ParaView for OpenFOAM: quantitative analysis and scientific post-processing

Third operating guide on OpenFOAM installed on a Linux server and used from Windows. The first explains how to connect ParaView to the server through an SSH tunnel; the second how to monitor the run and its convergence. This one covers the next step: using ParaView to measure, with OpenFOAM Foundation 14 and ParaView 5.13.2.

ParaView: quantitative analysis and scientific post-processing
From computed fields to reproducible measurements — OpenFOAM Foundation 14 and ParaView 5.13.2
Edition: 16 October 2026 · General operations handbook · Windows client / Linux server

Purpose. Use ParaView not only to visualize simulations but also to extract velocity profiles, cross-sectional averages, flow rates, pressure drops and recirculation regions. CFD cases remain on the Linux server while most interaction takes place on Windows. This guide assumes that FileZilla, PowerShell/SSH and starting pvserver are understood from Guide 1. Visual Studio Code is not required.

Reading path. Chapters 1, 2, 4, 5 and 9 form the minimum workflow. Chapters 6–8 provide three independent hands-on exercises. Background boxes are optional for readers already familiar with fluid dynamics. Original figures are schematic or analytical, not the output of CFD runs executed for this handbook.

1. Rule one: a visualization is not a measurement

A coloured field is excellent for orientation but does not establish a loss coefficient, conservation of mass or agreement with theory. Record the case name, time or iteration, field and physical units, geometrical region, filter, filter settings, extracted quantity and any reference used for comparison.

Background — measurements depend on the integration domain. Integrating pressure over a surface yields pressure × area, not pressure. Divide by surface area to obtain area-weighted mean pressure. Integrating the normal component of velocity over a surface yields volumetric flow rate.

2. Opening a case from Windows through pvserver

2.1 Before connecting

The ParaView client and server must have compatible versions, preferably exactly the same version (5.13.2 in this guide). On Linux, check:

foamVersion
pvserver --version
cd ~/cases/myCase
pwd
ls -d 0 constant system

A placeholder file may be created in the case directory to trigger ParaView’s native OpenFOAM reader:

touch myCase.foam

This empty file is a pointer to the case directory; it is not a results file. The actual reader must exist on the server because that is where file I/O occurs. OpenFOAM’s separately compiled paraFoam/PVFoamReader integration is a different route and may have different version constraints. If no reader works, consider foamToVTK and verify which arrays were exported. For decomposed parallel cases check the native reader’s reconstructed/decomposed case options.

2.2 Example secure connection

Start pvserver on the Linux host in a persistent terminal session:

pvserver --server-port=11111

In another Windows PowerShell terminal, start a local SSH tunnel and keep the terminal open:

ssh -N -L 11111:127.0.0.1:11111 USER@SERVER

In Windows ParaView choose File → Connect → Add Server, connection type Client / Server, host localhost, port 11111, then Connect. The SSH tunnel and the Linux server’s network/firewall rules must be correctly configured: do not expose the raw pvserver port directly to the Internet. If local port 11111 is busy, use 11112:127.0.0.1:11111 and connect locally to port 11112.

Once connected, File → Open browses the Linux server’s filesystem, not Windows drive C:. Open myCase.foam, click Apply, and enable the required regions and arrays. If p or U appears to be missing, inspect reader properties, selected timesteps and regions.

Efficiency rule. Apply filters on the server, export small CSV datasets and retrieve them with FileZilla when needed. Avoid routinely copying complete 3D simulation cases onto Windows.

pvserver --server-port=11111 --bind-address=127.0.0.1

3. Understand the underlying arrays first

1. Select the case source in the Pipeline Browser and consult Information: check bounds, time, cell/point counts and available fields.
2. Check the actual dimensions in OpenFOAM field files (0/p, 0/U etc.). A ParaView colour bar usually shows only the field name, not a verified physical unit.
3. Determine whether fields are Cell Data or Point Data. Cell Data to Point Data interpolates cell values; useful for visualization, but not identical to the source discrete values.
4. Display Surface With Edges to inspect the mesh, then Surface for results. Specify consistent colour ranges and record units.
5. In nominally 2D cases using extruded meshes with empty boundaries, distinguish the computational extrusion thickness from the apparatus’s true physical width.

Background — kinematic pressure. Many incompressible OpenFOAM cases store p in m²/s² (kinematic pressure). At constant density rho, a pressure difference in pascals is DeltaP [Pa] = rho [kg/m³] × Deltap [m²/s²]. Check the actual field dimensions in compressible and other model configurations; never multiply every pressure by density unconditionally. Pressure differences are independent of a consistently applied additive pressure reference.

Useful exploratory filters

• Slice: select an origin and a plane normal; this samples an interior section. Areas blocked by solids are not part of the fluid section.
• Clip: removes part of a dataset to reveal the interior; it does not automatically produce the desired measurement section.
• Threshold: isolates cells in a chosen scalar range. Selection semantics depend on point/cell association and inclusion settings.
• Gradient: computes derivatives and, optionally, divergence, vorticity and Q-criterion. Derivatives are especially sensitive to the mesh and any interpolation.

4. Extracting profiles and making graphs

4.1 Plot Over Line

Select the source containing U, usually the case or fluid-region branch. Choose Filters → Data Analysis → Plot Over Line, or find it through the filter search. Define endpoints such as (x0,y0,z0) and (x1,y1,z1), set an initial resolution of about 100–300 samples, then click Apply.

In Line Chart View, select only the desired component (usually U_X, or the X component of U in the reader) or velocity magnitude. Inspect the horizontal axis: label it as distance along the line or an appropriate coordinate rather than assuming the two are interchangeable. Samples outside the fluid domain may be invalid or separated by gaps: do not bridge solids by blind interpolation.

To export values, select the PlotOverLine output, then File → Save Data… and a CSV writer. Check point/cell association and selected output arrays. Column headings vary by reader and ParaView version, so inspect the exported file before downstream calculations.

4.2 Probe and time dependence

Probe samples the field at a specified location. Verify that the point actually lies in a fluid cell. For changing solutions, explore Plot Selection Over Time or OpenFOAM’s postProcessing/probes files (Guide 2). A Plot Over Line graph at one time is a spatial profile, not a time history.

4.3 Calculator and derived variables

Calculator creates an array from existing fields. For flow aligned with X, select the X component of U from the UI rather than typing an assumed component spelling that could differ across readers. Give the new array a descriptive name such as U_axial. For an incompressible constant-density case with kinematic pressure, a field p_Pa = rho × p can be calculated using the documented numerical value of rho. Do not apply this conversion in the wrong physical model.

# profile.py  -  run on the server:  pvbatch profile.py   (or pvpython)
from paraview.simple import *

case = '/home/USER/cases/caseName/caseName.foam'
r = OpenFOAMReader(FileName=case)
r.MeshRegions = ['internalMesh']
r.CellArrays = ['p', 'U']
r.UpdatePipelineInformation()
t = r.TimestepValues[-1]                 # last written time

pol = PlotOverLine(Input=r)
pol.Point1 = [0.08, -0.001, 0.0]         # line end points: adapt them to your domain
pol.Point2 = [0.08,  0.001, 0.0]
pol.Resolution = 200
pol.UpdatePipeline(t)

SaveData('/home/USER/cases/caseName/profile_x080.csv', proxy=pol,
         PointDataArrays=['U', 'p', 'arc_length', 'vtkValidPointMask'])
print('wrote profile_x080.csv at time', t)

5. Section means, pressure drop and flow rate

On a fluid cross section S, area-weighted mean pressure and volumetric flow rate are

[ \overline{p}_S = \frac{\int_S p\,dA}{\int_S dA}, \qquad Q_S = \int_S \mathbf{U}\cdot\mathbf{n}\,dA. ]

Integrate Variables produces the integrals, not a ready-made average. For a plane perpendicular to X, integrating the U_x component yields a signed volumetric flow rate according to your chosen +X convention; for arbitrary planes use the component normal to the surface.

Procedure with unambiguous definitions

1. Apply Slice to the original case using plane normal X at x = x_A. Confirm that the output is the intended fluid cross section, excluding solid blocks and irrelevant boundaries. When a suitable inlet/outlet patch is already present, Extract Block may be preferable.
2. Apply Integrate Variables to this Slice. Inspect the integral of pressure in Spreadsheet View/Information, and obtain the Area when exposed by the filter. If necessary, use Calculator on the same slice to create a constant array one = 1 and integrate that as the area. Compute p_mean = integral(p)/Area.
3. Repeat at x = x_B with the same definitions and obtain Delta p = p_mean,A − p_mean,B. Convert to Pa if, and only if, p is kinematic pressure and density is constant.
4. Use Calculator on a section normal to X to obtain U_axial = Ux, then apply Integrate Variables. The signed result is Q = integral(U_axial) with the +X convention. For a general section compute integral(U · n) using a consistently oriented normal.
5. Compare Q from at least two sections. For incompressible steady flow, they should agree within a justified tolerance. With varying density, compare the mass flow rate m_dot = integral(rho U · n) instead.

Important. Integrating |U| is not the normal flow rate unless the velocity happens to be normal everywhere and points in the same direction. Integrating pressure on a wall patch is not the same quantity as the area-mean pressure on a fluid section.

Background — orientation and signs. If boundary patch normals point outward from the fluid volume, inlet flow has a negative signed rate and outlet flow a positive signed rate. Check conservation through the signed sum, not by arbitrarily changing signs to make two numbers look alike.

6. Exercise 1 — Laminar channel and Poiseuille profile

Goal. Extract U_x(y) from a fully developed region, compare it with the analytical profile and report a reproducible error measure.

Required case. A straight channel with incompressible laminar flow, no-slip walls and constant section. This guide does not ship a ready-to-use OpenFOAM case. Use a copy of a validated introductory case. The theoretical formula only applies to steady, fully developed planar flow without additional acceleration effects.

Consistent illustrative parameters: full channel height H = 0.002 m, measurement length L = 0.100 m, density rho = 1000 kg/m³, dynamic viscosity mu = 0.001 Pa·s, bulk velocity U_mean = 0.100 m/s; physical width for volumetric flow, if relevant: W = 0.010 m. These give Re_H = rho·U_mean·H/mu = 200 and the ideal planar profile

[ U_x(y)=\frac32 U_{mean}\left[1-\left(\frac{2y}{H}\right)^2\right],\quad -H/2\le y\le H/2. ]

The analytical maximum is U_max = 0.150 m/s, while the predicted fully developed pressure drop is DeltaP = 12 mu L U_mean/H² = 30 Pa (Delta p = 0.030 m²/s² if stored as kinematic pressure). The physical flow rate is Q = U_mean H W = 2.0 × 10⁻⁶ m³/s. These are analytical targets, not CFD measurements.

Workflow. Open the converged final step. Apply Plot Over Line along Y in a section well downstream of inlet effects, with endpoints inside the fluid. Export position Y and U_x. In a spreadsheet construct columns for y, U_CFD, U_theory, difference and squared difference. Only compare valid samples at matching physical coordinates and with consistent normalization.

Error, for N paired samples on the same comparison grid:

[ RMSE=\sqrt{\frac1N\sum_{i=1}^{N}(U_{CFD,i}-U_{theory,i})^2},\quad RMSE_{rel}=100\,RMSE/U_{mean}. ]

The relative error is explicitly normalized by U_mean, ensuring a reproducible definition for later mesh comparisons. examples/poiseuille_reference.csv includes an analytic sampled profile for checking the spreadsheet workflow before CFD data are available.

Final checks. Check no-slip at walls, approximately 1.5·U_mean at the centreline, symmetry, negligible profile change between two subsequent sections, and agreement between the flow rate integrated by ParaView and the section-mean estimate. Do not treat the 30 Pa analytical target as an acceptance criterion for an entrance region that is not fully developed.

# rmse_poiseuille.py  -  python rmse_poiseuille.py profilo_x080.csv
import csv, math, sys

H, Umean = 0.002, 0.100                    # case data
yc = 0.0                                   # y coordinate of the channel axis
rows = list(csv.DictReader(open(sys.argv[1], newline='')))
pts = []
for r in rows:
    if r.get('vtkValidPointMask', '1') in ('0', '0.0'):
        continue                           # point outside the fluid
    y = float(r['Points:1']) - yc
    u = float(r['U:0'])                    # x velocity component
    if abs(y) <= H / 2:
        pts.append((y, u))
err2 = [(u - 1.5 * Umean * (1 - (2 * y / H) ** 2)) ** 2 for y, u in pts]
rmse = math.sqrt(sum(err2) / len(err2))
umax = max(u for _, u in pts)
print(f'N = {len(pts)}  RMSE = {rmse:.4g} m/s  RMSE_rel = {100 * rmse / Umean:.3g} %')
print(f'U_max CFD = {umax:.4g} m/s  (theory {1.5 * Umean:.4g})')

7. Exercise 2 — Pressure drop through a flow component

Goal. Obtain a reproducible DeltaP measurement and compare multiple flow rates or geometries.

Setup. Place two well-defined planes upstream and downstream, far enough from artificially imposed boundaries to avoid misleading values. Record plane coordinates and areas. Avoid planes crossing solids, no-data regions, and numerically perturbed inflow regions. Whenever possible keep the same measurement definitions in comparisons between geometry variants.

1. Create Slice_in and Slice_out with documented normals and coordinates.
2. On each, integrate pressure, measure area and compute the area-weighted mean pressure.
3. Verify signed flow rate using integral(U · n) (or axial component for a properly aligned plane).
4. Convert the difference to Pa only when the units require it.
5. Save Q, DeltaP, rho, mu, x_A, x_B, time, mesh and case identifier in a table.
6. Repeat for other flow rates without silently changing measurement-plane definitions. Plot DeltaP(Q) and indicate departures from a linear relationship.

Illustrative numbers only, not OpenFOAM output: p_mean,A = 0.120 m²/s², p_mean,B = 0.085 m²/s², rho = 998 kg/m³ give DeltaP = 998·(0.120−0.085) = 34.93 Pa. A physical comparison can be invalid even between two numerically converged solvers if the sampling planes do not represent the same measurement.

Background — static pressure and head loss. When inlet and outlet sections have different area or kinetic-energy flux, a static-pressure difference is not necessarily equal to the irreversible energy loss. State which quantity is being reported: static pressure difference, total pressure difference or an appropriately defined loss coefficient.

p_tot = p + 0.5*mag(U)^2

8. Exercise 3 — Wakes and recirculation regions

Suggested case. The official OpenFOAM Foundation 14 tutorial incompressibleFluid/pitzDailySteady, featuring a backward-facing step. Copy it to a personal case directory and run it according to the v14 User Guide; do not modify the installed tutorial. This is a quasi-two-dimensional numerical configuration, not a universally valid model of 3D separation.

Part A — visual exploration. Display U on an internal slice of the final solution. Apply Stream Tracer, seed inside the fluid near the upstream section and select vector field U. Inspect maximum streamline length and integration direction. Streamlines follow the instantaneous velocity field and are not necessarily particle trajectories in unsteady flows.

Part B — quantitative region selection. For average flow directed along +X, use Calculator to create U_axial, then Threshold to retain cells where U_axial < 0. Make sure the data association matches the intended source field. For an extruded nominally 2D case, volume integration of the selected U_x < 0 region includes the numerical thickness; to measure 2D area, use an appropriate planar slice. Clearly state the measurement’s dimensions and selection rule.

Part C — physical interpretation. Extract U_x(y) profiles at several downstream positions and inspect negative velocity and the shrinking separated region. Reattachment length is not automatically the coordinate where a coloured streamline ends; it needs a declared operational definition, such as the position where sampled wall shear stress crosses zero with appropriate sign. If results are sensitive to mesh refinement, report that dependence rather than presenting a single precise-looking number. Numerical validation is addressed in Guide 4.

foamPostProcess -solver incompressibleFluid -func wallShearStress -latestTime

9. Comparing cases, exporting and preserving work

9.1 Meaningful comparisons

Use a measurement table (template included) with one row per case: mesh, boundary conditions, density, viscosity, flow rate, pressure drop, measurement locations and time. Overlay profiles only when coordinates and units agree. When comparing datasets from different meshes, export CSVs and interpolate onto a shared sampling grid with the interpolation procedure stated. Do not subtract rows from two nonaligned files.

9.2 Windows-friendly output

• File → Save Data…: select the correct pipeline output before saving CSV. In a client/server session inspect where the destination dialog writes the result; some data exports are performed on the server and can then be retrieved with FileZilla.
• File → Save Screenshot…: specify resolution, labels and consistent colour bars; scientific figures should identify field, units and colour range.
• File → Save State… writes a .pvsm pipeline description. File → Load State… restores the pipeline but does not embed CFD datasets; ParaView may request new paths. A state tied to a remote server can need reconnection and dataset path remapping.
• Preserve CSV and PVSM outputs with a measurement record. PNG pictures alone are not sufficient for reproducing numerical values.

Suggested organization on Windows:

CFD_analysis/
  01_case_and_conditions.txt
  02_profiles_csv/
  03_sections_and_integrals/
  04_figures_png/
  05_paraview_state/
  06_report/

Excel or LibreOffice Calc can analyse the CSVs; Notepad++ can inspect headers and raw text; FileZilla retrieves outputs from Linux. No IDE is required. There is usually no reason to transfer full volumetric fields just to plot a velocity profile.

10. Frequent problems and practical checks

11. Reproducible measurement checklist

Before publishing or sharing a result, record the following (CSV template supplied):

1. Case ID/version, OpenFOAM and ParaView versions, date and original case path.
2. Field dimensions, final units, and whether p is physical or kinematic pressure.
3. Simulation time/iteration, mesh and relevant boundary conditions.
4. Sampling line or plane positions, normals, areas or thicknesses, and selected blocks.
5. Filter names and parameters (Plot Over Line, Calculator, Integrate Variables, etc.).
6. Measurements and an independent check (at least a flow balance or applicable analytical expectation).
7. Deliverable files (CSV, labelled PNG chart, PVSM state) and stated interpretation limits.

Learning outcome. Readers should be able to extract a velocity profile and RMSE, compute volumetric flow rate and pressure drop, distinguish flow recirculation from visualization artifacts, and deliver results another user can independently reconstruct.

case_id,time_or_iteration,mesh_cells,field,field_dimension,rho_kg_m3,mu_Pa_s,section_A_x_m,section_B_x_m,area_A_m2,area_B_m2,p_mean_A_field_units,p_mean_B_field_units,deltaP_Pa,Q_A_m3_s,Q_B_m3_s,method_notes,csv_file,pvsm_file

Official references and figure notes

• ParaView 5.13.2 — Filtering Data — Slice, Plot Over Line, Calculator, Gradient, Integrate Variables.
• ParaView 5.13.2 — Remote and parallel visualization — client/server connections and SSH tunnels.
• ParaView 5.13.2 — Saving Results — exports and PVSM states.
• ParaView 5.13.2 — Targeted: Computational Fluid Dynamics — CFD streamline filters.
• OpenFOAM Foundation v14 — ParaView — OpenFOAM readers and post-processing.
• OpenFOAM Foundation v14 — Backward-facing step — pitzDailySteady tutorial.
• OpenFOAM Foundation v14 — Field format and dimensions — field dimensions and unit conventions.

Figure provenance: all embedded figures were newly drawn for this guide; they are either operational schematics or analytic reference graphs. The GUI map is a reconstruction, not an actual ParaView screenshot. Illustrative plots are not CFD results unless explicitly stated otherwise. Filter descriptions were checked against the official documentation.

Related guides: OpenFOAM on a Linux server, working from Windows, monitoring, troubleshooting and convergence assessment and the Learning OpenFOAM 14 path.