How can I extract the Cp distribution plot around an airfoil from a VTK file using Paraview?

I have seen in other discussion pages that they can do it extracting the block or selecting the surfaces of the airfoil. However, in my VTK file I do not have those. I only have the fluid domain around the airfoil. Does anyone know how to extract the pressure distribution around an airfoil with the domain file I am attaching below?

Thank you in advance.

domain_00000080.vtm (4.0 KB)

You need to share the associated files : domain*.vti

1 Like

Thank you Mathieu. However, the software I am using to perform the simulation (called PALABOS) only generates .vtm files in this example. Is there something that I could do with the .vtm files?

alongside your .vtm file, there is a folder named domain_00000080, share it please.

1 Like

Oh you are right! These files below are the ones inside the folder domain_00000080.

domain_00000080-g001-00000000.vti (70.6 KB) domain_00000080-g001-00000001.vti (2.3 MB) domain_00000080-g001-00000002.vti (70.6 KB) domain_00000080-g001-00000003.vti (70.6 KB) domain_00000080-g001-00000004.vti (2.3 MB) domain_00000080-g001-00000005.vti (2.3 MB) domain_00000080-g001-00000006.vti (1.8 MB) domain_00000080-g001-00000007.vti (1.8 MB) domain_00000080-g001-00000008.vti (1.8 MB) domain_00000080-g001-00000009.vti (70.6 KB) domain_00000080-g001-00000010.vti (70.6 KB) domain_00000080-g001-00000011.vti (2.3 MB) domain_00000080-g001-00000012.vti (2.3 MB) domain_00000080-g001-00000013.vti (70.6 KB) domain_00000080-g001-00000014.vti (12.3 KB) domain_00000080-g001-00000015.vti (2.3 MB) domain_00000080-g001-00000016.vti (385.6 KB) domain_00000080-g001-00000017.vti (1.8 MB) domain_00000080-g001-00000018.vti (1.8 MB) domain_00000080-g001-00000019.vti (1.8 MB) domain_00000080-g001-00000020.vti (312.7 KB) domain_00000080-g001-00000021.vti (73.3 KB) domain_00000080-g001-00000022.vti (2.3 MB) domain_00000080-g001-00000023.vti (73.3 KB) domain_00000080-g001-00000024.vti (73.3 KB) domain_00000080-g001-00000025.vti (2.3 MB) domain_00000080-g001-00000026.vti (2.3 MB) domain_00000080-g001-00000027.vti (1.9 MB) domain_00000080-g001-00000028.vti (1.9 MB) domain_00000080-g001-00000029.vti (1.9 MB) domain_00000080-g001-00000030.vti (73.3 KB) domain_00000080-g001-00000031.vti (73.3 KB) domain_00000080-g001-00000032.vti (2.3 MB) domain_00000080-g001-00000033.vti (2.3 MB) domain_00000080-g001-00000034.vti (73.3 KB) domain_00000080-g001-00000035.vti (12.8 KB) domain_00000080-g001-00000036.vti (2.3 MB) domain_00000080-g001-00000037.vti (400.1 KB) domain_00000080-g001-00000038.vti (1.9 MB) domain_00000080-g001-00000039.vti (1.9 MB) domain_00000080-g001-00000040.vti (1.9 MB) domain_00000080-g001-00000041.vti (324.4 KB)

please share an archive containing all your files together for simple access, thanks.

Sorry, I will compress it.

The file is too large so I uploaded it here.

So, you dataset indeed contains only the fluid domain. To extract the pressure at the airfoil you would need to share the airfoil geometry as well.

1 Like

Okay. You mean this file, right?

30P30N_modified_slat_configF_0p2m_AoA5p5.stl (1.4 MB)


  • Open your .stl file, Apply
  • Open your .vtm file, Apply
  • Make sure the .vtm file is highlighted in the pipeline browser
  • Filters -> ResampleWithDataSet
  • Click on destination mesh and select the .stl file
  • Apply
  • Color by pressure

1 Like

Thank you! I followed your steps and I got the same! However, what I was actually looking for was: how could I extract those pressure values to generate a 2D Cp vs X/c distribution?. Is there any option inside Paraview to get those values (as well as their position in x)?

Thank you again Mathieu!

Please precise what your are trying to achieve.

Hi @Victor - regarding the 2D Cp vs X/c distribution once you have your pressure applied to the geometry, did you try the “Plot On Intersection Curves”? (Filters -> Alphabetical -> Plot On Intersection Curves)

Judging from the screenshot above, you could set the plane to Z Normal and select your z-slice locations. I think by default, it will try to plot everything so you can untick all the series you don’t want. You’ll also need to set the x-axis X Array Name to Points_X.

Hope that helps a bit!