# The mesh

We will create the mesh, start by double clicking Mesh in the box in Workbench. Once launched, the first thing he asks is the method of mesh. Here, because we'll give ourselves the specifications, the automated method will be fine.

Here we will learn how to mesh the boundary layers and wakes.

## Naming the parts

We'll start by naming the regions that have a particular interest:

• regeants entrance,
• recycling entrance,
• heater's wall,
• outlet,
• the walls,
• fluid zone.

Identifing these parts will allow us give them particular parameters in Fluent.

To name a party, you must select it => right click => Create the named selection => give it a name. To select a portion of the geometry, you need the tools accordingly: for surfaces, for the edges. Pressing Ctrl you can select multiple items.

Here is what we get :

## Meshing a boundary layer

### Around the heater

We'll now mesh the boundary layer around the resistor. We have to think about the number of cells our boundary layer must include. To do this we must know its size. According to the Blasius equation for a flat plate:

For the Reynolds Number, you have to give a feed rate: 100 l / min, a speed in the pipes of 0.85 m / s (with our pipes of 5 cm of diameter). It can be assumed that this speed is roughly the same around the cylinder as it is positioned just outside the diverging. We can estimate the thickness of the boundary layer around the sides to 2.5 cm.

To capture the dynamic and thermal effects, there should be about 20 cells. They should be closer near the cylinder, because the thermal boundary layer is thinner than dynamic.

A useful tool to mesh the boundary layers is inflation. It allows the mesh to reproduce the shape of the locally selected stops.

To do this: Right click on Mesh (left menu) => Insertion => Inflation. You must select a geometry that apply. The geometry is the area of the future grid will be changed by our specification. Here, they are the two areas close to the resistance. Then you must select a limit that is actually stops it will be reproduced by the mesh. Here is the resistance.

Now that we have specified the zone must specify what we want. The maximum thickness of the layer is 2.5 cm (attention, Mesher, the default unit is meters, think to convert), the number of layers is 20. To specify the spacing between the layers, you can play on the growth rate, it defines the ratio of the distances between two layers. We can leave it at 1.2.

If you generate the mesh now, you should see this:

We notice that we just created 10 000 cell. For a mesh tutorial, it's a lot. To thin the calculations in Fluent, put 200 divisions.

That's it for the mesh around the resistance.

### Around the wall

Here one must bear in mind that the phenomena of sheering to the walls does not really concern us. We are using inflation to determine the number and shape of the vertical divisions close to the walls. We will not immediately fix the number of axial divisions.

To do this: Right click on Mesh (left menu) => Insertion => Inflation. This time to select the geometry and limits, we will not click on it, we will use the names we have given to different elements. In fields: Method of scope and method of defining limits, choose the named selection option. Below, a menu appears. You just have to choose the area for the fluid geometry and walls as edges.

Regarding the parameters, say we want to have 10 point in a space of 0.5 cm around the walls. We must therefore seize: maximum thickness: 0.5 cm, the number of layers: 10. Always with a growth rate of 1.2.

That's what happens on the conduit entry:

## Meshing an area

### Meshing the mixing zone

To mesh the mixing zone, two methods available to us:

• specify the size of all the edges or number of divisions,
• give the size of the divisions that we want to see.

Here we will use the second method. To catch the phenomena, there should be a number of cell equivalent to the Reynolds Number. The surface is 100 cm ², Reynolds is about 4000. The side of a piece of square should measure about 1.6 mm.

To do this: Right click on Mesh (left menu) => Insertion => Sizing. Select the connection, and fix the size of elements: 1.6 mm (again, beware of the conversion). That's what you get:

As we see earlier that the specifications are cumulative. Here we see the influence of cell size and inflation.

To shorten the calculation with Fluent, you can increase the size of items.

### Meshing the wake

You will notice that if we use the same method as above, we will add cells near the wall, where they may not be very useful. Here we will use the second method mentioned earlier: We will precise the division of the edges. The method is the same as for divisions of the radial resistor.

This time, to specify to Mesher that divisions of the edges will extend over the surface, you must declare a face-mapped, right click on Mesh (in the left menu) => Insertion e=> Face mapped. Then you select the wake and confirm.

We'll begin with the horizontal edges. Let's start by right clicking on mesh (in the left menu) => Insertion => Sizing. Select the two parallel edges that border the wake. The size of elements in the center of the wake directly after the resistance is 0.1 mm. It is therefore no more branching. We're going to put elements of 0.1 mm square in the center of the wake and the component 10 times larger towards the walls.

The proposed control does extremely fine. In size of the elements, use 1 mm, this size is that of an element near the wall. Then select what type of gap (the cells will be smaller in the center as shown in the drawing):

The biasfactor is the ratio of lengths between most cell and that outside the innermost. Here, with 10, the cells in the center will be the order of 0.1 mm and outwards of about 1 mm.

We will now specify the divisions of the two vertical boundaries of the area. The edges are oriented, when choosing the type of bias should be careful not to branch out by the exit.

Let's start by right clicking on mesh (in the left menu) => Insertion => Sizing. Select one of the two edges. Apply the same choice as before: size of the elements, use 1 mm, and standard deviation factor deviation as follows:

Do the same with the other stops. Generating the mesh you should get:

Now, my mesh is around 40 000 cells. Feel free to drop the resolution for faster calculations.

## Meshing common areas

We do more than mesh areas that are the elbow and pipes. For this, we use the general settings. Click (left click) on mesh, tabs default settings and sinzing are particularly interesting.

In default setting, the relevance allows an offshoot of global mesh, regardless of geometry. By making your move towards -100 mesh becomes coarser, about 100 it becomes finer.

In sizing, you can choose the advanced size function.

The feature advanced size function offers several modes:

• curvature allows you to set the maximum angle formed by the successive centers of gravity. It is more compact, more branching will be important when approaching circular surface (it could very well use it to mesh around the resistance)
• proximity: you can control the number of cell between two walls,
• proximity and curvature mode combination of the two previous
• fixed: This mode tries to mesh meshed with regular quadrilaterals.

Given our setup, we choose the mode curvature. Since we have already specified the mesh around the cylinder, simply specify the size of face max (maximum allowable size of elements). We'll take 3 mm (three times the diameter of the pipe divided by Reynolds).

That's what happens at the entrance of the elbow:

Here, everything is meshed. With some reduction, my mesh is around 20 000 cells.

Now save and run Fluent from Workbench by double clicking it.