Page History

{include: ANSYSFlow WBover -an Airfoil - Panel}
{include: FLUENT Google Analytics}

h1. Physics Setup

h3. Launch the Solver

In this step, we will open fluent and define the boundary conditions of the problem. If you haven't already, close the meshing window to return to the _Project Outline_ window. Now, click !update.png!. This will load the mesh into FLUENT. Now, double click *Setup*.  The _Fluent Launcher_ Window should open. Check the box marked {color:#990099}{*}{_}Double Precision{_}{*}{color}. To make the solver run a little quicker, under _Processing Options_ we will select {color:#990099}{*}{_}Parallel{_}{*}{color} and change the {color:#990099}{*}{_}Number of Processes{_}{*}{color} to {{2}}. This will allow users with a double core processor to utilize both.

\\  !Fluent Launcher.png!\\

h3. Select the Solver

Click {color:#990099}{*}{_}OK{_}{*}{color} to launch Fluent. The first thing we will do once Fluent launches is define the solver we are going to use. Select {color:#990099}{*}{_}Problem Setup > General{_}{*}{color}. Under _Solver_, select {color:#990099}{*}{_}Density-Based{_}{*}{color}.

h3. Models and Materials

Next, we will define the model we are going to use. We do this by going {color:#990099}{*}{_}Problem Setup > Models > Viscous-Laminar{_}{*}{color}. Then press {color:#990099}{*}{_}Edit..._{*}{color} This will open the _Viscous Model_ Menu Window. Select {color:#990099}{*}{_}Inviscid{_}{*}{color} and press *OK*. Now, we will specify characteristics of the fluid. Because we specified the fluid as inviscid, we will only have to define the density of the fluid. To make matters even simpler, we are only looking for non-dimensionalized values like pressure coefficient, so we will define the density of our fluid to be 1 kg/m^3. To define the density, click {color:#990099}{*}{_}Problem Setup > Materials > (double click) Air{_}{*}{color}. This will launch the _Create/Edit Materials_ window.

\\  !create materials.png!\\

Under _Properties_, ensure that density is set to {color:#990099}{*}{_}Constant{_}{*}{color} and enter {{1 kg/m^3}} as the density. Click {color:#990099}{*}{_}Change/Create{_}{*}{color} to set the density.


h3. Boundary Conditions

h5. Inlet

Now that the fluid has been described, we are ready to set the boundary conditions of the simulation. Bring up the boundary conditions menu by selecting {color:#990099}{*}{_}Problem Setup > Boundary Conditions{_}{*}{color}. In the _Boundary Conditions_ window, look under _Zones_. First, let's set the boundary conditions for the inlet. Select {color:#990099}{*}{_}Inlet{_}{*}{color} to see the details of the boundary condition. The boundary condition type should have defaulted to {color:#990099}{*}{_}velocity-inlet{_}{*}{color}: if it didn't, select it. Now, click {color:#990099}{*}{_}Edit{_}{*}{color} to bring up the _Velocity-Inlet_ Window. We need to specify the magnitude and direction of the velocity. Select {color:#990099}{*}{_}Velocity Specification Method > Components{_}{*}{color}. Remember, we want the flow to enter the inlet at an angle of 6 degrees since the angle of attack of the airfoil is 6 degrees; thus, the x velocity will be {latex} $ \cos\theta $ {latex}, and the y velocity will be {latex} $ \sin\theta $ {latex}. Specify {color:#990099}{*}{_}X-Velocity{_}{*}{color} as {{0.9945 m/s}} and {color:#990099}{*}{_}Y-Velocity{_}{*}{color} as {{0.1045 m/s}}. When you have finished specifying the velocity as entering the inlet at 6 degrees (the same thing as having an angle of attack of 6 degrees), press {color:#990099}{*}{_}OK{_}{*}{color}

\\  !Velocity Inlet.png|border=1!\\

h5. Outlet

In the _Boundary Conditions_ window, look under _Zones_. Select {color:#990099}{*}{_}Outlet{_}{*}{color} to see the details of the boundary condition. The boundary condition type should have defaulted to {color:#990099}{*}{_}pressure-outlet{_}{*}{color}: if it didn't, select it. Click {color:#990099}{*}{_}Edit{_}{*}{color}, and ensure that the {color:#990099}{*}{_}Gauge Pressure{_}{*}{color} is defaulted to {{0}}. If it is, you may close this window.

h5. Airfoil

In the _Boundary Conditions_ window, look under _Zones_ and select {color:#990099}{*}{_}airfoil{_}{*}{color}. Select {color:#990099}{*}{_}Type > Wall{_}{*}{color} if it hasn't been defaulted.

h3. Reference Values

The final thing to do before we move on to solution is to acknowledge the reference values. Go to {color:#990099}{*}{_}Problem Setup > Reference Values{_}{*}{color}. In the _Reference Values_ Window, select {color:#990099}{*}{_}Compute From > Inlet{_}{*}{color}. Check the reference values that appear to make sure they are as we have already set them.
\\
\\
[*Go to Step 5: Numerical Solution*|ANSYS WB - Airfoil - Solution]

[Go to all FLUENT Learning Modules|FLUENT Learning Modules]