Compressible Flow In A Nozzle

Compressible Flow in a Nozzle Author: Rajesh Bhaskaran E-mail: [email protected] Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Problem Specification

Consider air flowing at high-speed through a convergent-divergent nozzle having a circular cross-sectional area, A, that varies with axial distance from the throat, x, according to the formula A = 0.1 + x2; -0.5 < x < 0.5 where A is in square meters and x is in meters. The stagnation pressure po at the inlet is 101,325 Pa. The stagnation temperature To at the inlet is 300 K. The static pressure p at the exit is 3,738.9 Pa. We will calculate the Mach number, pressure and temperature distribution in the nozzle using FLUENT and compare the solution to quasi-1D nozzle flow results. The Reynolds number for this high-speed flow is large. So we expect viscous effects to be confined to a small region close to the wall. So it is reasonable to model the flow as inviscid. Go to Step 1: Create Geometry in GAMBIT

Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Step 1: Create Geometry in GAMBIT Since the nozzle has a circular cross-section, it's reasonable to assume that the flow is axisymmetric. So the geometry to be created is two-dimensional. Start GAMBIT

Create a new folder called nozzle and select this as the working directory. Add -id nozzle to the startup options. Create Axis Edge

We'll create the bottom edge corresponding to the nozzle axis by creating vertices A and B shown in the problem specification and joining them by a straight line. Operation Toolpad > Geometry Command Button

> Vertex Command Button

>

Create Vertex Create the following two vertices: Vertex 1: (-0.5,0,0) Vertex 2: (0.5,0,0) Operation Toolpad > Geometry Command Button

> Edge Command Button

>

Create Edge Select vertex 1 by holding down the Shift button and clicking on it. Next, select vertex 2. Click Apply in the Create Straight Edge window. Create Wall Edge

We'll next create the bottom edge corresponding to the nozzle wall. This edge is curved. Since A=pi r2 where r(x) is the radius of the cross-section at x and A = 0.1 + x2 for the given nozzle geometry, we get r(x) = [(0.1 + x2)/pi]0.5; -0.5 < x < 0.5 This is the equation of the curved wall. Life would have been easier if GAMBIT allowed for this equation to be entered directly to create the curved edge. Instead, one has to create a file containing the coordinates of a series of points along the curved line and read in the file. The more number of points used along the curved edge, the smoother the resultant edge. The file vert.dat contains the point definitions for the nozzle wall. Take a look at this file. The first line is 21 1 which says that there are 21 points along the edge and we are defining only 1 edge. This is followed by x,r and z coordinates for each point along the edge. The r-value for each x was generated from the above equation for r(x). The z-coordinate is 0 for all points since we have a 2D geometry. Right-click on vert.dat and select Save As... to download the file to your working directory. Main Menu > File > Import > ICEM Input ... Next to File Name:, enter the path to the vert.dat file that you downloaded or browse to it by clicking on the Browse button.

Then, check the Verticesand Edges boxes under Geometry to Create as we want to create the vertices as well as the curved edge.

Click Accept. This should create the curved edge. Here it is in relation to the vertices we created above:

(Click picture for larger image) Create Inlet and Outlet Edges

Create the vertical edge for the inlet: Operation Toolpad > Geometry Command Button

> Edge Command Button

>

Create Edge Shift-click on vertex 1 and then the vertex above it to create the inlet edge. Similarly, create the vertical edge for the outlet.

(Click picture for larger image) Create Face

Form a face out of the area enclosed by the four edges: Operation Toolpad > Geometry Command Button

> Face Command Button

>

Form Face Recall that we have to shift-click on each of the edges enclosing the face and then click Apply to create the face. Save Your Work

Main Menu > File > Save This will create the nozzle.dbs file in your working directory. Check that it has been created so that you will able to resume from here if necessary. Go to Step 2: Mesh Geometry in GAMBIT Copyright 2002. Cornell University

Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Step 2: Mesh Geometry in GAMBIT Now that we have the basic geometry of the nozzle created, we need to mesh it. We would like to create a 50x20 grid for this geometry. Mesh Edges

As in the previous tutorials, we will first start by meshing the edges. Operation Toolpad > Mesh Command Button

> Edge Command Button

> Mesh

Edges Like the Laminar Pipe Flow Tutorial, we are going to use even spacing between each of the mesh points. We won't be using the Grading this time, so deselect the box next to Grading that says Apply. Then, change Interval Count to 20 for the side edges and Interval Count to 50 for the top and bottom edges.

(Click picture for larger image) Mesh Face

Now that we have the edges meshed, we need to mesh the face. Operation Toolpad > Mesh Command Button

> Face Command Button

Faces As before, select the face and click the Apply button.

(Click picture for large image) Save Your Work

> Mesh

Main Menu > File > Save Go to Step 3: Specify Boundary Types in GAMBIT Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Step 3: Specify Boundary Types in GAMBIT Specify Boundary Types

Now that we have the mesh, we would like to specify the boundary conditions here in GAMBIT. Operation Toolpad > Zones Command Button

> Specify Boundary Types Command

Button This will bring up the Specify Boundary Types window on the Operation Panel. We will first specify that the left edge is the inlet. Under Entity:, pick Edges so that GAMBIT knows we want to pick an edge (face is default).

Now select the left edge by Shift-clicking on it. The selected edge should appear in the yellow box next to the Edges box you just worked with as well as the Label/Type list

right under the Edges box. Next to Name:, enter inlet. For Type:, select WALL. Click Apply. You should see the new entry appear under Name/Type box near the top of the window.

Repeat for the outlet, centerline, and wall edges. You should have the following edges in the Name/Type list when finished:

Save and Export

Main Menu > File > Save Main Menu > File > Export > Mesh... Type in nozzle.msh for the File Name:. Select Export 2d Mesh since this is a 2 dimensional mesh. Click Accept. Check nozzle.msh has been created in your working directory. Go to Step 4: Set Up Problem in FLUENT Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Step 4: Set Up Problem in FLUENT Launch FLUENT

Start > Programs > Fluent Inc > FLUENT 6.0 Select 2ddp from the list of options and click Run. Import File

Main Menu > File > Read > Case... Navigate to your working directory and select the nozzle.msh file. Click OK. The following should appear in the FLUENT window:

Check that the displayed information is consistent with our expectations of the nozzle grid. Analyze Grid

Grid > Info > Size How many cells and nodes does the grid have? Display > Grid How many nodes are there in the radial direction? Are the nodes clustered towards the wall? Why? Define Properties

Define > Models > Solver... Under the Solver box, select Coupled. Under Space, choose Axisymmetric.

Click OK. Define > Models > Viscous Select Inviscid under Model.

Click OK. Define > Models > Energy The energy equation needs to be turned on since this is a compressible flow where the

energy equation is coupled to the continuity and momentum equations. Make sure there is a check box next to Energy Equation and click OK.

Define > Materials Select air under Fluid materials. Under Properties, choose Ideal Gas next to Density. You should see the window expand. This means FLUENT uses the ideal gas equation of state to relate density to the static pressure and temperature.

Click Change/Create. Close the window. Define > Operating Conditions We'll work in terms of absolute rather than gauge pressures in this example. So set Operating Pressure in the Pressure box to 0.

Click OK. It is important that you set the operating pressure correctly in compressible flow calculations since FLUENT uses it to compute absolute pressure to use in the ideal gas law. Define > Boundary Conditions Set boundary conditions for the following surfaces: centerline, inlet, outlet, wall. Select inlet under Zone and pick pressure-inlet under Type as its boundary condition. Click Set.... The Pressure Inlet window should come up.

Set the total (i.e. stagnation) pressure (noted as Gauge Total Pressure in FLUENT) and temperature at the inlet. For a subsonic inlet, Supersonic/Initial Gauge Pressure is the initial guess value for the static pressure. Calculate this initial guess value from the 1D solution. After you have entered the values, click OK to close the window.

Under the Thermal tab, the Total Temperature should be 300. Using the same steps as above, pick pressure-outlet as the boundary condition for the outlet surface. Then, when the Pressure Outlet window comes up, set the total pressure to 3738.9 as specified in the problem statement. Click OK. Make sure that wall zone is set to wall type and the centerline zone is set to axis type. Go to Step 5: Solve! Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Step 5: Solve! Now we will set the solve settings for this problem and then iterate through and actually solve it. Solve > Control > Solution Take a look at the options available. We want Second Order Upwind for the Flow (under the Discretization box).

Make sure that is selected and click OK. Solve > Initialize As you may recall from the previous tutorials, this is where we set the initial guess values (the base case) for the iterative solution. Once again, we'll set these values to be the ones at the inlet. Select inlet under Compute From.

Click Init. Solve > Monitors > Residual Now we will set the residual values (the criteria for a good enough solution). Once again, we'll set this value to 1e-06. Select the Plot option to see graphically whether the solution is converging.

Click OK. Solve > Iterate What does the convergence plot look like? How many iterations does it take to converge? Save case and data after you have obtained a converged solution. Go to Step 6: Analyze Results Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT

5. Solve! 6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Step 6: Analyze Results Mach Number Plot

As in the previous tutorials, we are going to plot the velocity along the centerline. However, this time, we are going to use the dimensionless Mach quantity. Plot > XY Plot We are going plot the variation of the Mach number in the axial direction at the axis and wall. In addition, we will plot the corresponding variation from 1D theory. You can download the file here: mach_1D.xy. Do everything as we would do for plotting the centerline velocity. However, instead of selecting Axial Velocity as the Y Axis Function, select Mach Number. Also, since we are going to plot this number at both the wall and axis, select centerline and wall under Surfaces. Then, load the mach_1D.xy by clicking on Load File....

Click Plot.

(Click picture for large image) How does the FLUENT solution compare with the 1D solution? Is the comparison better at the wall or at the axis? Can you explain this? Save this plot as machplot.xy by checking Write to File and clicking Write.... Pressure Contour Plot

Sometimes, it is very useful to see how the pressure and temperature changes throughout the object. This can be done via contour plots. Display > Contours... First, we are going to plot the pressure contours of the nozzle. Therefore, make sure that under Contours Of, Pressure... and Static Pressure is selected. We want this at a fine enough granularity so that we can see the pressure changes clearly. Under Levels, change the default 20 to 40. This increases the number of lines in the contour plot so that we can get a more accurate result.

Click Display.

(Click picture for large image) Notice that the pressure on the fluid gets smaller as it flows to the right, as is consistent with fluid going through a nozzle. Temperature Contour Plot

Now we will plot the temperature contours and see how the temperature varies throughout the nozzle. Back in the Contours window, under Contours Of, select Temperature... and Static Temperature. Click Display.

(Click picture for large image) As we can see, the temperature decreases towards the right side of the nozzle, indicating a change of internal energy to kinetic energy as the fluid speeds up. Go to Step 7: Refine Mesh Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve!

6. Analyze Results 7. Refine Mesh Problem 1 Problem 2

Step 7: Refine Mesh Solve the nozzle flow for the same conditions as used in class on a 80x30 grid. Recall that the static pressure p at the exit is 3,738.9 Pa. The grid for this calculation can be downloaded here. (a) Plot the variation of Mach number at the axis and the wall as a function of the axial distance x. Also, plot the corresponding results obtained on the 50x20 grid used in class and from the quasi-1D assumption. Recall that the quasi-1D result for the Mach number variation was given to you in the M_1D.xy file. Note all five curves should be plotted on the same graph so that you can compare them. You can make the plots in FLUENT, MATLAB or EXCEL. (b) Plot the variation of static pressure at the axis and the wall as a function of the axial distance x. Also, plot the corresponding results obtained on the 50x20 grid used in class and from the quasi-1D assumption. Calculate the static pressure variation for the quasi1D case from the Mach number variation given in M_1D.xy. (c) Plot the variation of static temperature at the axis and the wall as a function of the axial distance x. Also, plot the corresponding results obtained on the 50x20 grid used in class and from the quasi-1D assumption. Calculate the static temperature variation for the quasi-1D case from the Mach number variation given in M_1D.xy. Comment very briefly on the grid dependence of your results and the comparison with the quasi-1D results. Go to Problem 1 Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT

4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Grid Problem 1 Problem 2

Problem 1 Consider the nozzle flow problem solved using FLUENT in the tutorial. Recall that the nozzle has a circular cross-sectional area, A, that varies with axial distance from the throat, x, according to the formula: A = 0.1 + x2 where A is in square meters and x is in meters. The stagnation pressure poand stagnation temperature To at the inlet are 101,325 Pa and 300 K, respectively. Using the quasi-1D flow assumption, determine the static pressure at the nozzle inlet and outlet for the following conditions: (a) Sonic flow at the throat, and supersonic, isentropic flow in the diverging section. (b) Sonic flow at the throat, and subsonic, isentropic flow in the diverging section. (c) Sonic flow at the throat and normal shock at the exit. Go to Problem 2 Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback

Compressible Flow in a Nozzle Problem Specification 1. Create Geometry in GAMBIT 2. Mesh Geometry in GAMBIT 3. Specify Boundary Types in GAMBIT 4. Set Up Problem in FLUENT 5. Solve! 6. Analyze Results 7. Refine Grid Problem 1 Problem 2

Problem 2 Change the exit pressure to 40,000 Pa while keeping all the other boundary conditions the same. What flow regime do you expect for this exit pressure based on the quasi-1D results in problem 1? Re-run the FLUENT calculation with this exit pressure on the 50x20 grid. (a) Plot contours of the Mach number and static pressure for this case. Is the flow regime as predicted by quasi-1D theory? Explain briefly the possible causes for any similarities or disparities. (b) Plot the static and stagnation pressures at the axis as a function of the axial distance. Also, plot the corresponding values from the case where the exit pressure is 3,738.9 Pa. (These four curves should be on the same graph.) Explain briefly the salient features of this plot. (c) Plot the static and stagnation temperatures at the axis as a function of the axial distance. Again provide a brief explanation for the salient features. Back to Problem Specification Copyright 2002. Cornell University Sibley School of Mechanical and Aerospace Engineering. Fluent Short Course-Tutorial List | Feedback