|
[Sponsors] |
November 23, 2010, 08:28 |
cylindricalInletVelocity OpenFOAM
|
#1 |
Member
Alex
Join Date: Apr 2010
Posts: 48
Rep Power: 16 |
Hi,
Is there a paper/document which explains the meaning of the cylindricalInletVelocity Boundary Condition for OpenFOAM? I need to set up an inlet velocity in a tube with the following features: 133 m/s axial velocity, 0 m/s radial, 77 m/s tangential (clockwise). I tried to use the following BC available but there are some lines I don't get, like: axis (0 0 1) , centre (0 0 0). Can someone help me? The BC is the following: type cylindricalInletVelocity; axialVelocity 133; tangentialVelocity 77; centre (0 0 0); //by default (0 0 0) axis (0 0 1); rpm 0; radialVelocity 0; value uniform (0 77 133); |
|
March 2, 2011, 20:23 |
|
#2 |
Member
N. A.
Join Date: May 2010
Posts: 64
Rep Power: 16 |
Hey Alessio,
Were you able to get the information about axis and center? I dont know if the axis is in cartesion cordinate system or cylindrical. Thanks, Nir |
|
March 3, 2011, 01:55 |
|
#3 |
Member
Alan Russell
Join Date: Aug 2009
Location: Boise, Idaho USA
Posts: 61
Rep Power: 17 |
Alessio,
The best way to understand OF is to look at the source code. For your BC, look in src/finiteVolume/fields/fvPatchFields/derived/cylindricalInletVelocity. Looking through the .C and .H files usually tells you a lot. I think the Center (0 0 0) is the center of your cylindrical inlet, which is set to (0 0 0) by default. If your mesh geometry is different, use the input vector to align it. The axis vector is to specify the direction of axial flow (0 0 1) being positive z. I usually search the forum to see if there are relevant posts, then I will look through the source code. Good luck, Alan |
|
March 3, 2011, 07:52 |
|
#4 |
Member
Alex
Join Date: Apr 2010
Posts: 48
Rep Power: 16 |
Hi Nir, the system I was talking about was cylindrical. Axis and center refers to the mesh ones. The axis is the z, also considered as axial.
|
|
March 3, 2011, 07:57 |
|
#5 |
Member
Alex
Join Date: Apr 2010
Posts: 48
Rep Power: 16 |
Hi Alan, the problem was not so trivial: if you consider the situation, what I needed was a flow with axial and tangential velocity. The axial velocity of 133 m/s and tangential one of 77 m/s. The tangential obtained in the BC of Cyl BC was not the right one, because it is depented on the radius of the inlet tube, meaning that if I have a rpm value and a diameter, this tangential velocity is radius dependent, while, what I actually need, is a uniform tangential velocity (which has to recreate the swirler conditions). What I would like to set up a tangential velocity as I could do for the radial one (see the lines). Do you think is it possible?
|
|
April 26, 2011, 11:41 |
cylindricalInletVelocity needs revision
|
#6 |
New Member
|
Alex, the case you described is exactly what I've wanted from the cylindricalInletVelocity condition. The best way I found was to just modify the source code. The modified library is attached.
Firstly, there are a few things that I have learned. 1) the center point is in Cartesian coordinates; very few, if any, OpenFoam utilities are in Cylindrical coordinates 2) at no point in the library is a component defined in Cylindrical coordinates. Rather, radial and tangential are defined in the form (x-contribution, y-contribution, 0) 3) the specification for the radial and tangential velocities are incorrectly scaled. Note below that the variable "d" is the relative radial-tangential distance between the cell-face center and the "centre". The "d" used in subsequent calculations should be replaced with a "dhat" where vectorfield dhat = d/mag(d) This adjustment should clear the radial-dependent scaling on the components. As contained in cylindricalInletVelocityFvPatchVectorField.C (I've added a few comments): // * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * // void Foam::cylindricalInletVelocityFvPatchVectorField:: updateCoeffs() { if (updated()) { return; } vector hatAxis = axis_/mag(axis_); //unit-vector of axial coordinate vectorField r = (patch().Cf() - centre_); //relative distance vector vectorField d = r - (hatAxis & r)*hatAxis; //subtract out axial component vectorField tangVelo = (rpm_*mathematicalConstant:: pi/30.0)*(hatAxis)^d; //recall: hatAxis^hatRadial=hatTangential, therefore tangVelo = omega*hatTangential operator==(tangVelo + axis_*axialVelocity_ + radialVelocity_*d); //splice xyz components from tangential-axial-radial fixedValueFvPatchField<vector>::updateCoeffs(); } The modified library allows for a more convenient specification, namely inlet { type cylindricalInletVelocity; axis (0 0 1); centre (0 0 0); radialVelocity -10; tangentVelocity 10; axialVelocity 30; value (0 0 0); //the value is not really necessary for the condition but OpenFOAM give me an error if I don't include it. } I've attached the new library folder. Simply unzip the folder into a convenient place and run wmake libso |
|
May 2, 2011, 12:01 |
|
#7 |
Member
Alex
Join Date: Apr 2010
Posts: 48
Rep Power: 16 |
Thanks Alex, it is very usefull!
considering I am not very familiar with the libraries, if I compile this version you attached, which has got the same name of the default one in OF, do you suggest me to change the name, or simply shall I compile and then the previous default one will be replaced? i will try to run simulation and check if it works, with the inlet values you gave me. thanks for the help! cheers, alessio |
|
March 28, 2012, 14:33 |
OpenFoam 2.1 version version
|
#8 |
New Member
|
In OpenFOAM 2.1, the compiling structure has changed to some degree. Attached is the drop-and-run source code for the cylindricalInletVelocity. Because OF2.1 has a native condition of the same name (which I have reservations against using for the reasons in a previous post), the name of the condition has been altered to cylindricalVelocityInlet.
1) uncompress the file to a convenient location. I use my openfoam user folder. 2) compile using: wmake libso 3) the boundary condition should compile smoothly. The condition can be applied to the velocity on a patch. in the initial condition specify type cylindricalVelocityInlet; axis (x y z); // axis of rotation centre (x y z); // axial center radialVelocity scalar; // V_r tangentVelocity scalar; // V_theta axialVelocity scalar; // V_z value uniform (0 0 0); // not necessary, but paraView results in an error without it |
|
March 25, 2013, 12:56 |
Use of classical cylindricalInletVelocity in OF 2.0.x
|
#9 |
New Member
Gregory Paladin
Join Date: Jul 2012
Posts: 10
Rep Power: 14 |
Hi Foamers !
I am trying to simulate a swirling flow with an anular inlet, and therefore I'd like to use the cylindricalInlet Velocity. (OF 2.0.x) I'll have to run my simulation on a cluster so I can't use any additional user library suggested above... Does anyone knows if this boundary condition works properly? Even when I change de rpm, the velocities, etc, i still get this error : Code:
Starting time loop Courant Number mean: 4.24721e-05 max: 0.0535831 deltaT = 2.85714e-06 Time = 2.85714e-06 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 --> FOAM FATAL ERROR: attempted copy of a deallocated temporary From function Foam::tmp<T>::tmp(const tmp<T>&) in file /Volumes/OF/OpenFOAM/OpenFOAM-2.0.x/src/OpenFOAM/lnInclude/tmpI.H at line 63. FOAM aborting Anyone has an idea? I am no OF expert, so I don't even understand what the error means... Thanks in advance ! |
|
March 25, 2013, 13:16 |
|
#10 |
New Member
|
What does your initial condition file for U look like?
The cylindricalInletVelocity of OF2.x should work. |
|
March 25, 2013, 13:55 |
|
#11 |
New Member
Gregory Paladin
Join Date: Jul 2012
Posts: 10
Rep Power: 14 |
Here is the burner geometry : http://cl.ly/NpGk
My swirling jet is between the bluff body (r=25mm) and the annular shroud (r=30mm) The axial velocity is 16.3m/s and the tangential velocity 25.9m/s. Axis is in the X direction. Here is my boundary condition in 0/U Code:
Pilot { type cylindricalInletVelocity; axis (1 0 0); centre (0 0 0); axialVelocity 16.3; rpm 8244; radialVelocity 0; value uniform (0 0 0); } RPM 8244 seems high but 25.9m/s tangential velocity for a 30mm annulus... I double checked the maths. I had to put a "value" keyword, otherwise it doesn't run. Thanks for your help |
|
March 25, 2013, 15:01 |
|
#12 |
New Member
|
After looking into it a bit further, I am noticing the same error with the native bc that is available.
The error is associated with the handling of the tangential component. In the source code: tmp<vectorField> tangVel ( (rpm*constant::mathematical:i/30.0)*(hatAxis) ^ d ); By some unknown reason, it is trying use this variable without allocating it properly. Unless you can modify the source code or use one of the user libraries above. I don't know what to suggest. |
|
April 24, 2013, 17:25 |
|
#13 |
Member
Vishal Achasrya
Join Date: Nov 2011
Posts: 38
Rep Power: 14 |
Why cant you use the user libraries on a cluster?
I know the installation is in a non-default place and the env vars are set based on those. But the *_USER dirs can be set to you where you want your src and lib folders to be and then when you "wmake libso" user codes, it would put them there. Then you can just add the appropriate .so files to your controldict and it should work. |
|
May 9, 2014, 04:02 |
|
#14 |
New Member
Join Date: May 2013
Posts: 1
Rep Power: 0 |
Hi Alex!
I'm using OpenFOAM 1.6-ext and I would also like to use your cylindricalInletVelocity BC. Have you already adjusted your version to OF 1.6-ext because there is a big difference to OF 2.x and my programming knowledge is a bit limited ? BR Markus |
|
May 14, 2014, 04:16 |
|
#15 |
Member
sirLentschi
Join Date: Nov 2010
Posts: 87
Rep Power: 15 |
Hello Markus,
you can find the appropriate file for OF-1.6-ext at http://www.cfd-online.com/Forums/ope...tml#post305143 |
|
August 28, 2014, 01:28 |
help
|
#16 | |
Member
Ndong-Mefane Stephane Boris
Join Date: Nov 2013
Location: Kawasaki (JAPAN)
Posts: 53
Rep Power: 12 |
Quote:
How would you proceed if your inlet velocity components were all functions of the radial direction: type cylindricalVelocityInlet; axis (x y z); // axis of rotation centre (x y z); // axial center radialVelocity scalar; // V_r =f1(r) tangentVelocity scalar; // V_theta =f2(r) axialVelocity scalar; // V_z=f3(r) Stephane |
||
February 10, 2015, 04:21 |
cylindricalInletVelocity
|
#17 |
Senior Member
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16 |
Hello Stephane,
were you able to adapt the BC with the radius dependant values? I would also need such a BC. Kind regards Chrisi |
|
May 7, 2015, 11:58 |
|
#18 | |
Member
Howar
Join Date: Mar 2015
Posts: 53
Rep Power: 11 |
Quote:
|
||
June 28, 2017, 05:57 |
strange tangential velocity
|
#19 |
Member
Join Date: Sep 2016
Posts: 63
Rep Power: 10 |
Dear Foamers,
I set the cylindricalInletVelocity as the following: lateral { type cylindricalInletVelocity; axis (0 0 1); centre (0 0 0); axialVelocity constant 0; radialVelocity constant 0.3; rpm constant 955; } The radius of the cylindrical boundary is 3mm. Therefore the tangential velocity is the same as the radial velocity, and the velocity vector at this boundary should be 0.42m/s, with 45° deviating from the tangential/normal direction of the boundary. However the resulting inlet velocity was 0.37m/s and closer to the normal direction of the boundary, as you can see in the attached image. Did I misunderstand something? I would appreciate if anybody can give me some suggestions! Best regards, sitajeje |
|
July 3, 2018, 09:48 |
Accuracy of the results regarding inlet volumetric flow
|
#20 |
New Member
Matthias Frechen
Join Date: Jan 2013
Posts: 1
Rep Power: 0 |
Hi All!
We usally use cylindricalInletVelocity for square swirl diffusers, but we are not totally convinced by the accuracy of the results regarding inlet volumetric flow when using a single square inlet area. The resultant inlet volumetric flow we see in Paraview seems to be about 20- 30% to low compared to the axialVelocity we put in the input file. Does anyone tried to use swirlFlowRateInletVelocityFvPatchVectorField or groovyBC for swirl diffusers or a different approach with promising results? Regards Matthias |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Superlinear speedup in OpenFOAM 13 | msrinath80 | OpenFOAM Running, Solving & CFD | 18 | March 3, 2015 05:36 |
Cross-compiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingw-w64 | wyldckat | OpenFOAM Announcements from Other Sources | 3 | September 8, 2010 06:25 |
Modified OpenFOAM Forum Structure and New Mailing-List | pete | Site News & Announcements | 0 | June 29, 2009 05:56 |
64bitrhel5 OF installation instructions | mirko | OpenFOAM Installation | 2 | August 12, 2008 18:07 |
Adventure of fisrst openfoam installation on Ubuntu 710 | jussi | OpenFOAM Installation | 0 | April 24, 2008 14:25 |