Jet: Turbulent flow
Geometry Creation……………………………………….PG.2
Mesh Creation……………………………………………PG.6
Set up……………………………………………………..PG.9
Solution…………………………………………………...PG.13
Results…………………………………………………….PG.15
Validation…………………………………………………PG.16
Geometry Creation:
- Open ANSYS Workbench and start a new project.
- Drag the Fluid Flow (Fluent) Analysis System to the project schematic.
- Since dealing with a 2d geometry, right click on Geometry and select Properties.
- Under Advanced Geometry Options for Analysis Type select 2d.
Figure 1J
- Double click on geometry and a new window will appear.
Figure 2J.
- click on the default unit, Meter then OK
Under Tree Outline, select XY-Plane, and then click on Sketching right before Details View. This will bring up the Sketching Toolboxes
- Click on the +Z axis on the bottom right corner of the Graphics window to view the XY-Plane.
Figure 3.J
It should now look like this
Figure 4 J
- Select sketching from the Tree Outline
- Select Rectangle from the Draw options.
- In the graphics window place the cursor at the origin. The letter P should be visible meaning that point is fixed at the origin.
- Begin by drawing a small rectangle, then draw another rectangle on top of it, and then another rectangle to the right of it
Figure 5J
- Next under Sketching toolboxes select modify and click trim and remove the lines inside the jet
Figure 6J
- Once that is done under sketching toolboxes go to modeling, select the radio button for XY plane, click on the sketch 1 and then go up to concept select surfaces from sketches. Once that is done select generate
- The user should now have a figure that looks approximately like this
Figure 7 J
- To give it dimensions the usernow needs to go under tree outline on the left and select sketching. Next select dimensions and select the following sides and give them the following dimensions
Figure 8J
- Select generate and exit
Mesh Creation
- Open up mesh from the main window
- Under outline click on mesh and then on the top of the screen select mesh control and mapped faced meshing
- Then click the cube sizing on the top of the screen and then click on the shape, and then under details of mapped faced meshing select apply, this should turn the shape green
Figure 9J
- Next select edge cub button
- Select a side and then under select sizing, repeat this step for the following sides in this order
The screen should now look like this with 8 different edge sizing’s
Figure 11J
Then the user has to apply biasing with different divisions for each , the bias should be toward the bottom, and toward the jet
Edge size / Divisions / Bias factor / Behavior1 / 30 / 10 / Hard
2 / 30 / 12 / Hard
3 / 70 / 40 / Hard
4 / 70 / 40 / Hard
5 / 5 / 5 / Hard
6 / 5 / 5 / Hard
7 / 30 / No bias / NA
8 / 30 / No bias / NA
Table 1. Mesh Values
Next the user should hit update and the mesh should appear
Figure 12J.
Once this is done select the edge cube again and select the top and right to be pressure outlets, and the left and top of the pipe to be wall, and then the inlet be jet, naming them respectively
Figure 13J
- Update and then exit
Set up
- On the main window select it and press when the new widow comes up
- Under general make sure under 2d space axisymmetric is selected
Figure 14J
- Under models for viscous double click it and change the values around to look like so
Figure 15J
- Under materials double click on air and make sure the following values are there
Figure 16J
- Under boundary conditions, click on Jet and make sure the following values are set
Figure 17J
- Then click ok, double click on pressure outlet and ensure the following values are set
Figure 18J
- Then click ok, click on wall and ensure the values are set
Figure 19J
- Then click ok, make sure each of the names under zone is set to its respective type
Zone / Type
Axis / Axis
Interior- Surface_ body / Interior
Jet / Velocity-inlet
Pressure_ outlet / Pressure_outlet
Wall / Wall
Table 2J. Zone Names
Solution
- Under reference values, where it says compute from click on that drop box and select Jet
Figure 20J
- Under solution method make sure the following are selected
Figure 21J
- Select solution controls and then under relaxation factors make sure the following values are there for each
Under- Relaxation Factors / Values
Pressure / .3
Density / 1
Body forces / 1
Momentum / .7
Turbulent Kinetic Energy / .8
Turbulent Dissipation Rate / .8
Turbulent Viscosity / 1
Table 3J. Relaxation Factors
- Under Solution Initialization, under where it says compute from, select jet and click initialize
- Go down to run calculation and check for 300 iterations and select calculate
Results
- Under graphics and animation, select contours and where it says contours of select Velocity and then under surfaces select interior surface body and then under options to the left select filled
Figure 22J
- Select display
Figure 23J
- This is what it should look like
Validation
- Go to plots and select XY plot under Plots and display the velocity plot along the axis
- It should look like this
Figure 24J
- In a Jet the highest velocity should appear a bit past the orifice as it is seen and then the velocity should die down as it is seen.
- However, to truly validate these results again select plot, xy plot and in there select write to file and save it somewhere, under file types click that drop down and select all files and then name it whateveryouwant.xls this file can then be opened in excel go ahead and open it
Once in excel create a graph is as follows
- The left y-axis Is going to be the centerline velocity divided by the velocity at the exit in our case 104.716
- The x-axis will be the centerline distance meaning the total length of our design divided by the diameter of the orifice the graph should look like so
Figure 25J
Figure 26J
- The next validation is the Log Log graph. In excel by right clicking each of the axis numbers under format axis the user can select log scale. Do so for both and the graph should look like so
Figure 27J
- Where this value should have a slope of -1 , which it is.
1 | Page