Volume Output

Volume Output#

Volume Output in Flow360 allows you to visualize flow field variables throughout the entire computational domain. This is essential for understanding 3D flow structures, vortex development, shockwaves, and other volumetric flow features.

Available Options#

Option

Description

Applicable

Output fields

Flow variables to include in the output

always

Output format

Format for saving volume data

always

Save interval

When to save outputs

always

Frequency

How often to save outputs

when Save interval is Custom

Frequency offset

Time step at which to start the output animation

when Save interval is Custom

Global Time Stepping in Child Cases#

When working with child cases (cases forked from a parent simulation), it’s important to understand that the Frequency and Frequency offset parameters refer to the global time step, which is transferred from the parent case.

Example: If the parent case finished at time_step=174, the child case will start from time_step=175. If Frequency=100 is set in the child case, the output will be saved at global time steps 200 (25 time steps into the child simulation), 300 (125 time steps into the child simulation), etc. Frequency offset also refers to the global time step, meaning that if in the previously mentioned child case, Frequency offset=50 was set (with Frequency=100), the output would be saved at global time steps 250 (75 time steps into the child simulation), 350 (175 time steps into the child simulation), etc.

Detailed Descriptions#

Output fields#

Select the flow variables to include in the volume output.

  • Default: None selected

  • Example: Mach, pressure, qcriterion

Notes:

  • See detailed field descriptions below.

  • Only select fields you need to analyze to keep file sizes manageable.

Output format#

The file format used to save the volume output data.

  • Default: paraview

  • Options:

    • paraview

    • tecplot

    • both

Notes:

  • Choose the format that best suits your post-processing workflow.

  • Select paraview for .vtu format, tecplot for .plt format, or both to save in both formats.

Save interval#

Choose the points in the simulation where the results are saved.

  • Default: Save at end

  • Options:

    • Save at end

    • Custom (only available when Time stepping is Unsteady)

Notes:

  • Choose Save at end to save only the final results of the simulation.

  • Choose Custom to save the results in given intervals.

Frequency#

How often to save outputs, in number of physical time steps.

  • Default: -1 (only at the end of simulation)

  • Example: 100 — saves output every 100 physical time steps.

    • Standalone case: If you start a simulation from time_step=0 with frequency=100, outputs are saved at time steps 100, 200, 300, etc.

    • Parent-child case: If the parent finished at time_step=174, the child starts from time_step=175. With frequency=100 in the child, outputs are saved at global time steps 200 (25 steps into child), 300 (125 steps into child), 400 (225 steps into child), etc.

Notes:

  • Higher frequencies provide better temporal resolution but increase storage requirements.

  • Important for child cases - this parameter refers to the global time step (see Global Time Stepping).

  • This setting is only applicable for unsteady cases.

Frequency offset#

The time step at which to start the output animation.

  • Default: 0 (beginning of simulation)

  • Example: 1000 — with frequency=100, outputs are saved at time steps 1000, 1100, 1200, etc.

    • Standalone case: If you start a simulation from time_step=0 with frequency=100 and frequency_offset=1000, outputs are saved at time steps 1000, 1100, 1200, etc.

    • Parent-child case: If the parent finished at time_step=174, the child starts from time_step=175. With frequency=100 and frequency_offset=200 in the child, outputs are saved at global time steps 200 (25 steps into child), 300 (125 steps into child), 400 (225 steps into child), etc.

Notes:

  • Useful when you want to skip initial transient flow development.

  • Important for child cases - this parameter refers to the global time step (see Global Time Stepping).

  • This setting is only applicable for unsteady cases.

  • For time-averaged volume output settings, see the Time-Averaged Volume Output documentation.

Available Output Fields#

Variables from Available Output Fields and the following specific variables

Volume-Specific Variables (non-dimensional)#

  • betMetrics - BET Metrics

  • betMetricsPerDisk - BET Metrics per Disk

  • linearResidualNavierStokes - Linear residual of Navier-Stokes solver

  • linearResidualTurbulence - Linear residual of turbulence solver

  • linearResidualTransition - Linear residual of transition solver

  • SpalartAllmaras_hybridModel - Hybrid RANS-LES output for Spalart-Allmaras solver (supports both DDES and ZDES)

  • kOmegaSST_hybridModel - Hybrid RANS-LES output for kOmegaSST solver (supports both DDES and ZDES)

  • localCFL - Local CFL number

Hybrid RANS-LES Output Variables#

The SpalartAllmaras_hybridModel and kOmegaSST_hybridModel output fields provide diagnostic variables for hybrid RANS-LES simulations. The specific variables included depend on whether you’re using DDES (Delayed Detached Eddy Simulation) or ZDES (Zonal Detached Eddy Simulation) as the shielding function.

DDES Variables (when shielding_function="DDES")#

When using DDES, the hybrid model output includes five key variables:

  1. f_d – The shielding function that delineates the RANS and LES regions. When f_d = 0, the RANS model is fully applied; when f_d = 1, the LES model is used. Intermediate values represent a smooth transition between the two regimes.

  2. r_d – A modified ratio of the modeled length scale to the wall distance, from which f_d is derived.

  3. DDES_lengthRANS – The wall distance from the computational cell to the nearest solid boundary.

  4. DDES_lengthScale – The characteristic DES length scale: \(\tilde{d} \equiv d - f_d \max(0, d - C_{DES}*\Delta)\)

  5. DDES_lengthLES – The characteristic LES length scale: \(C_{DES}*\Delta\)

Among these variables, f_d is the most significant, as it enables users to identify and visualize the regions dominated by RANS and DES behavior within the computational domain.

ZDES Variables (when shielding_function="ZDES")#

When using ZDES, the hybrid model output includes four key variables:

  1. ZDES_fp – The enhanced shielding function that determines whether RANS or LES is used. When ZDES_fp = 0, RANS is active; when ZDES_fp = 1, LES is active. This function is computed from ZDES_fd, ZDES_fR, and ZDES_fp2.

  2. ZDES_fd – Original DDES shielding function used in computing ZDES_fp.

  3. ZDES_fR – is included to disable or inhibit this second shielding function in regions where vorticity magnitude is increasing away from walls - this is designed to disable the secondary shielding function where a shear layer is detected above a wall. Component used in computing ZDES_fp.

  4. ZDES_fp2 – Causes the model to revert to RANS mode in the outer portion of boundary layers, used in computing ZDES_fp.

💡 Tips

Q-Criterion

The qcriterion field is extremely valuable for visualizing vortices in the flow field. To effectively use this field:

  • Create isosurfaces of Q-criterion to identify vortical structures

  • The default isosurface value is calculated as RefMach² / (all walls' bounding box length)²

  • For aircraft simulations: a good starting value is approximately Mach² / WingSpan²

  • For rotor flows: try TipMach² / RotorDiameter²

  • Smaller values show more vortical structures but may clutter visualization

  • Larger values show only the strongest vortices

Note: Q-criterion can also be directly exported as an isosurface with a specific iso value using the Isosurface Output feature, which provides better control over the visualization.

BET Visualization

When using Blade Element Theory (BET) models for propellers or rotors, the betMetrics field provides valuable data for analyzing:

  • Blade loading distributions

  • Induced velocities

  • Local angle of attack

  • Flow conditions at each blade element

These metrics are essential for understanding propeller and rotor performance characteristics.

Performance Considerations

Volume outputs can generate very large files, especially for fine meshes. Consider the following to manage file sizes:

  1. Limit the frequency of volume outputs

  2. Be selective about which fields to include

  3. Use time-averaged volume outputs for statistical analysis of unsteady flows

  4. Consider using slices or isosurfaces instead for targeted analysis

❓ Frequently Asked Questions

  • How large are volume output files typically?

    File sizes depend on mesh size, selected output fields, and output format. For a mesh with several million cells:

    • Each field adds approximately 4-8 bytes per cell

    • A full domain output with 5 fields might be 1-5GB per time step for 100M mesh

    • Consider using time-averaged outputs or selective fields to reduce storage requirements

  • What’s the difference between ParaView and Tecplot formats?

    • ParaView format (.vtu): Open-source visualization tool with excellent performance for large datasets. Provides a wide range of visualization and analysis capabilities.

    • Tecplot format (.szplt): Commercial visualization software with specialized aerodynamic analysis tools. May provide more streamlined workflows for certain aerospace applications.

    • Choose “both” if you’re unsure which tool you’ll need or if different team members use different tools.

  • How do I choose the right frequency for volume outputs?

    Consider these factors:

    • For steady-state simulations: Set to -1 (final solution only) or use a high number (e.g., every 1000 steps)

    • For unsteady simulations: Ensure you capture the relevant time scales (e.g., for vortex shedding, ensure at least 20-30 snapshots per shedding cycle)

    • Storage constraints: Higher frequencies generate more data

    • A good starting point for unsteady flows is 50-100 time steps between outputs

  • Why are my volume outputs missing data in certain regions?

    Missing data in volume outputs typically occurs for these reasons:

    • For parallel simulations, check that all partitions are being correctly combined

    • Ensure the simulation has valid data in those regions (check convergence)

    • For moving mesh simulations, ensure mesh movement is properly configured

  • How can I visualize specific flow features effectively?

    For different flow features:

    • Vortices: Use Q-criterion (isosurfaces) with values around Mach²/Length²

    • Shock waves: Density gradient or Mach number gradients work well

    • Boundary layers: Use slices with velocity profiles near walls

    • Wake structures: Combine Q-criterion with velocity magnitude contours

  • Can I add custom output fields to volume output?

    Currently, Flow360 supports only the predefined output fields listed in this documentation. If you need additional derived quantities:

    • Export the primitive variables and calculate derived quantities in your visualization tool

    • Use Python post-processing with the Flow360 API to create custom fields

    • Contact support if you need a specific field that might benefit other users

🐍 Python Example Usage

 
# Example of configuring volume output using Flow360 Python API
import flow360 as fl

# Define volume output settings
volume_output = fl.VolumeOutput(
    name="Main Flow Volume",
    output_format="paraview",
    output_fields=["Mach", "pressure", "qcriterion", "velocity"],
    frequency=100,  # Save every 100 time steps
    frequency_offset=1000,  # Start at time step 1000
)

# Add volume output to simulation parameters
simulation_params = fl.SimulationParams(
    # ... other simulation parameters ...
    outputs=[volume_output]
)
Contents