[kac24]

Hi,

I wrote a very similar post a couple of days ago on pre-processing forum. I went through a range of issues and here >

Case is supposed to simulate heat transfer in standard heating pipe (copper, 15mm diameter).


The error that I am getting is:
--> FOAM FATAL ERROR: (openfoam-2306)

failed lookup of phi (objectRegistry pipe)
available objects of type surfaceScalarField:
0()


From const Type& Foam:bjectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::GeometricF>
in file /home/k/kac24/codes/v2306-alice3/OpenFOAM-v2306/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line>

FOAM exiting

The case is very similar to tutorial case tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater

The commands I am using are:
blockMesh
topoSet
restore0Dir
splitMeshRegions -cellZones -overwrite
changeDictionary -region water
changeDictionary -region pipe
chtMultiRegionFoam

(the last one mostly because I can't get parallel to work)

My suspition is with boundary condition for p_rgh:

inlet
{
type fixedFluxPressure;
}

[peterhess]

Hello!

The values of p & prgh in your case have both the value 0.

That means it is absolutely vacuum.

Increase them to the 1e5.

Take a look to the tutorial:

multiRegionHeater

Most likely stored here:

/usr/lib/openfoam/openfoam2306/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/

and use the default setups.

Regards
Peter

[kac24]

Thank you for your help, I really appreciate it. Unfortunately, after changing the pressure I still encounter the same error. Do you have any other ideas?

[peterhess]

Upload the case please and let me have a closer look.
The whole case please.
Regards
Peter

[kac24]

I have finally managed to solve it:

The issue was:

file: solid/T

outlet
{
type inletOutlet;
inletValue uniform 333.15;
value uniform 333.15;
}

patch outlet is called outlet only because it was easier for me to call it that for the sake of fluid region.

inletOutlet boundary condition can not be used in solid region.