[gu1]

Originally Posted by wyldckat

Hi Vimal,

Of course! The mapped BC, I wasn't remembering it. One such tutorial is "incompressible/pisoFoam/les/pitzDailyMapped".
And as of OpenFOAM 2.2, you can find more details about boundary conditions and function objects here: http://foam.sourceforge.net/docs/cpp/modules.html

What you're looking for is in the section Coupled boundary Conditions

The general idea is that:

1. You define in the file "constant/polyMesh/boundary" the geometrical relation between two patches, where one is the slave and the other the master.
   The offset is defined here and is the indication of the relative position between the current patch and the other patch. For example, if your "inlet" is at "X= -5.0m" and the "outlet" is at "X=+10.0m", and if the "inlet" is the one that is defined as the "mappedPatch", then the offset is "(15.0 0 0)". Well, actually, it might have to be "(14.99 0 0)", so that the offset point falls inside the cells that are near the "outlet" patch.
   If the "outlet" was the "mappedPatch", then the offset would be "(-15.0 0 0)"... I mean, "(-14.99 0 0)".
2. As for the type you defined for the "inlet" in "0/U", it depends on the specific mapped type you're looking for, as listed in the Coupled boundary Conditions.

Best regards,
Bruno

Hi Bruno,

I have doubts related to mapped BC and maybe you can help me.
I have attached an image (Fig.1) of my domain and below are the settings that I used in OpenFOAM so that it was possible to use such a BC.
*I left the grid so you can see the dimensions of my domain.

blockMeshDict:
    inlet
    {
        type mappedPatch;
        offset          (0 0.1 0);  EDIT 1: The ERROR is here.
        sampleRegion    region0;
        sampleMode      nearestCell;
        samplePatch     none;
        faces
        (
            (0 1 14 13)
            (1 2 15 14)
        );
    }

0/U:
    internalField   uniform (0 0 0);

    inlet
    {
        type            mapped;
        field           U;
        setAverage      1;
        average         (3.45 0 0);
        interpolationScheme cell;
        value           uniform (3.45 0 0);
    }

0/k:
    internalField   uniform 0.04;

    inlet
    {
        type            fixedValue;
        value           uniform 0.04;
    }

Well, from the results, it's clear that what I wanted to do did not work. EDIT 1: Solved.
My intention was that with this BC being able to develop the velocity profile at the inlet.

I put the mapping point above the step, Is it interesting to use this point so close to the entrance?
Unfortunately I was trying to import a velocity profile that I developed into a channel, but it was not succeeding and so I resorted to this option.
Can you suggest something beyond this BC? Unfortunately the mapFields function, as far as I understand, can not import only the U profile from a channel to my inlet backward facing step.

Two other issues are:
Would it be interesting to use directMapped?
From the moment I decided to use this BC, when should I add the mapped condition to my files (k, epsilon ...)? Because I'm just adding in U.

Thanks.

[Moderator note: Moved from simple open channel flow, the inlet and outlet are periodic ]

[gu1]

Hi,

Below I've attached two images of two cases I'm working on.
One of the images contains the velocity profile for the channel (v2f-newtoniano) and the other one is a backward facing step (pitzDailyMapped) also using the same model (v2f Model). Both cases have the same BC and both are set to a Re_tau = 395.

The channel domain is cyclic, different from that used in the backward facing step geometry.
In backward facing facing geometry was used to mapped BC, according to the code below.

blockMeshDict:
    inlet
    {
        type mappedPatch;
        offset          (-0.05 0 0); 
        sampleRegion    region0;
        sampleMode      nearestCell;
        samplePatch     none;
        faces
        (
            (0 1 14 13)
            (1 2 15 14)
        );
    }

0/U:
    internalField   uniform (0 0 0);

    inlet
    {
        type            mapped;
        field           U;
        setAverage      true;
        average         (3.45 0 0);
        interpolationScheme cell;
        value           uniform (3.45 0 0);
    }

0/k:
    internalField   uniform 0.04;

    inlet
    {
        type            mapped;
        field           k;
        setAverage      false;
        average         0.04;
        interpolationScheme cell;
        value           uniform 0.04;
    }

0/epsilon:
    internalField   uniform 0.4;

    inlet
    {
        type            mapped;
        field           epsilon;
        setAverage      false;
        average         0.4;
        interpolationScheme cell;
        value           uniform 0.4;
    }

0/v2:
    internalField   uniform 0.024;

    inlet
    {
        type            mapped;
        field           v2;
        setAverage      false;
        average         0.024;
        interpolationScheme cell;
        value           uniform 0.024;
    }

Why did the velocity profile diverge? The inlet channel of the backward facing step geometry has the same mesh division at Y (y+ <1) as that used for the channel geometry and therefore also has the same height H (0.2 m).
*Remembering again that the same BCs are being used on the wall for both cases.

NOTE: I used the mapped BC for the first time, and the intention was to develop the velocity profile at the inlet geometry (backward facing step), since I am not able to import the channel velocity profile (Could someone advise me here?).
Would it be interesting to use BC directMapped?
Are the conditions I used for k, epsilon, and v2 correct?

Thanks

[wyldckat]

Quick answers:

Originally Posted by gu1

Can you suggest something beyond this BC? Unfortunately the mapFields function, as far as I understand, can not import only the U profile from a channel to my inlet backward facing step.

If your inlet is using a fixed value and your first channel has the last cell overlapping the patch faces on your second case, then it should work... that's what the cut patches (can't remember the exact name) are for... although I never used it myself. The idea is that it would then interpolate the values from one mesh to the other one.
Having the two patches overlap would be a problem.

Originally Posted by gu1

Would it be interesting to use directMapped?

I only have the vague idea that it requires strict mapping...

Originally Posted by gu1

From the moment I decided to use this BC, when should I add the mapped condition to my files (k, epsilon ...)? Because I'm just adding in U.

Mapping only U should be enough, since the other properties can be inferred during simulation... and mapping all others also can potentially cause serious difficulty to converge or generate unexpected flow profiles...

You could also have two meshes within the same case, and having the mapping be done from one mesh to the other one on the patch you have right now... If blockMesh doesn't let you generate the two independent blocks, then you can simply merge the meshes of two cases into a single one, without stitching.

[gu1]

Originally Posted by wyldckat

You could also have two meshes within the same case, and having the mapping be done from one mesh to the other one on the patch you have right now... If blockMesh doesn't let you generate the two independent blocks, then you can simply merge the meshes of two cases into a single one, without stitching.

To do this, without an example, would be quite complex for me. It's my first contact with blockMesh... but thank you for your response.

Incidentally, I even generated a new topic in the forum... if you want to give an opinion, I would be very grateful. LINK.

[wyldckat]

Quick answer: Now I'm just confused... if you have a backward step case, you cannot map the velocity field within the same mesh, because the channel widens and therefore changes the profile velocity... it's pretty much a physical reality, therefore it's borderline impossible for that to ever converge...


I've now remember of something that has been released with OpenFOAM 6 and is documented in the respective commit: https://github.com/OpenFOAM/OpenFOAM...a0d9e72d5a7968

Unfortunately I don't have the time needed to work out an example case for this boundary condition
But the tutorial case "incompressible/simpleFoam/pitzDailyExptInlet" can be used as a basis for creating such a case.