[tH3f0rC3]

Hi,

it is possible to show the temperature field on a surface with paraFoam.
But is it possible to put out a value of the temperature on a selected point?

I want to know the temperature on several points. Up to now I can only compare the color with the color legend. But this is not that precise!

Best Regards,
tH3f0rC3

[MartinB]

Hi,

you can select several points on the surface with the "Select points on" button, see red arrow in attached screenshot.

Use "Filters->Alphabetical->Extract Selection" to get an entry in the Pipeline Browser. Click "Apply" in the Object Inspector.

In the "Information" tab you have information about the selected point(s).

With a spread sheet view you can see detailed information about your selected points like position in space or field values.

To visualize the selected points mark the "ExtractSelection" entry in the Pipeline Browser and select "Filters->Alphabetical->Glyph" filter. Select type "Sphere" from the Glyph Type drop down menu, set an appropriate value for "Radius" and activate "Set Scale Factor" with value 1 (see second screenshot, red markers).

Be aware, that all values at points are interpolated. For exact evaluation you might need to use cell values instead of point values.

Martin

[Bernhard]

Alternatively you can use the sample utility to probe at predefined locations. You can do that after the simulation or during runtime.

[tH3f0rC3]

I'm afraid it doesn't work.
Can you guess what I'm doing wrong?

As soon as I have marked the points paraView crashes down and puts out an error message:
/OpenFoam/bin/paraFoam: line 119: 20766 Segmentation fault praview --data=$caseFile"

Best Regards,
tH3f0rC3

[MartinB]

Hmmmhhhh,

can you make a try via foamToVTK and paraview instead of paraFoam? Just import the wall surface from the VTK folder... is ParaView crashing again?

Or can you try to import only the patches, but not the internal mesh in paraFoam?

Martin

[tH3f0rC3]

Originally Posted by MartinB

Hmmmhhhh,

can you make a try via foamToVTK and paraview instead of paraFoam? Just import the wall surface from the VTK folder... is ParaView crashing again?

Or can you try to import only the patches, but not the internal mesh in paraFoam?

Martin

I have now tried by importing only the patch. This doesn't work.

What do you mean with foamToVTK instead of paraFoam?

Best Regards,
tH3f0rC3

[MartinB]

With the OpenFOAM utility foamToVTK you convert the results into native Paraview file format. Type in your shell:

foamToVTK

and you will get a new folder named "VTK", and there are all patches separated. Then you start paraview by typing:

paraview

in your shell. Not paraFoam, but paraview. Import one of the vtk files with "File->Open" and give this one a try.

If this fails, you might even want to try it with a windows version of ParaView, since you can easily handle the VTK files in a windows environment, sometimes with even better perfomance than in a Linux environment.

Good luck

Martin

[tH3f0rC3]

It is probably due to the chtMultiRegionSimpleFoam-solver I use, that the foamToVTK doesn't work.
chtMultiRegionSimpleFoam has an other file structure than for example simpleFoam.

error message:
Cannot find file "points" in directory "polyMesh" in times 0 down to constant

I even don't understand the error message. Why does foamToVTK search down to constant for a file 0? I think tThis doesn't make sence.

Best Regards,
tH3f0rC3

[MartinB]

In this thread you can find the usage of foamToVTK with chtMultiRegionFoam:
http://www.cfd-online.com/Forums/ope...ltiregion.html

To check if the selection mode does work in other situations you can make a quick try this way:
- click "Sources->Cylinder", then click "Apply"
- click "Filters->Alphabetical->Tetrahedralize"
- test the "Select points on" function.
Does Paraview crash again?

Martin

[tH3f0rC3]

1.- For main mesh (region0)
~/.../caseDirectory $ foamToVTK -case caseName

2.- For other meshes
~/.../caseDirectory $ foamToVTK -case caseName -region otherMeshName

3.- Visualization with ParaView
Open: caseDirectory/CaseName/VTK/caseName*.vtk
Open: caseDirectory/CaseName/VTK/otherMeshName/caseName*.vtk
Use Paraview filter: GroupDataSet to join both meshes results.

This is what I've found.
But what is meant with caseDirectory? the file where 0 constant and system lies?
And what is meant with -case? I have three regions in my case.

Best Regards,
tH3f0rC3

[MartinB]

But what is meant with caseDirectory? the file where 0 constant and system lies?

Yes. You don't type it, it's just the location in your file system. The command itself starts behind "$".

And what is meant with -case? I have three regions in my case.

May be, it's an ancient parameter, don't know... try

foamToVTK -region Your_Region_Name

If it does not work, try

foamToVTK -case The_Folder_Name_in_Which_Your_Simulation_Is_Locate d -region Your_Region_Name

Does the other quick test run, i.e. can you select points in another Paraview dataset?

Martin

[tH3f0rC3]

Hi,

I'm afraid it hasn't worked up to now.

But I recieved a mail, where another idea was described. I tried this idea and succeded:

Use FILTER -> ProbeLocation
set point and rescale to data range

That's it.
Be careful to use the patch not the volume.

Best Regards,
tH3f0rC3