computationnel fluide Dynamics PDF

Preview

Summary

a pdf that show you how to work on ansys fluent
for biggeners on fluent you can learn how to solve simple problem on cfd...

Description

19.2 Release

Workshop: Ball Valve ANSYS Fluent Meshing with Watertight Geometry Workflow

Introduction • This workshop demonstrates the single-window workflow in ANSYS Fluent, using the Watertight Geometry workflow in Fluent Meshing to solve for the flow through a ball valve assembly • All steps are not shown explicitly in the slides – please watch the video for complete details

2

© ANSYS, Inc.

Start Fluent • Activate Meshing Mode in Fluent Launcher before starting • Use 4 solver processes if available

3

© ANSYS, Inc.

Activate Watertight Geometry Workflow

4

© ANSYS, Inc.

Import CAD • Select Import Geometry task, click ellipsis and select ball-valve-assembly.scdoc

5

© ANSYS, Inc.

Add Local Sizing • Leave Add Local Sizing input as "no" and click Update

6

© ANSYS, Inc.

Create Surface Mesh

Set Minimum Size and Maximum Size to 0.36 mm and 2.5 mm, respectively. Keep default settings for curvature and proximity sizing functions.

7

© ANSYS, Inc.

Describe Geometry

Geometry consists of only solid regions.

Select Yes to cap openings and extract fluid regions. The fluid-fluid boundary types setting does not apply in this example, leave default entry.

8

© ANSYS, Inc.

Create Capping Surfaces: Inlet Change "Select By" option to "zone". Using the right mouse button, click the annular surface shown in the figure to select it. Enter "inlet" for Name and select "velocity-inlet" for Zone Type Click Enclose Fluid Regions (Capping)

9

© ANSYS, Inc.

Create Capping Surfaces: Outlet Using the right mouse button, click the annular surface shown in the figure to select it. Enter "outlet" for Name and select "pressureoutlet" for Zone Type Click Enclose Fluid Regions (Capping)

10

© ANSYS, Inc.

Create Capping Surfaces: Outlet Using the right mouse button, click the annular surface shown in the figure to select it. Enter "outlet" for Name and select "pressureoutlet" for Zone Type Click Enclose Fluid Regions (Capping)

11

© ANSYS, Inc.

Create Regions & Update Regions Click Create Regions.

Four solid regions will be extracted from the CAD model and one fluid region will be extracted based on the capping surfaces. In the Update Regions task, click on the name field for "fluid:0", rename it "fluid" and click Update Regions

12

© ANSYS, Inc.

Create Volume Mesh

Set Number of Layers to 8. Keep method of "polyhedral" for volume fill.

Click Create Volume Mesh.

13

© ANSYS, Inc.

Minimum orthogonal quality of 0.13 is acceptable, so proceed to solution .

Write Mesh and Switch to Solution

Write the mesh file before switching to solution. This is not required, but in case it is desired to make changes in the future, the mesh file can be read into Fluent Meshing and all the workflow inputs are preserved so it is easy to make changes.

14

© ANSYS, Inc.

Click on Switch to Solution. Click Yes when prompted.

Setting Up Physics: Viscous Model

In the Setting Up Physics tab, click Viscous and and activate the SST k-omega turbulence model

15

© ANSYS, Inc.

Setting Up Physics: Boundary Conditions

Set inlet velocity to 7.5 m/s Retain default values for outlet 16

© ANSYS, Inc.

Solving: Solution Methods

Set Pressure-Velocity Coupling scheme to Coupled. Select "Pseudo Transient" near the bottom of panel. For most incompressible flows, these settings offer superior convergence to default settings.

17

© ANSYS, Inc.

Solving: Report Definitions

Define a surface report to plot the area weighted average of static pressure on the inlet. The inlet pressure is the quantity of interest for this simulation and the report plot will help to ensure that its converged value has been established. 18

© ANSYS, Inc.

Solving: Run Calculation 2. 1.

3.

Click Initialize, set the number of iterations to 200 and click Calculate. Residuals decrease monotonically until convergence criteria are achieved. Plot of inlet pressure shows that final value has been attained.

19

© ANSYS, Inc.

Postprocessing: Fluxes

Go to Fluxes… in the Postprocessing tab and perform a mass balance. The net imbalance is several orders of magnitude less than the inlet flow rate, indicating excellent mass conservation has been achieved in the numerical solution.

20

© ANSYS, Inc.

Postprocessing: Iso-Surface

Create an iso-surface of Z-coordinate = 0 to display the solution on a plane through the center of the flow passage.

21

© ANSYS, Inc.

Postprocessing: Contours

Create contours of static pressure and velocity magnitude on the z=0 iso-surface

22

© ANSYS, Inc.

Postprocessing: Pathlines

Right click in graphics window and select Create > Pathline. Set Color By to Particle Variables, Time and release from inlet.

23

© ANSYS, Inc.

Postprocessing: Mesh Display Object

Right click in graphics window and select Create > Mesh Display. Under Options, select only Faces. Under Surfaces, select all wall boundaries.

24

© ANSYS, Inc.

Postprocessing: Scene Display

Right click in graphics window and select Create > Scene Select mesh and pathlines objects.

Apply transparency to the mesh object so both mesh and pathlines are visible. Exact value of transparency is unimportant – use any value that produces an appealing visual. 25

© ANSYS, Inc.

Postprocessing: Create an Additional Scene with Velocity Contours

Save the case and data file after creating the second scene. All graphics objects are stored in the case file. They can be displayed at any time after loading the data file (no need to repeat the setup, just right click in the tree and select "Display") and will be automatically updated if the solution is recalculated (e.g. if boundary conditions, material properties, … are changed). 26

© ANSYS, Inc.

Summary • This workshop demonstrated the use of the single-window workflow in ANSYS Fluent • Within the same window, and in the same session − Geometry was imported from CAD − Capping surfaces were defined and a flow volume was extracted − A high quality CFD volume mesh was created with polyhedral cells and boundary layers − Solution mode was activated after the mesh was created − The problem was defined and solved − Persistent graphics objects and scene displays were created in postprocessing

• The Watertight Geometry workflow in Meshing mode enabled CAD import, volume extraction and meshing through a sequence of predefined tasks with simple and intuitive user inputs 27

© ANSYS, Inc....