[openfoammaofnepo]

Hi All,

In OpenFOAM, when I have the three dimensional fields, say velocity, can we interpolate a 2D slice from the 3D results during the post process stage? Thank you so much.

OFFO

[openfoammaofnepo]

Anybody knows this?....

[wyldckat]

Hi OFFO,

I'm going to use this thread of yours to answer both the original question and the questions you've sent me via PM.

First about the original question here:

Originally Posted by openfoammaofnepo

can we interpolate a 2D slice from the 3D results during the post process stage?

It really depends on the time of interpolation you're looking for. If you want to do a slice similarly to how it's done with ParaView, then you can either use the sample utility or the respective function object. You've got several solutions to choose from: https://github.com/OpenFOAM/OpenFOAM...ple/sampleDict - but I guess the main ones you're looking for would be:

• cuttingPlane
• sampledTriSurfaceMesh

As for the questions asked via PM:

Originally Posted by openfoammaofnepo

Probably you know the Openfoam utility "patchIntegate", which can be used to calculate the mass flow rate when we use it for "phi". However, this calculation is only for the boundary surfaces. If I would like to calculate an internal surface, is this possible?

My answer was:

Quick answer: you need to create a faceZone and use the respective function object.
Since you didn't specify a thread where you asked about this, I won't point you to one or two that already talk about this

Then you asked:

Thank you so much for your reply. When you say "create a faceZone", do you mean I need to have a face (created when generating the mesh) for that location ?

I use ICEM CFD to generate the mesh. So I can create an internal face there. Is this the faceZone you mentioned? For the internal face, there is a problem. It does not appear in the constant/polymesh/boundary. So this is not a boundary and then we cannot use patchIntegrate to get the mass flow rate over that surface.

A few reference posts where I and other people have already written about this (i.e. continue reading the threads starting from that post):

• http://www.cfd-online.com/Forums/ope...tml#post459086 - post #24
• http://www.cfd-online.com/Forums/ope...tml#post425251 - post #4

The faceZones should not appear in "constant/polymesh/boundary", they should appear in "constant/polymesh/faceZones".

If you want to use the utility patchIntegrate, then you will need to convert the faceZone to a baffle and define the boundary conditions for the new double-sided patch to be cyclic. Sorry, I'm in a hurry right now and I'm not able to look for a good example on how to do this. Search for createBaffles or run:

find $FOAM_TUTORIALS -name "createBafflesDict"

Best regards,
Bruno