[babakflame]

Dear Fellows

I have a circular inlet with a radius R=4 mm which is surrounded by an annulus and I have an inlet boundary file from experimental data as:

PHP Code:

r[m]        <U>[m/s]      <u">[m/s]     <V>[m/s]     <u"v">[m2/s2] 
    0.0000       51.3500        2.4271        0.3063       -0.9264 
    0.0003       51.5537        2.5904        0.3310        0.9904 
    0.0005       51.1199        2.6052        0.2284        0.7745 
    0.0008       50.7026        2.7016        0.2807        0.7238 
    0.0010       50.2622        2.9098        0.3242        2.5900 
    0.0013       49.8528        3.2504        0.2703        3.2164 
    0.0015       49.1442        3.4229        0.2676        2.9736 
    0.0018       48.3404        3.6807        0.2456        3.7594 
    0.0020       47.4366        3.7990        0.2525        4.2001 
    0.0022       46.1662        4.0460        0.1636        4.9178 
    0.0025       44.9207        4.1902        0.2234        4.8890 
    0.0027       43.1457        4.5092        0.0299        5.3801 
    0.0030       41.5304        4.6757        0.0201        5.1691 
    0.0032       39.2590        4.8087       -0.0004        5.5684 
    0.0035       36.2186        5.1897       -0.0851        5.6541 
    0.0037       31.1781        6.2540       -0.0154        5.8344 
    0.0040       15.5284        5.9890        0.2606        2.1353 
    0.0043        1.8618        0.5309       -1.2781        0.0585 
    0.0045        0.6689        0.2316       -1.8449       -0.0291 
    0.0050        0.5267        0.2335       -1.0840        0.0122 
    0.0060        0.3520        0.0847       -0.1164        0.0057 


would somebody PLZ hint me how can I define my velocity inlet values in OpenFOAM correctly from this file?

Best,
Bobi

[Tobi]

Dear Bobi,

you can handle some inlet bc with groovy.
At the moment I think you have the ability to do it by your own that means defining all velocitys manual in groovy. Maybe you also have some abilitys to get access to your data file and make it easier. At least may be there is some available BC for OpenFOAM like codedFixedValue.

My first suggestion is using groovy BUT I remember that there was some BC that uses values out of a file (maybe just time dependend variables).

For groovy you should have sth. like:

type groovyBC;
valueExpression "pos().x < 0.0003 ? vector(0 51.35 0) : pos().x < 0.0005 ? vector(0 51.5531 0) . . . : 0.3520";
value uniform (0 0 0);

You also can use some variables etc. I think Bernhard has much more nicer solutions in groovy than mine. But it will work.
If you can make a fitting curve (polynomial or other function), then you can implement the function and let the function do all the work like:

type groovyBC;
variables "f= 42*pow(e,pos().x-0.23);e=2.71828182845904";   // just an example
valueExpression "vector(0, f, 0)";
value uniform (0 0 0);

[babakflame]

Dear Tobi

Many thanks for your kind hints.

Actually, I was familiar with groovyBC. Accordingly, I have used this formulation which is derived from poiseuille fully developed flow. However, this formulation is not sufficiently accurate. (In this formulation Y-axis is the axis of Cylinder). This is the formulation I have used:

FUEL
    {
        type                groovyBC;
        variables        "Vm=54;Xp=pos().x;Zp=pos().z;h=0.004;a=-Vm/(h*h);b=Vm;";    
    fractionExpression    "1";
    valueExpression        "vector(0, a*((Xp*Xp)+(Zp*Zp))+b, 0)";
    value            uniform (0 0 0);

    }

Nonetheless, My preference is using input files since I am working on LES error simulation. I have read this link:
http://www.openfoam.org/version2.1.0...conditions.php

However, My problem is the format of input file I tried some but the file format was not accepted. Have you ever done this before, If hopefully yes is it possible to upload a file according to the following :

CSV file

uniformValue csvFile;
csvFileCoeffs
{
fileName "$FOAM_CASE/myDataFile"
outOfBounds clamp;
hasHeaderLine true;
refColumn 0;
componentColumns (0 1 2); // vector example
}



polynomial

uniformValue polynomial // y = 0.1 + 1.3x^2 + 2.7x^3
(
(0.1 0)
(1.3 2.0)
(2.7 3.0)
);



Best Regards
Bobi

[wyldckat]

Greetings to all!

@Bobi:

1. Which OpenFOAM version are you using?
2. Have you read this thread: http://www.cfd-online.com/Forums/ope...ross-wind.html - it gives details on how to use CSV for a boundary condition.

Best regards,
Bruno

[babakflame]

Dear Bruno

Many thanks for your quick reply.

1. I am using OpenFOAM 2.1.x

2. I am going to take a deep look at your link.

Best Regards
Bobi

[babakflame]

Dear Bruno

Many thanks for your link. I read your link carefully. Nonetheless, your link was about time dependent inlet velocities. I think this does not work out for me quite well, since my case (the uploaded file in the first post of this thread) does not vary with time but vary with location. The only thing that comes to my mind is changing the header of your example from:

Time, Ux, Uy, Uz

to:

X, Y, Z, Ux, Uy, Uz

and put the vectors of location in the columns related to space coordinates ( I mean X, Y, Z)

However, is it correct ,i mean is this the way to define space dependent inlet boundary files?

Any hint is appreciated.

Best Regards
Bobi

[wyldckat]

Hi Bobi,

Oh, sorry, I didn't notice that important detail

OK, then AFAIK, there isn't a BC ready made in OpenFOAM 2.1.x to do that.
You'll have to code your own BC. You can use as references the following BCs:

• "parabolicVelocity", for ideas on how to build your own BC: Compile boundary condition as a new dynamic library post #10
• "uniformFixedValue", for ideas on how to use the table values, i.e. from CSV file. This BC is located at "src/finiteVolume/fields/fvPatchFields/derived/uniformFixedValue".
• There is a BC introduced in OpenFOAM 2.2 or 2.3, named "externalCoupledMixed". The related tutorial is "heatTransfer/buoyantSimpleFoam/externalCoupledCavity".

There is also the tutorial "incompressible/simpleFoam/pitzDailyExptInlet", but this requires you to change from CSV to the specific format that OpenFOAM uses.

I don't have enough time to look further into this myself

Good luck! Best regards,
Bruno

[Mitchell Baum]

Hi Bobi,

I also require a similar application of a time independent, spatially varying inlet velocity profile which I have determined from experimental data. Have you made any further progress on this since your last post?

Any guidance is greatly appreciated!

Kind regards,
Mitchell