You are viewing the documentation for an older COMSOL version. The latest version is available here.
PDF
Stationary Incompressible Flow over a Backstep
Introduction
This tutorial model solves the incompressible Navier-Stokes equations in a backstep geometry. A characteristic feature of fluid flow in geometries of this kind is the recirculation region that forms where the flow exits the narrow inlet region. The model clearly demonstrates the formation of such a region, which is best displayed by visualizing the flow streamlines.
Model Definition
Model Geometry
The model consists of a pipe connected to a block-shaped tank; see Figure 1. Due to symmetry, it is sufficient to model one eighth of the full geometry. The pipe has an inlet at one end, and the tank has an outlet at the opposite end. All other boundaries are solid walls.
Figure 1: Model geometry.
Domain Equation and Boundary Conditions
The flow in this model is laminar, so a Laminar Flow interface will be used. The inlet flow is fully developed, which will be specified by the corresponding inlet boundary condition. This boundary condition computes the flow profile for fully developed flow in a channel of arbitrary cross section. The boundary condition at the outlet sets a constant relative pressure. Furthermore, the vertical and inclined boundaries along the length of the geometry are symmetry boundaries. All other boundaries are solid walls described by a no slip boundary condition.
Results
Figure 2 shows a combined surface and arrow plot of the flow velocity. This plot does not reveal the recirculation region in the tank immediately beyond the inlet pipe’s end. For this purpose, a streamline plot is more useful, as demonstrated in Figure 3.
Figure 2: The velocity field in the backstep geometry.
Figure 3: The recirculation region visualized using a velocity streamline plot.
Application Library path: CFD_Module/Single-Phase_Tutorials/backstep
Modeling Instructions
From the File menu, choose New.
New
In the New window, click Model Wizard.
Model Wizard
1
In the Model Wizard window, click 3D.
2
In the Select Physics tree, select Fluid Flow>Single-Phase Flow>Laminar Flow (spf).
3
Click Add.
4
Click Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click Done.
Global Definitions
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
v0
1[cm/s]
0.01 m/s
Inlet velocity
Geometry 1
You can build the backstep geometry from geometric primitives. Here, instead, use a file containing the sequence of geometry features that has been provided for convenience.
1
In the Geometry toolbar, click Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file backstep_geom_sequence.mph.
3
In the Settings window for Cylinder, click Build All Objects.
4
Click the Zoom Extents button in the Graphics toolbar.
The model geometry is now complete (Figure 1).
Add Material
1
In the Home toolbar, click Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-In>Water, liquid.
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click Add Material to close the Add Material window.
Laminar Flow (spf)
Inlet 1
1
In the Physics toolbar, click Boundaries and choose Inlet.
2
Select Boundary 1 only.
3
In the Settings window for Inlet, locate the Boundary Condition section.
4
From the list, choose Fully developed flow.
5
Locate the Fully Developed Flow section. In the Uav text field, type v0.
Symmetry 1
1
In the Physics toolbar, click Boundaries and choose Symmetry.
2
Select Boundaries 2 and 3 only.
Outlet 1
1
In the Physics toolbar, click Boundaries and choose Outlet.
2
Select Boundary 7 only.
3
In the Settings window for Outlet, locate the Pressure Conditions section.
4
Select the Normal flow check box.
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Coarse.
4
Click Build All.
5
Click the Zoom Extents button in the Graphics toolbar.
Study 1
In the Home toolbar, click Compute.
Results
Slice
In the Model Builder window, expand the Velocity (spf) node.
Velocity (spf)
1
Right-click Slice and choose Delete.
. Click Yes to confirm.
Arrow Surface 1
1
In the Model Builder window, right-click Velocity (spf) and choose Surface.
2
Right-click Velocity (spf) and choose Arrow Surface.
3
In the Settings window for Arrow Surface, locate the Coloring and Style section.
4
From the Arrow length list, choose Logarithmic.
5
From the Color list, choose Yellow.
6
Click the Zoom Extents button in the Graphics toolbar.
7
In the Velocity (spf) toolbar, click Plot.
To see the recirculation effects, create a streamline plot of the velocity field.
Streamline 1
1
In the Home toolbar, click Add Plot Group and choose 3D Plot Group.
2
In the Model Builder window, right-click 3D Plot Group 3 and choose Streamline.
3
Select Boundary 1 only.
4
In the Settings window for Streamline, locate the Coloring and Style section.
5
Find the Line style subsection. From the Type list, choose Tube.
Color Expression 1
Right-click Results>3D Plot Group 3>Streamline 1 and choose Color Expression.