[ANSYS, Inc. Logo] return to home search
next up previous contents index

6.8.11 Scaling the Mesh

Internally, ANSYS FLUENT stores the computational mesh in meters, the SI unit of length. When mesh information is read into the solver, it is assumed that the mesh was generated in units of meters. If your mesh was created using a different unit of length (inches, feet, centimeters, etc.), you must scale the mesh to meters. To do this, you can select from a list of common units to convert the mesh or you can supply your own custom scale factors. Each node coordinate will be multiplied by the corresponding scale factor.

Scaling can also be used to change the physical size of the mesh. For instance, you could stretch the mesh in the $x$ direction by assigning a scale factor of 2 in the $x$ direction and 1 in the $y$ and $z$ directions. This would double the extent of the mesh in the $x$ direction. However, you should use anisotropic scaling with caution, since it will change the aspect ratios of the cells in your mesh.


If you plan to scale the mesh in any way, you should do so before you initialize the flow or begin calculations. Any data that exists when you scale the mesh will be invalid.


It is a good practice to scale the mesh before setting up the case, especially when you plan to create mesh interfaces or shell conduction zones.

You will use the Scale Mesh dialog box (Figure  6.8.10) to scale the mesh from a standard unit of measurement or to apply custom scaling factors.

figure General figure Scale...

Figure 6.8.10: The Scale Mesh Dialog Box

Using the Scale Mesh Dialog Box

The procedure for scaling the mesh is as follows:

1.   Use the conversion factors provided by ANSYS FLUENT by selecting Convert Units in the Scaling group box. Then indicate the units used when creating the mesh by selecting the appropriate abbreviation for meters, centimeters, millimeters, inches, or feet from the Mesh Was Created In drop-down list. The Scaling Factors will automatically be set to the correct values (e.g., 0.0254 meters/inch).

If you created your mesh using units other than those in the Mesh Was Created In drop-down list, you can select Specify Scaling Factors and enter values for X, Y, and Z manually in the Scaling Factors group box (e.g., the number of meters per yard).

2.   Click the Scale button. The Domain Extents will be updated to show the correct range in meters. If you prefer to use your original unit of length during the ANSYS FLUENT session, you can follow the procedure described below to change the unit.

Changing the Unit of Length

As mentioned in Step 2. of the previous section, when you scale the mesh you do not change the units; you just convert the original dimensions of your mesh points from your original units to meters by multiplying each node coordinate by the specified Scaling Factors. If you want to work in your original units, instead of in meters, you can make a selection from the View Length Unit In drop-down list. This updates the Domain Extents to show the range in your original units and automatically changes the length unit in the Set Units dialog box (see Section  5.4). Note that this unit will be used for all future inputs of length quantities.

Unscaling the Mesh

If you use the wrong scale factor, accidentally click the Scale button twice, or wish to undo the scaling for any other reason, you can click the Unscale button. "Unscaling'' simply divides each of the node coordinates by the specified Scale Factors. (Selecting m in the Mesh Was Created In list and clicking on Scale will not unscale the mesh.)

Changing the Physical Size of the Mesh

You can also use the Scale Mesh dialog box to change the physical size of the mesh. For example, if your 2D mesh is 5 feet by 8 feet, and you want to model the same geometry with dimensions twice as big (10 feet by 16 feet), you can enter 2 for X and Y in the Scaling Factors group box and click Scale. The Domain Extents will be updated to show the new range.

next up previous contents index Previous: 6.8.10 Reordering the Domain
Up: 6.8 Modifying the Mesh
Next: 6.8.12 Translating the Mesh
Release 12.0 © ANSYS, Inc. 2009-01-29