CFD Analysis

When the Incompressible check box is selected, the density of the fluid and its specific heat ( ), viscosity ( ), and conductivity ( ) must be entered. Gamma ( ), the ratio of specific heats at constant volume and pressure, is unity for incompressible fluids, so the Gamma section is inactive. Gas Constant ( ) is also inactive. The thermal and caloric equations of state for incompressible fluids are shown below. is density, and represents the internal energy per unit mass.

Since the density entered in the Fluid Properties dialog represents the density of the fluid throughout the physical domain, you are not allowed to enter a reference value for density in the Reference Values dialog, or choose a density field variable on the Field Variables dialog (see Identifying State Variables).

Specific heat ( ) is the amount of energy required to raise a unit mass of the fluid one degree. It has dimensions of:

Viscosity ( ) represents the dynamic viscosity coefficient, in units of

Conductivity ( ) is the thermal conductivity of the fluid, in units of:

When the Incompressible check box is not selected, the specific gas constant, gamma, viscosity and conductivity must be entered. Since density is not a constant property of compressible fluids, the Density text field is inactive, as is the Specific Heat section of the dialog. The thermal and caloric equations of state for compressible fluids are shown below. is pressure, and is internal energy per unit mass:

The gas constant is the universal gas constant divided by the molecular weight of the fluid:

giving units of:

Gamma is the ratio of the gas specific heats and is non-dimensional:

Consider a case where temperature is non-dimensionalized by dividing it by free-stream temperature:

and pressure is non-dimensionalized with gamma (the ratio of specific heats) and free-stream pressure:

We wish to know what to enter for the gas constant in the Fluid Properties dialog. We plug what we know into the thermal equation of state (where is density and is the gas constant):

Since the equation of state must hold for the free-stream conditions, we know:

From this, we see that the product of denominators (1) and (2) in the second-previous equation must equal thus:

This doesn’t entirely answer our question, however, and in the absence of additional information, we simply need to decide how and are each individually non-dimensionalized. The requirement we just determined is that the product of the two must be non-dimensionalized by So we may decide to non-dimensionalize density by free-stream density, , which leaves the gas constant non-dimensionalized (that is, divided) by . In the Fluid Properties dialog, we enter for Gas Constant. If we chose to leave Gas Constant at unity, density would be non-dimensionalized by gamma and free-stream density, .

Select the convective variables in your dataset by clicking the Select button in the top section of the Field Variables dialog. Choose one of the two options on the Field Variables dialog to indicate whether these variables represent pure velocity or momentum.

The State Variables region of the dialog allows you to identify up to two variables, such as pressure and temperature, in your data. From the two drop-downs, select any two choices from the types: Pressure, Temperature, Density, Stagnation Energy, Mach Number, or Not Used. Then click Select, and choose the corresponding variable(s) from your data. If you have only one thermodynamic variable, select "Not Used" in one of the drop-downs. For incompressible flow, (see Specifying Incompressible Fluid Properties) you may specify Pressure for one variable, and you may specify Temperature or Stagnation Energy (per unit volume) for the other.

The Select button launches the Select Variables dialog which allows you to select variables in your dataset. The selections in the drop-down menus mentioned above determine whether these variables represent pressure, temperature, density, stagnation energy or Mach number.

Establishing connections across zone boundaries allows Tecplot 360 to calculate better gradient quantities at these locations. There may be a substantial performance penalty for ordered-zone calculations, because at these boundary locations, Tecplot 360 uses the finite element least-squares formulation for calculating the gradients. Refer to Gradient Calculations for a discussion of gradient calculations.

You may associate cell boundary faces (cell faces on the exterior of a zone) with a boundary condition. There are two reasons why you might want to do this:

If you set a boundary condition on a particular cell boundary face, that face will not be considered connected to any other cells by the gradient calculation routines. This may be advantageous, for example, in solutions containing a thin flat plate, where nodes on either side of the flat plate overlap and would otherwise be connected by the connection mechanism.

For three-dimensional flow solutions, you can use the Extract Flow Features dialog to extract separation and attachment lines. These lines are only calculated on boundaries you have identified as wall boundaries. While other boundary conditions may be specified, this information is not currently used, aside from inhibiting connections.

The Edit Boundary dialog is displayed by clicking New on the Geometry and Boundaries dialog, or by selecting an existing boundary and then selecting Edit.

It allows you to identify a boundary of one or more zones, either by entering the zone number(s), face and index range on that face, or by entering the zone numbers of boundary zones, as discussed in Setting Geometry and Boundary Options. Enter the desired options and select OK to add the boundary to the Geometry and Boundaries dialog.

To direct Tecplot 360 to treat your dataset as representing a steady-state solution, select the Flow Solution is Steady-State option. This setting disables the remainder of the dialog.

To direct Tecplot 360 to treat your dataset as an unsteady solution, toggle-off Flow Solution is Steady-State. This enables the remainder of the dialog, where you can identify your solution time levels.

An unsteady flow solution consists of a sequence of zones that represent successive solution times. Each time level may be represented by one or more zones. Identify solution time levels by entering the zone number(s) for a particular solution time level in the Zones text field and the time they represent in the Time text field, then selecting [Add]. The zones and associated time appear in the Solution Time Levels list. You may edit an existing time level by selecting it in the list. Its time and zones appear in the text fields, where you may edit them. Clicking Replace updates the currently selected list time level with the modified one.

By manually entering each time and associated zones in the text fields, you may identify all solution time levels in the current dataset. For large numbers of zones, two additional methods of entering time levels are provided. If your solution, or some portion of it was calculated with a constant time step, you may use the Group Zones by Time Step Dialog to enter all of these time levels at once. Alternatively, if your zone names contain the solution time each zone represents, you may enter all of your time levels by parsing the zone names for their corresponding solution time. These options are discussed below.

The Group Zones by Time Step dialog allows you to enter a sequence of solution time levels into the Unsteady Flow dialog more easily than manually entering each time level.

If the names of your solution zones contain the solution time they represent, you may automatically enter all time levels by parsing the zone names for these times. Zones of the same solution time will be grouped together. The times must be preceded in the zone name by some identifiable text, such as "Time=." Enter this text (without quotes) in the text field, then select Parse.

If variable sharing is enabled, all variables from which the function is calculated are shared between multiple zones, and they and the calculated variable are all at the same location (cell-centered or nodal), the new variable will be shared as well. You can see which variables in a dataset are shared in the Data Set Info dialog (accessed via the Data menu).

Variables calculated with the Calculate-on-demand option are added to the dataset, but are not calculated until they are needed. This can save a lot of time when working with unsteady solutions where only a small number of zones are displayed at any given time. Displaying a contour plot of the calculated variable will only result in calculation of the variable for the currently active zones. Activating new zones (by, for example, advancing the solution time displayed in Tecplot 360) will result in the calculation being performed only for the newly displayed zones.

A calculate-on-demand variable is a function of other variables in the dataset and is calculated using the Calculate dialog. Calculate-on-demand variables are recalculated whenever a variable that they are a function-of is recalculated. For example, given Pressure = f(Gas Constant), if the value of Gas Constant changes, Pressure is recalculated.

To avoid circular data dependencies, you are prevented from selecting calculate-on-demand variables in the Fluid Properties or Field Variables dialogs. In addition, you cannot delete any variables on which a calculate-on-demand variable is dependent.

If you plan to make a sequence of changes to your data and analysis settings, you can inhibit these automatic recalculations by turning off Tecplot 360’s Auto-Redraw feature. Recalculation will then take place only when you redraw the frame.

If the data journal is valid, alterations made to the dataset with the Calculate dialog may be undone by selecting Undo from the Edit menu. This will result in Tecplot 360 re-executing the data journal, which may be a lengthy process.

The function name may be typed into the Name text field, or selected from a list which contains all available functions. Click [Select] to display the Select Function dialog.

Selecting a function from this dialog and selecting OK enters that function in the appropriate area. Functions in this list which only apply to 3D solution data begin with (3D). Vector functions, whose names are appended with (vector), calculate three vector components. Each of the available functions is described in Calculate Variables Reference.

An alternative method of selecting a function is to enter its equivalent PLOT3D function number. These numbers may also be found in Calculate Variables Reference. If a valid function number is entered into the Name text field in the Calculate dialog, Tecplot 360 replaces the number with the name of the corresponding function and sets the Normalize drop-down to None or Reference Values as appropriate.

Most of the PLOT3D functions are scalar functions. Gradient calculations are a notable exception to this rule, however, and depend on values at neighboring points. Understanding how these calculations are performed may help you interpret the results.

With Tecplot 360’s CFDA variable calculation feature, you can calculate and display surface normal vectors on your plot. This includes the following steps:

In detail, the steps above include the following.

To calculate the normal, choose "Calculate Variables" from the Analyze menu. In the Calculate dialog, choose "Grid K Unit Normal (vector)" as the variable to calculate (to do this, click the Select button, and scroll down in the list that appears to find "Grid K Unit Normal (vector)", and click it). Choose "Cell Center" as the New Var Location, and click Calculate.

Next, toggle-on the Vector layer in the Plot sidebar to turn on the normal vectors, and choose the components of the calculated vector to display in the Select Variables dialog for vectors. This dialog appears when you toggle-on the vector layer for the first time; you can also open the dialog by going to Plot → Vector → Variables in the menu bar. To display the "Grid K Unit Normal (vector)" normal, choose the three components "X Grid K Unit Normal", "Y Grid K Unit Normal", and "Z Grid K Unit Normal" for the X, Y, and Z components of the vector layer, respectively.

Lastly, click the Zone Style button in the Plot sidebar to open the Zone Style dialog. In that dialog, switch to the Points page, and choose "Cell Centers Near Surfaces" from the Points to Plot menu.

Macro commands may access the results of the most recent integration through specific environment variables. Each of these variables represents the total over all zones (the final number shown in the Integration Results dialog). For all integration types except Forces and Moments, the single result is stored in the variable INTEGRATION_TOTAL. Table 1 shows the variable names for forces and moments.

Environment variables are accessed in macros in the same way as regular macro variables, except that a $ is prefixed to the variable name. For example, the following macro command would display the result of the most recent scalar integration:

You can also access integration results as frame auxiliary data. For example, to access the INTEGRATION_TOTAL variable as aux data, use the following syntax:

The following sections demonstrate potential uses of the Integrate dialog.

The first two drop-down menus on the Turbulence dialog allow you to specify which turbulence variables are contained in your dataset. The options are Kinetic Energy ( ), Dissipation Rate ( ), Turbulent Frequency ( ), Turbulent Kinematic Viscosity ( ), and Turbulent Dynamic Viscosity( ). This last option is the kinematic viscosity, which is equal to the dynamic viscosity divided by the density.

You may select the location (nodal or cell-centered) of new variables Tecplot 360 creates during a calculation with the New Var Location dropdown. This setting only affects new variables added to the dataset when you click Calculate. Variables that already exist in the dataset keep their existing locations. If you wish to change the location of an existing variable, you can delete or rename the variable and then perform the calculation with the desired setting for New Var Location.

Selecting the Calculate on Demand option results in the calculated variable being added to the dataset when you click the Calculate button, but the actual calculation is delayed until it is actually needed. Please refer to the discussion of calculate-on-demand in Calculating Variables.

Once you have identified two turbulence variables in your dataset, you may calculate either of the other two. Select the desired function from the Function drop-down menu and click Calculate. The function is calculated and added to your dataset as a variable with the same name as the function selected. If your dataset variables are and , the following formulae will be used for the calculations of and :

with . Equations for other input variables are derived from these.

If both variables from which the turbulence function is calculated are shared between multiple zones, and they and the calculated variable are all at the same location (cell-centered or nodal), the new variable will be shared as well. This mimics the behavior of the Data→Alter→Specify Equations dialog.

A particle path is the path that a single particle follows through a solution. In steady flow, particle paths are the same as streaklines and streamtraces for massless particles. To calculate particle paths, you must:

Streaklines simulate experimental techniques which involve the periodic or continuous release of a tracer substance, such as oil drops or smoke. Tecplot 360 produces streaklines by releasing a sequence of particles from the release points and integrating the unsteady velocity field to find their positions in the flow at the end solution time. The final positions of all particles emitted from a particular release point form one streakline. Once streaklines have been calculated, they may be animated on screen or to a file.

To calculate Streaklines, perform the following actions:

It is not reasonable to calculate streaklines for steady-state flow, because in steady-state flow, even for particles with mass, streaklines are the same as particle paths (just more time consuming to compute).

Whereas massless particles always travel with the local fluid velocity, particles with mass travel according to a more complicated equation of motion where the fluid creates drag on the particle. In addition, particles with mass may have a temperature that is different from the local fluid temperature, and they may lose mass due to ablative processes such as vaporization. The Particle Mass Options dialog allows you to enter coefficients and particle properties to indicate how these mass-related effects are calculated.

The Particle Mass Options dialog is displayed by selecting Mass Options on the Particle Paths and Streaklines dialog. It allows you to specify either general or detailed coefficients related to the particle trajectory and heat transfer calculations, plus options related to gravity and the initial particle velocity. If you choose to calculate the particle temperature, you may choose to terminate the particle at a specified temperature, or, with the detailed coefficient option, to ablate the particles until their mass reaches zero.

The accuracy of a sequence of three solutions is estimated using Richardson extrapolation on a particular dataset variable you select. The resulting accuracy in both the 1-norm and the Max- (infinity-) norm is reported in a text dialog. You also have the options of plotting the overall error versus grid spacing, or plotting the calculated accuracy at each grid node.

To calculate solution accuracy, you must identify three zones from your dataset. The zones must represent coarse, medium, and fine grid solutions of the same problem. The order in which you enter the zone numbers does not matter. The medium grid must have twice the number of cells in each index direction as the coarse grid, or twice, plus one, the number of nodes. The fine grid must have four times the number of cells, or four times, plus one, the number of nodes as the coarse grid.

Since finite element zones do not have identifiable index directions, the requirement for the coarse, medium and fine grid sizes is only in terms of the total number of cells. It is assumed that successively finer grids have been refined equally in all directions. The requirement is that the medium grid have eight times as many cells (four in 2D) as the coarse grid and the fine grid have 64 times as many cells (sixteen in 2D).

For all zone types, the medium and fine grids must have nodes that overlap the coarse grid nodes.

You may type the zone numbers in the text field, or select them by clicking Select and choosing three zones from the resulting list.

Under some circumstances, Richardson extrapolation can report an accuracy in excess of the solver’s theoretical maximum accuracy. For this reason, Tecplot 360 limits the accuracy used by this technique to the value you enter in the Maximum Accuracy text field. Although fractional values are allowed in this text field, you should enter the theoretical maximum order of accuracy of your solver as an integer. That is, two for a second-order accurate solver.

For the accuracy calculation, Tecplot 360 performs Richardson extrapolation on one variable in your dataset. It must not be a grid variable. Enter the name of the variable in the Use Data Set Variable text field, or click Select to choose the variable.

You can plot the results of the accuracy calculation in either or both of two ways. First, you can plot the accuracy at each grid node as a contour plot (XY-plot for 1D data) by setting the Plot Accuracy at All Grid Nodes check box. Second, you can plot the overall error as a log-log XY-plot by setting the Plot Overall Accuracy (log-log) check box. If you select either of these options, new frames will be created to display the plots when you perform the calculation.

The plot of overall accuracy plots the error in the 1-norm and max- (infinity-) norm versus grid spacing for each of the three zones. The grid spacing of the coarse grid zone is taken as unity for this plot. The 1-norm is the average absolute value of the difference between the extrapolated solution and the solutions of the input zones. The max-norm is the maximum absolute value of this difference. Figure 12 shows an example of this plot. The slopes of the two lines represent the accuracy of the solver. A significant difference in the slopes may indicate discontinuities in your solution, or other problems with the calculation.

The plot of accuracy at all grid nodes plots the calculated accuracy on the grid from your coarse solution. For 2D and 3D grids, it is plotted as a contour plot. For 1D solutions, it is plotted as an XY-plot.

Because this feature creates a new frame, it cannot be saved in the data journal, and the current data journal is invalidated. If you subsequently save a layout file, you will be prompted to save a new data file.

When you select [Calculate Accuracy], the accuracy calculation is performed. The accuracy in the 1-norm and max-norm is reported in a text dialog. If you selected either of the plot options, the plots are created in new frames.

Given three solutions on successively finer grids, Tecplot 360 can perform Richardson extrapolation to improve the accuracy of the solution, and report the difference between the extrapolated solution and the original, fine grid solution.

To perform this extrapolation, three zones must be identified in the Error Analysis dialog as previously discussed (see Selecting Solution Zones) and the maximum accuracy of the solver entered (see Specifying the Solver’s Maximum Accuracy). Once these are entered, clicking Extrapolate Solution creates two new zones in the solution dataset. The first new zone contains the extrapolated solution on the coarse grid. The second new zone contains the difference between the extrapolated solution and the original fine grid solution.

To extract shock surfaces, select Shock Surfaces from the Feature drop-down, then click Extract. The remaining controls on the dialog are disabled. After calculation, shock surfaces are then displayed as iso-surfaces of a new dataset variable named ShockFeature. This variable is similar to the Shock variable available on the Calculate dialog.

You may note that the displayed shock surface is obscured by clutter due to the sensitivity of the shock function capturing minor oscillations in the solution. A useful technique for displaying only the true shock is to use the value blanking feature to eliminate regions where this clutter appears. Use Tecplot 360’s Calculate dialog to calculate the Pressure Gradient Magnitude variable, then use the value blanking to blank the plot where this variable is less than some constant. A good value to use is , or for PLOT3D non-dimensional data, just 0.1.

To extract vortex cores, select Vortex Cores from the Feature drop-down, choose from the two available extraction methods, then click Extract. The cores consist of a group of line segments that may not all be connected. As a result, they are displayed using a line segment finite element zone. Display the Mesh or Edge plot layer to see the new zone.

If you are using value blanking, you may need to interpolate the blanking variable to the new zone. Refer to Data Interpolation for information on interpolation and Value Blanking for information on value blanking.

Due to the properties of the algorithm used, vortices that happen to exactly align with grid lines may not be properly extracted. This is unlikely to occur in real-world solutions, but is common in test data generated by extruding 2D solutions to produce artificial 3D solutions.

Separation and attachment lines show where a fluid flow separates from or reattaches to a no-slip wall boundary. These lines can give you an indication of where separation bubbles or recirculation regions appear in your data. To calculate them you must first identify one or more Wall boundaries using the Geometry and Boundaries dialog. (See Setting Geometry and Boundary Options.) The separation and attachment lines will be calculated on these boundaries.

Due to the algorithm used by the FX library to detect separation and attachment lines, these lines may not be detected for flows that are essentially two-dimensional. (That is, flows which contain no variation along one of the three spatial dimensions.)

To calculate separation and attachment lines, select this option in the Feature drop-down and click Extract. The lines, if any, will be displayed in new static zones, one zone for separations lines and a separate zone for attachment lines. As with vortex cores, the lines consist of sets of possibly unconnected line segments, which are displayed using line segment finite element zones. Display the Mesh or Edge layer to see the lines.

For vortex core and separation/attachment line calculations in ordered zones, you may choose to exclude blanked regions from the calculation. Select this option by selecting the Exclude Blanked Regions from Ordered Zones toggle. This will prevent lines from being calculated in regions of ordered zones that are not plotted due to blanking. Note, however, that this will invalidate the data journal. If you subsequently save a layout file, you will be prompted to save a new data file as well.