There is a method how to use and what the main question under the pdf named WORKSHOP5 .Run according to pdf and after that follow the under points .And dont forget to put photos per cases.
This is an extra credit project – an opportunity to learn practical fluid mechanics career skills.
- Run the manifold example from class as your "baseline" case for reference. Experiment with changing the output plots and data that are available.
- There are hundreds of input parameters that make CFD run. Experiment with some of them and see the results.
- Select 4 specific inputs that have an appreciable or significant impact in changing the results.
- Run 4 cases, changing each of the 4 inputs – one at a time.
- Compare results from each of the 4 runs with your baseline reference case. For example – compare streamlines, pressures, velocities, etc.
- Research why the results changed the way they did.
- Prepare a Word document describing your results. For each of the 4 cases, describe:
- why did you chose changing this particular input?
- include plot(s) from the CFD comparing results to baseline.
- use science to explain why you believe the results changed.
- upload the Word doc (doc or docx file format) to this assignment link by the due date and time (Sunday 20 July at noon.)
No specific page length or work count is required. Quality is more important than quantity. It is certainly possible to communicate effective mastery of knowledge with relatively few words. On the other hand, it is also possible to write many pages and not explain much. However, it is anticipated that at least 1 to 1.5 pages, per case, would be reasonably required to articulate your results using words and graphs. Thus, a reasonable total page count target would somewhere in the 4 to 6 page range.
Original work is expected for credit. Cheating by copying other students work or plagiarizing the internet is unreasonable. No extra credit is offered if your work significantly matches another student's work, or the internet is plagiarized. Your submission will be checked for AI content and plagiarism
1
Workshop 5: Flow Through a Manifold
ANSYS Fluent Getting Started
Release 2022 R1
Introduction
• In this workshop you will start with an existing mesh file and setup a simulation of flow through a manifold. The goal of this simulation is to determine if the flow rate through each of the three outlets is uniform.
2
Problem Description
• Manifold is connected to an air supply pumping 30 liters per minute
• Goal is to split the airstream into three streams each at 10 liters per minute
– Within +/- 5%
• Gauge pressure = 0 Pa at each of the three outlets
• Simulation will predict whether the desired flow uniformity can be achieved with the existing design
It’s a good idea to identify the key simulation outcomes from the start. You can use these to monitor progress of solution.
3
Geometry and Operating Conditions
Air supplied to inlet at 30 liters per minute
3 outlets @ gauge pressure = 0 Pa
4
Start Fluent and Load the Mesh File
1. Launch Fluent in “Solution Mode” and once started, go to “File > Read > Mesh” and read “manifold-volume.msh.h5“ from the “Workshop5_Input_Files” directory.
5
Review of Fluent Workflow (Solution Mode): Ribbon
• The Ribbon is used to guide the basic Fluent workflow
• The four primary tabs used in every simulation are – Domain – Physics – Solution – Results
• For this case (and probably most other cases too), you will use them going in order from left to right
6
Domain: Mesh Check
2. In the Domain tab, click on “Check > Perform Mesh Check.” Ensure that there are no errors printed in the console.
The mesh check returns no error messages.
7
3. In the Physics tab, click “General…” and inspect the default settings in the general task page. This will be a steady state solve, so we can leave the defaults here.
Physics: Solver and Models
8
4. Still in the Physics tab, click on “Create/Edit…” in the Materials section of the ribbon. When the materials panel opens, inspect the default air material. This corresponds to air at atmospheric pressure and 15° C. This is appropriate for this workshop, so close this panel.
Physics: Materials
9
Physics: Zones
5. In Fluent, the cells in the mesh are grouped into one or more cell zones and each cell zone is bounded by one or more boundary zones. You will define boundary conditions for boundaries and cell zone conditions for cell zones. Default cell zone settings apply for this problem – you will learn about defining cell zone conditions in other workshops. However, boundary conditions need to be applied. Click “Boundaries” to bring up the Task Page for Boundary Conditions.
10
Physics: Boundary Conditions
6. There are six zones listed in the Boundary Conditions Task Page. There are three outlets, one inlet, and a wall boundary representing the exterior surface of the domain. The other zone in the list, interior-fluid, is the collection of all the internal faces of all the mesh cells. Fluent needs this for its internal data structure but no condition is applied on these faces.
Select “inlet” in the list and click “Edit…” to bring up the Edit Boundary panel. We will define appropriate conditions here in the next step.
11
7. Enter a value of 0.987 m/s for the velocity. This corresponds to a flow rate of 30 lpm (see appendix). Additionally, Change the turbulence specification method to “Intensity and Hydraulic Diameter.” Set the hydraulic diameter to 0.0254 m. Click “Apply” and “Close” the panel. (It is best practice to use this specification method for internal flows.)
Select “outlet-1” in the Boundary Conditions Task Page and click “Edit…” Note that the default setting for outlets is Gauge Pressure = 0. This is appropriate for this model. As with the inlet, change the turbulence specification method. This time set the hydraulic diameter to 0.01905 m. “Apply” and “Close.”
Physics: Boundary Conditions
12
Physics: Boundary Conditions
Set the turbulence specification method and hydraulic diameter for the remaining outlets.
The default behaviour for walls is to be adiabatic and impose the no-slip condition. This is also appropriate for this model, so the “wall” boundary condition does not require setup.
The boundary conditions are now correctly set for this model.
13
Solution: Report Definition
8. You will now setup a report definition to aid in monitoring the solution. In the Solution tab, click on “Definitions” in the Reports section and choose “New > Surface Report > Volume Flow Rate.” In the definition panel, set the name and surfaces as shown in the image below. Be sure to check the “Per Surface,” “Report File,” and “Report Plot” check boxes. Click “OK” to finalize the report when finished.
14
Solution: Residuals and Report Definitions
You will soon see that by default Fluent plots values of the residuals, which are indications of errors in the current solution. Residuals should decrease during the calculation and there are guidelines on the level of reduction needed for the solution to be considered converged. This will be covered in the class – defaults work fine for the majority of cases and will be used here.
It is also recommended to observe other important solution quantities, which is the role of Report Definitions. We are interested in the flow distribution, so for this problem it makes sense to check the flow rate at the outlets. We want to see that the values have stopped changing by the time the residuals converge.
15
Solution: Initialize and Calculate
9. You will now initialize and solve the model. Click “Initialize.” The iterative method used by Fluent to calculate the flow solution requires each of the cells to be assigned an initial value for all solution variables, which is what Initialize does.
Set the number of iterations to 600 and click “Calculate.”
16
10. Right click on the window tab and choose “SubWindow View” to show both the residuals and the report definition plot. If you want to go back, just right click and select Tabbed View.
The iterations will automatically stop when the residuals reach convergence. Notice in the plot on the right that the volume flow rates have reached a constant value. When the solution stops choose “File > Write > Case and Data” to save your progress.
Solving: Solution
In some models, due to the nature of the iterative solution method, the residuals can reach the default convergence level before the solution values become constant. This is undesirable and later in the course you will learn what to do if that happens.
17
Results: Reports
11. Move to the Results tab. In the Reports section, click on “Fluxes.” Select the “Mass Flow Rate” option and choose the inlet and three outlets in the list of boundaries. Click “Compute.” It is fine if your net result is not identical to the image to the right, but the results should be of the same order.
In the Flux Reports panel, a positive value of mass flow rate means that flow enters the domain and a negative value means it leaves the domain. Therefore, according to conservation of mass, if the values from all inlets and outlets are added together, they should sum to zero. Due to the nature of the numerical method, the Net Results value will never be exactly zero, but it should be small compared to the inlet value. Here it is O(10-6)%, which is practically zero. The normal expectation is that it should be less than 1%.
18
• The flux reports section on the previous slide showed the following
• The inlet flow rate is 6.06E-4 kg/s so if the flow were uniformly distributed between each of the three outlets, the flow rate at each outlet would be 2.02E-04 kg/s
• The flow rate through outlet3 is approximately 43% greater than the flow rate through outlet1
Results: Flow Distribution
19
Boundary Mass Flow Rate (kg/s)
Inlet 6.06E-04
Outlet1 1.57E-04
Outlet2 2.20E-04
Outlet3 2.29E-04
Outlet Deviation from Uniform Flow (%)
Outlet1 -22.3%
Outlet2 8.9%
Outlet3 13.4%
Results: Flow Pathlines
12. In the Graphics section, click “Pathlines > New…” In the Pathlines panel, select “inlet” for the release surface and color by “Time” instead of Particle ID. Click “Save/Display” and then Close.
20
Results: Flow Pathlines
Pathlines appear in the graphics window after Save/Display was clicked. The display can be improved to make a more appealing and easier to understand image. This can be done by combining the pathlines with the geometry. You will do this next.
Remember you can toggle the graphics between tabbed view and sub-window view by right clicking on the title bar of the tab or the window.
21
Results: Mesh Display
13. Right click in the Graphics window, select “Create > Mesh Display…” Under Options, unselect Edges such that only Faces are checked, and then select all surfaces in the list. Click “Save/Display” and then “Close.”
22
Results: Scene
14. To add transparency to the faces and show both the geometry and the pathlines, right click in the graphics window and select “Create” and then “Scene.” In the Scene panel, tick the checkbox for the mesh-1 and pathlines-1 objects. Set the transparency of the mesh object to about 80. Click “Save & Display.”
Mesh and Scene objects can also be created from the tree and the ribbon
23
Results: Summary
Using mesh display and scene to add the geometry to the graphics makes the flow pathlines easier to interpret.
The inlet flow mostly bypasses outlet-1 and feeds more directly into outlet-2 and outlet-3, which is probably the reason for the non- uniform flow distribution.
24
Save Case and Data, Close Fluent
15. You have completed this workshop. Write the case and data file using “File > Write > Case & Data…” Exit Fluent when finished.
25
Summary: Goals and Results
The purpose of this simulation was to determine whether this manifold design would achieve the design goal of equal flow distribution between its three outlets. After the solution was converged, the Flux Reports panel was used to check the flow rate through each of the outlets. The results showed that for this design, there was significant variation in the flow rate at each outlet
You used pathlines to visualize the flow and provide insight to the root cause of the non- uniform distribution in this design. Much of the flow entering the manifold passes over the opening for the first outlet and goes more directly into outlet-2 and outlet-3. This effect should be reduced in order to be able to achieve the design goal of uniform flow at each outlet.
26
Appendix
27
Flow Rate Hand Calculations
28
Geometry
Inlet Feed Diameter 1 inches
0.02540 meters
Inlet Feed Area 5.07E-04 square meters
Operating Conditions
Flow Rate 30 liters per minute
0.00050 cubic meters per second
Velocity (= Flow Rate / Inlet Feed Area) 9.87E-01 meters per second