Defining a time step for a flow analysis

In any analysis, it is important to consider what time step to use for the model. This article gives guidelines for selecting a time step type for your analysis, and specifying its value. For a steady state flow analysis, you must decide whether to use a physical time step or a local time step. For a transient flow analysis, a physical time step is required.

Choosing a Local Time Step

When you choose the Local setting for Steady State – Relaxation Time Step, the flow solver computes a local reference time step based on local velocity and element length scale at each node (control volume) in the domain, and scales all the diagonal terms of the coefficient matrix by:

(1+1/α)

where α is the Time Step Factor.

This method is particularly useful for models that include varying time scales. For example, when there are small time scales near an inlet fan and long time scales at a stagnation point, a sufficiently small physical time step value is required to converge the solution in the inlet fan region, while it is excessively small in the stagnation region. Using the local time step method, the solver resolves this automatically by using small time steps near the inlet and larger time steps at the stagnation points. A converged solution is obtained with a minimum computational cost.

Decreasing the value of the Time Step Factor provides more relaxation to the convergence process but usually increases the computational cost. A default value of 20 is suggested for the Time Step Factor but when a model exhibits oscillations in the convergence, a value as low as 2 can help the convergence rates.

Choosing a Physical Time Step

It is generally recommended that you calculate a reasonable physical time step for your model and use the Physical option for the Steady State – Relaxation Time Step. Always use a physical time step for simulating natural convection (fluid buoyancy). It is important to define a time step value that is sufficiently small in order to resolve the non-linearities. That is, the solution should be linear over the time step interval. If you choose a time step value that is too large the solution may not converge; values which are too small ensure convergence but at severe computational cost. The best time step value is typically some fraction of a physical time scale for the model. You can specify a physical time step as a constant expression or as a field where the independent domain is iteration. The following examples show you how to calculate a reasonable physical time step value.

Forced Convection

A value of ½ the model length scale divided by the model velocity scale generally produces good results without severe computational cost. Hence, the time step δt can be evaluated as:

δt = ½ L / V

where L is the mean flow distance from the inlet to the outlet and V is the average velocity. If the solution does not converge using this value then divide the time step by 2 and try solving again.

Natural Convection

Always use a physical time step for simulating natural convection (fluid buoyancy). Calculate the time step as follows:

Time step,

Where:

Grashoff Number,

g = Gravitational acceleration

β = Coefficient of thermal expansion. (for air, β = 3.4x10 -3)

ΔT = Change in air temperature from outlet to inlet. (Typical is 10°;C to 25°;C.)

h = Chimney height as shown above

ν = Kinematic viscosity, for air at 27°;C ν = 25.90 × 10 6m 2/s

For example,

• h = 0.3m

• β = 3.4x10 -3

• g = 9.81m/s 2

• ΔT = 25°;C,

• Gr = 0.09

• δt = 0.6s

Use time step of 0.3s to be safe.

How do I

How to choose values for Maximum Normalized Velocity Change and Maximum Normalized Pressure Change

Learn more

Adjusting solver parameters

Setting thermal solver parameters

Setting flow solver parameters

Setting coupled solver parameters

Understanding radiation parameters

Setting relaxation factors for the flow solver

Understanding the freeze flow field options

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal boundary conditions

Defining a time step for a flow analysis, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });