam.org/download/git.php For diesel spray simulation, I would recommend you the latest git version of 2.2.x. However, there are still some outstanding bugs (see link above). I'm using the latest git version of 2.2.x plus some fixes to the outstanding bugs (distorted sphere drag model, droplet distortion parameter, Lagrangian sub-cycle). For the time being, you should avoid the KHRT breakup model. The ReitzDiwakar should be fine. Also note that the spray angle thetaInner/thetaOuter in coneInjection and coneNozzleInjection is defined as the half cone angle. |
|
|
I tried reducing parcel per second to a lower value of 6000000 instead of 20000000. It does give injected mass to a closer value of 9.5e+8. But I'm not sure if its the right way of getting the correct mass. But anyway, since the commit I'm using reports wrong injected mass, I guess I will have to try again with the updated version. Noted. I'm aware of inaccurate result from using KH-RT. Liquid penetration constantly registers 0.001m. Looks like the droplets breaks-up way sooner than it should be. Liquid properties like density and specific heat set in sprayProperties that resembles water gives odd result when it's replace with n-heptane liquid properties. Not sure what role does this properties plays. A researcher from CMT was kind enough to share his validated case using OpenFOAM 1.5. The case setup with OpenFOAM is leaner and involves less assumption |
|
|
1. You definitely hit some other bugs as well. By reducing the number of parcels per seconds, you actually weaken the effect of another bug. ;) I know, nasty stuff, but I also had to figure it out the hard way! There were more bugs like that, especially concerning evaporation and thermodynamics (see e.g. bug #938, #939, #945, #950, #960). Anyway, this stuff should be fixed in the latest git version. 2. Concerning the KHRT model: It's not really inaccurate, it's just wrong (see bug #990 and #1014)! This is still broken, even in the latest git version, so just use another BU-model. 3. Concerning the liquid properties, there are some bogus properties listed in the SprayCloudProperties. E.g. Pr and Tbp can be just removed and Tvap is not used in the spray solver, it's a left over and wrong anyways. The Cp and rho values are just dummies and reset during run-time. I know, it's confusing to have them there and fixing it wouldn't be that hard... Thus, if you set T0 correct, your thermodynamics should be fine (of course, assuming you are using the latest git version!). Btw, I provided for most of the outstanding bugs patches, they should be attached in bug reports. Just let me know if you plan to use them, I'm not sure if all of them are still up-to-date. All my simulations are btw for the ECN test case "Spray A": http://www.sandia.gov/ecn/cvdata/targetCondition/sprayA.php |
|
|
I'm doing roughly the same thing. It's just i'm using n-heptane instead of nC12. Running on a 40 specie 62 reaction scheme that includes low temperature combustion. How much is the deviation between your simulation result if compared to sandia? I have got an agreement that missed by a mile if not two. Everything looks wrong to me. Maybe I should give OpenFOAM-1.6-EXT a shot. Perhaps,the solver there aren't as screwed as this. I will keep you posted. By the way, the patch you are talking about; Where and how to use them? Perhaps, we can discuss this via email before moderator ban us for turning this place into our private chatroom. My email is rj_5847@hotmail.com |
|
|
I'm even surprised you didn't get any crash with your spray solver. Prior to fixing the above mentioned bugs, I was running into floating point exceptions all over the place. But even if you were able to run a case without crashes, all results from a sprayFoam solver prior to August 2013 are numerical rubbish! This includes OF versions 2.0.x, 2.1.x and 2.2.1! The latest bugs in the sprayFoam solver were fixed November 5th, 2013, after the 2.2.2 release. Thus you need the latest git version for spray simulation. With the latest 2.2.x git version, I'm able to match the Sandia data for the non-reacting Spray A case (0% O2) accurately. Also for the reacting baseline case (15% O2), the spray results are in good agreement. In an earlier study, I still used 2.0.x with the dieselFoam solver, and also with this setup I got good results, see: LARGE EDDY SIMULATION OF HIGH-VELOCITY FUEL SPRAYS: STUDYING MESH RESOLUTION AND BREAKUP MODEL EFFECTS FOR SPRAY A Armin Wehrfritz, Ville Vuorinen, Ossi Kaario, Martti Larmi DOI: 10.1615/AtomizSpr.2013007342 I have never used the OpenFOAM-1.6-EXT, but as far as I know they are still using the dieselSpray library for sprays (pretty much the same as in 2.0.x). To my experience, the simulation are more stable with the new Lagrangian library in 2.2.x, AFTER the bugs were fixed! Hence my recommendation to use the latest git version of 2.2.x and if you avoid the KHRT model, you should be fine. I probably would even give try without the patches for the outstanding bugs, especially when using the ReitzDiwakar BU-model. Also the sub-cycle feature (bug #953), can be partially circumvented by setting the maximum Lagrangian Courant number. Per default, i.e. if not explicitly specified in the SprayCloudProperties, it's 0.3, if you add right under the 'coupled' switch a option 'maxCo 0.1;' you can adjust the maximum Courant number, which increases the number of Lagrangian sub-cycles for droplets with high velocities. |
|
|
How do you set the injected mass to match your set value. I have update my git version. It still reports half the value it's supposed to be. Tweaking the number of parcel persecond again? Another thing that amuses me. Why is it set to constant volume false? If we are to simulate sandia case, then we have to set it to true? And did you set the dimension to match the sandia chamber volume. As far as I have tested, mesh geometry does influence the predicted pressure. Any comment on this? Btw, how did you do the post-processing? I modified the sprayFoam solver to register value for pressure, max temperature and max CO2 concentration in logSummary. Some how, liquid penetration just refuse to show up. The solver kept insisting that the variable is not declared when its picked directly out of solver itself. |
|
|
Closing - please keep this area for posting bug reports only |
| Date Modified | Username | Field | Change |
|---|---|---|---|
| 2013-11-05 07:32 |
|
New Issue | |
| 2013-11-05 07:35 |
|
File Added: Report.tar.gz | |
| 2013-11-05 13:22 | dkxls | Note Added: 0002608 | |
| 2013-11-05 15:12 |
|
Note Added: 0002609 | |
| 2013-11-05 16:06 | dkxls | Note Added: 0002611 | |
| 2013-11-05 17:24 |
|
Note Added: 0002612 | |
| 2013-11-05 18:29 | dkxls | Note Added: 0002613 | |
| 2013-11-05 18:31 | dkxls | Note Edited: 0002613 | |
| 2013-11-06 00:41 |
|
Note Added: 0002614 | |
| 2013-11-06 12:04 | dkxls | Note Added: 0002615 | |
| 2013-11-06 12:05 | dkxls | Note Edited: 0002615 | |
| 2013-11-06 13:01 |
|
Note Added: 0002616 | |
| 2013-11-06 13:07 |
|
Note Edited: 0002616 | |
| 2013-11-06 13:07 | administrator | Note Added: 0002617 | |
| 2013-11-06 13:07 | administrator | Status | new => closed |
| 2013-11-06 13:07 | administrator | Assigned To | => administrator |
| 2013-11-06 13:07 | administrator | Resolution | open => no change required |
| 2015-07-29 12:02 |
|
Tag Attached: axisymmetric |
