|
[Sponsors] |
simple open channel flow, the inlet and outlet are periodic |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 3, 2013, 06:09 |
|
#21 |
Member
phil
Join Date: Oct 2013
Posts: 36
Rep Power: 13 |
Hey,
I've got nearly the same case as u do. My case is a periodic cooling pipe. At the moment i am setting up my BC but i have quiet a lot problem especially when it comes to mapping the outlet values to the inlet. For me it is very difficult to setup the BC and the offset of the mappedPatch BC because my patches are not parallel to the coordinate patches. Perhaps you can have a look at my thread and help me. Best Regards, Phil |
|
December 4, 2013, 17:05 |
|
#22 |
New Member
Vimaldoss Jesudhas
Join Date: Aug 2013
Posts: 15
Rep Power: 13 |
Hi Bruno,
thanks for the reply, I tried what is mentioned in the directory, but was not able to get it work. Should I run the commands mentioned in the web page in the OpenFOAM/user/run directory or some other location, kindly let me know. Thanks, Vimal |
|
December 28, 2013, 15:28 |
|
#23 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Hi Vimal,
OK, a very quick way to build swak4Foam is like this: Code:
mkdir -p $FOAM_RUN cd $FOAM_RUN cd .. wget https://github.com/wyldckat/swak4foam/archive/OF22X.zip unzip OF22X.zip cd swak4foam-OF22X ./Allwmake > make.log 2>&1 #run the last line once again: ./Allwmake > make.log 2>&1 Best regards, Bruno
__________________
|
|
January 9, 2014, 11:37 |
|
#24 |
Member
phil
Join Date: Oct 2013
Posts: 36
Rep Power: 13 |
Hey Sniper and wydlckat,
I had a look at your hints about Snipers case. My case is nearly the same as the one frome him. The only difference is, my patches are not parallel to the coordinate axes/planes. Right at the moment i am facing a lot of problems with setting up my case with cyclic as well as mapped boundary conditions. Especially with setting the offsets for the cyclic/mapped planes in a case where the planes are not exactly conformal. As i explained in my thread already i want to compare OpenFoam with a Fluent case. The Fluent case has a periodic inlet with steady state pressure based simple solver. - Can you look at my case and give ma a hint why my cyclic BC's dont work. - Can you tell me where i can edit the pressure gradient or the mass flux for the inflow because out of the fluent case i get that it is pressure based. - Is my geometry working at all or do i have to edit it with i dont know commands like topoSet etc. Greetings Phil |
|
January 18, 2014, 14:20 |
|
#25 | ||
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Greetings gelbebanane,
Quote:
I was going to suggest that you had a look into the tutorial "incompressible/pisoFoam/les/pitzDailyMapped" and to suggest using the "mapped" boundary condition, taking into account that the offset is the vector between the centroids of each patch... but since the cell count is not identical, things get a bit complicated. Quote:
I've taken a look into the list of posts you've made lately and I got lost. I have no idea to which thread you're referring to. The inlet and outlet patches do not have the exact same area, which are part of the problem. I suggest that you take a slightly different approach:
Bruno
__________________
|
|||
January 20, 2014, 06:32 |
|
#26 |
Member
phil
Join Date: Oct 2013
Posts: 36
Rep Power: 13 |
Hey,
thanks for your suggestions. Unfortunately i saw too late that you will answer my question at your github so i had no more time to update my post above. From your other link that you have attached i couldn't get any information because there it is just an blockMesh created mesh. 1. I made a point transformation in Salome and translated my inlet to my outlet and exported this as my new .stl file. 2. Generated the mesh but without any improvements. 3. Dont know what you meant here, so i came to the point that i started already wrong at 1. What i also tried is to rotate my geometry by an angle so that the inlet and outlet patches are parallel to the blockMesh patches. but it still gives me a different number of cells back. I think the main problem is the snappy process and my sharp edges. (snappy run without snap and layer add, just castellatedmesh feature) edge.jpeg Isn't it possible to use different cell numbers as well as the mapped condition? I can also use the mentioned rotated mesh for my case, i just have to edit my velocity vector. I have also tried, using the main edges of my geometry for my blockMesh mesh but the mesh quality after snappy didn't improve and it also didn't snap anymore. I also tried cyclic and cyclicAMI. cyclic does not work because of different cell numbers and cyclicAMI gives me an error back when i try to change my patches with "createPatch" command. Code:
>createPatch -overwrite .... Build : 2.2.x-ae7a43cbbfe3 Exec : createPatch -overwrite Date : Jan 13 2014 Time : 10:46:56 Host : PID : 28596 Case : nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Reading createPatchDict Adding new patch inlet as patch 4 from { type cyclicAMI; neighbourPatch outlet; } Adding new patch outlet as patch 5 from { type cyclicAMI; neighbourPatch inlet; } Moving faces from patch eingang to patch 4 Moving faces from patch ausgang to patch 5 Doing topology modification to order faces. AMI: Creating addressing and weights between 142345 source faces and 142177 target faces --> FOAM Warning : From function AMIInterpolation<SourcePatch, TargetPatch>::checkPatches(const SourcePatch&, const TargetPatch&) in file lnInclude/AMIInterpolation.C at line 109 Source and target patch bounding boxes are not similar source box span : (0.000115329 0.0987398 0.152781) target box span : (8.22414e-05 0.0987483 0.152795) source box : (0.00671131 1.90699e-06 -0.00673927) (0.00682664 0.0987417 0.146042) target box : (0.0301843 1.448e-06 0.0167262) (0.0302665 0.0987498 0.169521) inflated target box : (0.0210879 -0.0090949 0.00762988) (0.0393629 0.107846 0.178617) --> FOAM FATAL ERROR: Unable to find initial target face From function void Foam::AMIInterpolation<SourcePatch, TargetPatch>::calcAddressing(const SourcePatch&, const TargetPatch&, label, label) in file lnInclude/AMIInterpolation.C at line 712. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 at cyclicAMIPolyPatch.C:0 #3 Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::update(Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&) in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/lib/libmeshTools.so" #4 Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::AMIInterpolation(Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::autoPtr<Foam::searchableSurface> const&, Foam::faceAreaIntersect::triangulationMode const&, bool) in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/lib/libmeshTools.so" #5 Foam::cyclicAMIPolyPatch::resetAMI() const in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/lib/libmeshTools.so" #6 Foam::polyBoundaryMesh::movePoints(Foam::Field<Foam::Vector<double> > const&) in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #7 Foam::polyMesh::movePoints(Foam::Field<Foam::Vector<double> > const&) in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #8 in "/sw/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/bin/createPatch" #9 __libc_start_main in "/lib64/libc.so.6" #10 at /usr/src/packages/BUILD/glibc-2.11.2/csu/../sysdeps/x86_64/elf/start.S:116 Abgebrochen Looking forward for any further suggestions Greetings Phil |
|
January 26, 2014, 16:26 |
|
#27 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Hi Phil,
Mmm... OK, I've got two suggestions:
Bruno
__________________
|
|
January 28, 2014, 09:53 |
|
#28 |
Member
phil
Join Date: Oct 2013
Posts: 36
Rep Power: 13 |
Hey there,
i've managed to get my case running with "cyclicAMI". Now my case is running with a modified simplefoam/cyclic solver from here. The problem is now that i dont get the expected values like in Fluent. My pressure gradient is not the same and i dont know if i specified my mass flow rate with "Ubar" correctly. My inlet velocity is (12 0 0) m/s and my mass flow rate 0.07865 kg/s. All other initial values are specified under 0/include/initialConditions. I've uploaded my case with the appropriate BC. You have to use the solver that is also attached in this thread. Just "make" the solver, i have already changed all neccessary files. ribbed.zip simpleFoamCyclic.zip Regards, Phil |
|
February 2, 2014, 11:26 |
|
#29 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Greetings Phil,
I'm getting this error message: Code:
Unknown patchField type knutRoughWallFunction for patch type wall In addition, the solver gives a warning about these two: Code:
inlet { type cyclicAMI; value 101325; } outlet { type cyclicAMI; value 101309; } Code:
inlet { type cyclicAMI; value uniform 101325; } outlet { type cyclicAMI; value uniform 101309; } Code:
inlet { type cyclicAMI; value uniform 0; } outlet { type cyclicAMI; value uniform -16; } Beyond this, the relaxation factors seem very relaxed. Are you certain that the solution converged? Best regards, Bruno
__________________
|
|
February 2, 2014, 18:19 |
|
#30 |
Member
phil
Join Date: Oct 2013
Posts: 36
Rep Power: 13 |
Ok,
i have changed my case. Actually it was called nutkRoughWallFunction not knutRoughWallFunction. i have also changed my pressure to what you said. But for my outlet pressure im not sure. First of all my boundaries. My mass flux is 0.07865 kg/s, density=1.1697 kg/m^3, pressure gradient -485.4435 pascal/m, dynamic viscosity 1.85964e-05 kg/m s. My inlet flow is U=(12 0 0). So i calculated my boundaries based on these values: Code:
nu=1,85964e-05 / 1,1697 = 1,58984e-05 the distance from inlet to outlet in x direction is 0.023483. Code:
outlet pressure= -485,4435 * 0,023483 / 1,1697 = -13, 7785 Did i use the wrong length for the gradient? Do i have to use the distance vector that is perpendicular to the inlet/outlet patches or is the distance vector in flow direction ok? So the last value was "Ubar" to calculate. I used the continuum equation for this. But here i have the same problem as mentioned above. Is the mass flux perpendicular to the inlet and outlet patch or is it in flow direction? i made up 2 calculation, 1 with mass flux orthogonal and 1 with mass flux in flow direction. So i got this Ubar values: Code:
Ubar= massflux / (densitiy *patch area) I hope you understand halfway what i want so say you with my calculations and problems. For now i made 4 cases. Each a variation of Ubar direction and pressure gradient on/off. Here is a picture with what i mean about perpendicular and in flow direction (view is on top of my geometry to the ground, bird perspective, dont know the english word for this). flowdir.jpg And here is a case with pressure gradient on and mass flux in flow direction. The problem for now is that my flow does not look not even close like the one in Fluent. rippencase_salome.zip Last edited by gelbebanane; February 4, 2014 at 04:38. Reason: case+rest+explanation |
|
February 16, 2014, 12:25 |
|
#31 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Greetings Phil,
I finally managed to give a proper look into this. Here's what I've found:
Bruno
__________________
|
|
December 28, 2023, 03:12 |
Pressure gradient
|
#32 |
New Member
SOURAV GANGULI
Join Date: Dec 2018
Posts: 11
Rep Power: 7 |
In case of fvOption, we impose momentum source term but can, though there is flow but we cannot observe any pressure gradient along the channel length. Can anyone please tell me how to obtain actual pressure in case of fvoptions
Regards, Sourav |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Open Channel Flow | ElanMorin | FLUENT | 4 | February 25, 2015 17:26 |
Net mass flow inlet vs outlet | Nigui28 | FLUENT | 1 | August 12, 2011 11:09 |
Outlet condition for open channel flow? | gareth__it_power | OpenFOAM Running, Solving & CFD | 1 | July 17, 2011 04:44 |
pressure outlet (open channel flow) | Willem Brantegem | FLUENT | 2 | April 4, 2007 03:40 |
pressure outlet (open channel flow) | Willem Brantegem | Main CFD Forum | 0 | April 3, 2007 10:39 |