Boundary-Layer Flow Between Parallel Plates (COMSOL) This example is essentially a reproduction, on our part, of one of the sample problems that was part of the COMSOL Model Library of several years ago, and we are indebted to COMSOL for the idea. A fluid of density 1,000 kg/m^3 and viscosity 0.01

Question

Boundary-Layer Flow

Between Parallel Plates (COMSOL)

This example is essentially a reproduction, on our part, of one of the sample problems that was part of the COMSOL Model Library of several years ago, and we are indebted to COMSOL for the idea.

A fluid of density [latex]1,000 \mathrm{~kg} / \mathrm{m}^{3}[/latex] and viscosity [latex]0.01 \mathrm{~kg} / \mathrm{m}[/latex] s flows freely in the [latex]y[/latex] direction with an initially uniform velocity [latex]v_{0}=0.02 \mathrm{~m} / \mathrm{s}[/latex]. After a distance of [latex]y=0.01[/latex], it encounters flat plates of length [latex]0.04[/latex] located at [latex]x=\pm 0.01 \mathrm{~m}[/latex] (all units are SI). The exit pressure from the plates is [latex]p=0[/latex]. The corresponding boundary conditions are shown in Fig. E8.3.1.

We wish to solve for the velocities, make the following plots, and comment on them:

The streamlines.
Arrows showing the velocity vectors.
A two-dimensional contour plot of the velocity.

Additionally, for [latex]y=0.015[/latex], we want to make and comment on the following cross-sectional plots:

The [latex]y[/latex] velocity.
The [latex]x[/latex] velocity.
The vorticity.

Finally, we comment on the relative values of the pressure and [latex]y[/latex] velocity [latex]v_{y}[/latex] at [latex]x=0, y=0.01[/latex], marked as [latex]\mathrm{P}[/latex] in Fig. E8.3.1, and at the exit [latex](x=0, y=0.05)[/latex].

Accepted Answer

See Chapter 14 for more details about COMSOL Multiphysics. All mouse-clicks are left-clicks (the same as Select) unless specifically denoted as right-click (R).

Select the Physics

Open COMSOL and L-click Model Wizard, 2D, Fluid Flow (the little rotating triangle is called a "glyph"), Single-Phase Flow, Laminar Flow. L-click Add. Note the COMSOL names [latex]u, v, w[/latex] for the three velocity components, and [latex]p[/latex] for pressure.
L-click Study, Stationary, Done.
Pull down the Windows menu to Desktop Layout and then Regular Screen Layout - it gives more graphics window space, at the expense of somewhat reducing the Model Builder and Settings windows, in which you may have to scroll down.

Define the Parameters

R-click Global Definitions and select Parameters. In the Settings window (now below the Model Builder window), enter the parameter rho1 in the Name column and [latex]1000\left[\mathrm{~kg} / \mathrm{m}^{3}\right][/latex] in the Expression column. Similarly, define [latex]m u 1=0.01[/latex] [latex][\mathrm{Pa} * \mathrm{~s}], v 0=0.02[\mathrm{~m} / \mathrm{s}], x 0=-0.01[\mathrm{~m}], y 0=0.015[\mathrm{~m}], x 1=0.01[\mathrm{~m}][/latex], and [latex]y 1=[/latex] [latex]0.015[\mathrm{~m}] .[/latex] Finally, add ySlip [latex]=0.01[\mathrm{~m}][/latex] and [latex]H=0.05[\mathrm{~m}][/latex], which are the length of the slip boundary and height of the entire domain, respectively.

Establish the Geometry

R-click Geometry and select Rectangle. Note the default is based on the lower left corner being at [latex](0,0)[/latex]. Enter the values for Width and Height as [latex]x 1-x 0[/latex] and [latex]H .[/latex] Modify the values of the base corner to be [latex](x 0,0) .[/latex] L-click Build Selected.
Add an embedded rectangle to form the region for the full slip condition. R-click Geometry and select Rectangle. Enter the values for Width and Height as [latex]x 1-x 0[/latex] and [latex]y[/latex] Slip. Set the base corner at [latex](x 0,0)[/latex]. L-click Build Selected.
R-click Geometry and select Boolean and Partitions, Union. Add the two geometries to the union by L-clicking each in the Graphics window. Ensure that the Keep interior boundaries option is selected in Settings. L-click Build Selected.
Define the Fluid Properties
R-click the Materials node within Component 1 and select Blank Material. Enter the parameters [latex]r h o 1[/latex] and [latex]m u 1[/latex] as values for Density and Dynamic viscosity.
Define the Boundary Conditions
L-click the Laminar Flow glyph, select Wall 1, and note the six default No-slip boundary conditions.
R-click the Laminar Flow node and select Inlet to define an inlet boundary condition. L-click the bottom boundary [latex](\# 2)[/latex] to select it as the inlet. Within the Settings window note that the default form for the Boundary Condition is Velocity. Change the value of the Normal inflow velocity to [latex]v 0[/latex].
R-click the Laminar Flow node and select Outlet to define an outlet boundary condition. L-click the top boundary [latex](\# 5)[/latex] to select it as the outlet. Additionally, deselect the Suppress backflow option and select Normal flow option. Note that the exit pressure is zero.
Add the slip boundary conditions by overriding a portion of the default Wall boundary conditions. R-click the Laminar Flow node and L-click Wall. Within the Settings window change the Boundary Condition from No Slip to Slip. Add the two slip walls to the Boundary selection by L-clicking the two lower vertical segments (#1 and #6).

Create the Mesh and Solve the Problem

L-click the Mesh node and change the Element Size in the Settings window to Fine. L-click Build All to construct the mesh, which contains approximately 4,000 elements.
R-click the Study node and select Compute, which takes about 5 seconds and gives a plot of the magnitude of the velocity, Fig. E8.3.2(c).

15 Save the model file regularly!

Display the Results

Create a data set at the line segment representing section A-A. R-click the Data Sets node within the Results tree and select Cut Line 2D. In the Settings window enter the values [latex](x 0, y 0)[/latex] and [latex](x 1, y 1)[/latex] for Points 1 and 2 . L-click Plot near the top of the Settings window to display the cut line.
Generate the streamline plot. R-click the Results node and select 2D Plot Group. R-click this newly created Plot Group 3 and select Streamline. Within the Settings window, note the default positioning option is set to On selected boundaries. Select the inlet [latex](\# 2)[/latex] as the boundary for positioning and set the Number to 40. L-click Plot, giving Fig. E8.3.2(a).
Generate the velocity-vector plot. R-click the Results node and select 2D Plot Group. R-click this newly created Plot Group 4 and select Arrow Surface. In the Settings window, modify the number of points for the [latex]x[/latex] grid points to be 20 . L-Click Plot at the top of the Settings window, giving Fig. E8.3.2(b). Change the color to black and increase the arrow length for better printing.
Create the plot for the upward velocity across the section A-A. R-click Results and L-click 1D Plot Group. In the Settings window, L-click the dropdown dialog and change the data set to Cut Line 2D 1 created above. R-click the 1D Plot Group 5 and select Line Graph. Within the Settings window enter the variable for the [latex]y[/latex]-component of velocity, [latex]v[/latex], in the Expression field. Additionally, change the [latex]x[/latex]-Axis Data Parameter to be Expression using the dropdown dialog and enter [latex]x[/latex]. L-Click Plot at the top of the Settings window, giving Fig. E8.3.3.
Create the plot for the transverse velocity along the section A-A. R-click Results and L-click 1D Plot Group. In the Settings window, L-click the dropdown dialog and change the data set to Cut Line 2D 1 created above. R-click the 1D Plot Group 6 and select Line Graph. Within the Settings window enter the variable for the [latex]x[/latex]-component of velocity, [latex]u[/latex], in the Expression field. Additionally, change the [latex]x[/latex]-Axis Data Parameter to be Expression using the dropdown dialog and enter the expression [latex]x[/latex]. L-Click Plot at the top of the Settings window, giving Fig. E8.3.4.
Create the plot for vorticity across the section A-A. R-click Results and L-click 1D Plot Group. In the Settings window, L-click the dropdown dialog and change the data set to Cut Line 2D 1 created above. R-click the 1D Plot Group 7 and select Line Graph. Use the Expression Builder (the little glyph at the right-hand end of the [latex]y[/latex]-Axis Data line, also shown in Fig. E11.3.5) to plot the vorticity. L-click Component 1, Laminar Flow, Velocity and pressure, Vorticity field, spf.vorticityz-Vorticity field, [latex]z[/latex]-component. Additionally, change the [latex]x[/latex]-Axis Data Parameter from Arc Length to Expression using the dropdown dialog and enter the expression [latex]x[/latex]. L-click Plot.
Note the discontinuous nature of the vorticity plot, since it is based on gradient data. Smooth the data by accessing the Quality section in the Settings window. Change the Recovery option to Within domains. Plot, giving Fig. E8.3.5.

Discussion of Results

Overall plots. The overall picture of the flow is displayed in Fig. E8.3.2. After the initial small "free-flow" entrance region, the formation of boundary layers on the two plates is very evident, either by examining the movement of the streamlines away from the plates or by noting the reduction in velocity adjacent to the plates. From continuity, this velocity reduction also causes an acceleration in the middle of the stream.

The results for the cross section A-A are shown in Figs. E8.3.3-E8.3.5, for which we make the following comments:

The velocity [latex]v_{y}[/latex] in the primary flow direction is still essentially flat in the central region, falling to zero as the wall is reached.

(a) At values of [latex]x[/latex] that are clearly in the boundary layer, such as [latex]x=-0.008[/latex] and [latex]x=0.008[/latex] in Fig. E8.3.3, [latex]v_{y}[/latex] would continue to decrease in the [latex]y[/latex] direction, so that [latex]\partial v_{y} / \partial y[/latex] is negative at these locations.

(b) In the central core [latex]v_{y}[/latex] continues to accelerate as seen in Fig. E8.3.2(c), so that the reverse occurs and [latex]\partial v_{y} / \partial y[/latex] is positive.

Following on Item 1 (a), the continuity equation, [latex]\partial v_{x} / \partial x+\partial v_{y} / \partial y=0[/latex], mandates that [latex]\partial v_{x} / \partial x[/latex] must be positive in the boundary layer, and this is evidenced in Fig. E8.3.4 at, for example, [latex]x=-0.008[/latex] and [latex]x=0.008[/latex]. Conversely, from Item [latex]1(\mathrm{~b}), \partial v_{x} / \partial x[/latex] must be negative in the central core, and this is also seen.
The vorticity is [latex]\zeta=\partial v_{y} / \partial x-\partial v_{x} / \partial y \doteq \partial v_{y} / \partial x[/latex] (because [latex]v_{y} \gg v_{x}[/latex] ), leading to a positive vorticity (counterclockwise rotation) near the left-hand plate and a negative vorticity (clockwise rotation) near the right-hand plate. In the central region the vorticity is essentially zero because [latex]v_{y}[/latex] is virtually constant there.

Values at point [latex]P[/latex]. Finally, we investigate the pressure [latex]p[/latex] and velocity [latex]v_{y}[/latex] at the entrance point [latex]\mathrm{P}[/latex] and exit. By constructing a surface plot for [latex]p[/latex] (we already have one for the magnitude of the velocity, which is essentially [latex]v[/latex] ), and clicking on [latex]\mathrm{P}(x=0, y=0.01)[/latex] and the exit [latex](x=0, y=0.05)[/latex], we find [latex]p=0.3340 \mathrm{~Pa}[/latex] and [latex]v_{y}=0.02215 \mathrm{~m} / \mathrm{s}[/latex] at point P. Similarly, the exit centerline values are [latex]p=0[/latex] (given) and [latex]v_{y}=0.02984[/latex]. As expected at the centerline, there is an acceleration from P to the exit and a corresponding reduction in pressure, and we leave it to the reader to check numerically to what extent these values conform to Bernoulli's equation.

Question 8.3: Boundary-Layer Flow Between Parallel Plates (COMSOL) This ex...

This Question has been Answered.

Already have an account?

Login

Related Answered Questions