Getting Started Manual
Tecplot 360 2025 Release 2

Start Tecplot 360 from the Start menu (Windows), by typing tec360 in a terminal window (Linux), or by double-clicking the application icon in the Applications folder (Mac). The Tecplot 360 Welcome Screen appears, as shown here. (We will show the Windows version of Tecplot 360 in this document, but the product looks substantially the same on other platforms.)

The Welcome Screen appears each time you launch Tecplot 360 and gives you easy access to layouts you have recently worked with, along with quick links to documentation and other resources to help you get the most out of the product.

To begin loading the Onera M6 data, click Load Data at the top of the Welcome Screen. (You may also choose Load Data from the File drop-down menu in the menu bar, or click the folder icon, second from the left, in the toolbar. These alternate methods are convenient when the Welcome Screen isn’t visible.)

The Load Data dialog appears.

Navigate to your Tecplot 360 installation folder, then the examples folder, then the OneraM6wing folder. Then double-click the OneraM6_SU2_RANS.plt file to open it in Tecplot 360. (If you can’t see this file, choose All Files in the menu at the bottom of the dialog.) The data file is opened and a 3D plot of the Onera M6 wing appears in the Tecplot 360 workspace, as shown here.

To rotate the view of the wing, hold down the Control key on the keyboard (Command on Mac), then hold down the right mouse button in the Tecplot 360 workspace and move the mouse to rotate the wing.

You’ll notice that the range of rotation is not very great, making it hard to make significant changes to the view of the wing. This is because the rotation origin (the point around which rotation is performed) is not set anywhere near the wing. To change this, simply place the mouse pointer in the approximate center of the wing on the screen, then press the lowercase letter O (for origin) on the keyboard.

Then hold down the Control key (Command on Mac) and drag with the right mouse button again. You’ll see it is now much easier to rotate the wing, since it rotates around its center.

To see information about the Onera M6 data set, choose Data Set Info from the Data drop-down menu. The Data Set Information dialog, shown here, appears.

This dialog provides a wealth of information about the data set. The two lists at the top of the dialog show you the names of the zones and the variables in the data set.

The zones in this data set are:

You may wish to explore the other information in the dialog, which is divided into three pages. Click the Help button for more information about the information displayed on any page of the dialog. When you’re finished, close the Data Set Information dialog.

As you rotated the wing in step 2, you may have noticed a dashed orange line swoosh by in the plot. We have caught a glimpse of it here.

This is the bounding box of the FluidVolume zone, which represents the air around the wing. This zone does not have any style (that is, visual appearance) so it would normally be invisible. Tecplot 360 adds the dashed orange line so that you know it’s there and can see its dimension.

Choose Fit Everything from the View menu to see the full extent of the volume zone (see above). The wing is a tiny part of the data set! Choose View>Last to return to the previous view.

The bounding box does not add anything to the plot we’re making, so let’s turn it off. Choose Show Bounding Boxes for Enabled Volume Zones with No Style from the Options menu. The dashed orange line disappears.

To view the mesh for the WingSurface zone, right-click on the wing in the Tecplot 360 workspace. A context toolbar appears, as shown here.

From left to right on this toolbar are buttons that allow you to turn on and off the mesh, contours, vectors, shade, edge, and translucency. Click the first button to display the mesh for the WingSurface zone, as shown here.

The Color Chooser lets you choose a single solid color, or, using the 1-8 buttons at the bottom of the dialog, you may choose to have the mesh colored using a contour, such as a gradient based on the value of some variable. (These numbers actually refer to Tecplot 360’s eight contour groups, which associate variables and color maps. We will look at contours in more depth shortly.)

For now, let’s choose a blue color for the mesh.

Close the Zone Style dialog, so that the wing surface is visible again.

Scenic Detour: Context Menu and Toolbar

Try right-clicking the wing. A context menu and toolbar appears, allowing you to make many of the same changes you can make in the Zone Style dialog—without needing to pull up the dialog. Here we are using the drop-down menu to the right of the mesh icon (the first icon on the toolbar) to choose the mesh color.

If you are changing the styles of many zones at once, it still makes sense to pull up the Zone Style dialog. For many other situations, the context menu and toolbar are faster.

We will use this context menu again in later steps.

At the top of the dialog is a drop-down menu for choosing a variable. Next to this are eight numbered buttons, which specify the contour group you are editing. Each contour group has its own settings for this dialog. The contour group provides a way to associate a variable with a color map and other settings. The color map specifies how the zone will be colored according to the value of the specified variable.

For our tutorial, we will set up two contour groups. The first will display density with the Large Rainbow color map. The second will display the pressure coefficient using the Magma color map.

First, move the dialog so you can see most of the plot and the dialog at the same time.

The dialog should appear as shown above. You should have noticed the plot changing as you made each change in the dialog, since the wing surface is already using contour group 1 by default.

Next, we’ll set up contour group 2 for the Pressure_Coefficient variable.

The Contour & Multi-Coloring Details dialog should now appear as shown here.

Now that we’ve set up our contour groups, close the Contour & Multi-Coloring Details dialog. Ensure the Contour layer is checked on the Plot sidebar.

Now, we can change the contour variable displayed on the wing by right-clicking the wing, clicking the drop-down menu next to the contour icon in the context menu, and choosing contour group 2 C2: Pressure Coefficient.

The plot so far is shown below.

That contour legend is useful, but it overlaps our plot. Double-click the legend title to open the Legend page of the Contour & Multi-Coloring Details dialog, shown here.

This is the same dialog we just closed a moment ago, just a different page. You can also get to it by clicking the button next to Contour in the Plot sidebar, or by choosing Plot>Contour/Multi-Coloring from the Tecplot 360 menu bar.

In the Contour & Multi-Coloring Details dialog:

The desired settings are shown above. Close the dialog after changing these settings.

Using the mouse, you may now drag the legend to the bottom of the plot. The final plot is shown here.

A Tecplot 360 layout (.lay) file containing a snapshot of the final result of this tutorial segment is in OneraM6wing/finallayouts/ExtenalFlowVideo1.lay in the examples folder in your Tecplot 360 installation folder. You can compare this with your result to see how you did.

You might even try saving a layout of your own work. Choose File>Save Layout from the Tecplot 360 menu bar, then navigate to the folder in which you want to save the layout, name it, and click Save.

To move the slice with the mouse, first click the slice tool in the Plot sidebar, next to the Slices checkbox.

Then click the surface of the wing. (You probably can’t see the wing at first, with the slice in front of it, but you can still click it even though you can’t see it.) The slice moves to pass through the point that you clicked. You can see the slice at various positions in the following images.

You can also drag the mouse on the surface of the wing to fine-tune the slice location. A blue-gray preview plane shows where the slice will be when you release the mouse button.

Click the button next to the Slices in the Plot sidebar to launch the Slice Details dialog.

Let’s spend a moment on the Slice Details dialog.

You can leave the Slice Details dialog open while you experiment with dragging the slice around. Notice that the slice position field in the dialog updates as you move the slice in the plot. (Most dialogs in Tecplot 360 can be left open while you work, updating whenever you change a plot by other means.)

With the Slice Details dialog still open, let’s take a quick detour to the Contour page of this dialog, which allows you to specify how the slice itself will be colored.

This ties back to the contour groups we discussed in the previous segment of this tutorial (see Step 7: Set Up Contour Groups and Color Maps). As a refresher, a contour group ties a color map to a variable, thereby establishing how an object in your plot will be colored based on the values of the selected variable.

On the Contour page of the Slice Details dialog, we can choose the contour group to be used for the slice, which in turn determines the color map and the variable used for the contouring. Flooding best represents continuous values, so we’ll use the Flood By drop-down menu to choose the Pressure group.

If the variable we want to use isn’t listed on the Flood By drop-down menu, we’ll want to go to the Contour and Multi-Coloring Details dialog to set it up. Conveniently, that dialog can be accessed right from the Slice Details dialog by clicking the gear icon next to the Flood By drop-down menu. Try it now if you like, just to see it’s the same dialog, then close the Contour and Multi-Coloring Details dialog.

As shown here, we’ll contour our slice by Pressure, which is contour group 7.

Scenic Detour: Creating Multiple Slices

Slices are great, so let’s add more of them! We don’t need to do this for the plot we’re trying to make, which is why this section is labeled as a detour. You can skip it if you want.

Here’s what the Slice Details dialog should look at this point, along with the plot.

Streamtraces are a useful tool for visualizing the flow around a surface. We’ll try out three different types of streamtraces: volume lines, volume ribbons, and surface lines.

We only need a single slice for this, so if you followed the multiple-slice detour, go back to the Slice Details dialog, turn off Show Start/End Slices, and turn Show Primary Slice on.

We want our slice at the tip of the wing; that’s where the pressure differential can cause vortex shedding. Enter 1.18 for the primary slice’s location in the Slice Details dialog to place it close to the wing’s tip.

The Slice Details dialog should now look as shown here. You can close the dialog at this point, as we won’t need it for a while.

Now, rotate the wing so that the tip is pointing almost directly at us. (Hold Control, or Command on Mac, while dragging with the right mouse button.) The orientation axis in the upper right corner of the plot will help you get the wing pointed the right way. It should look roughly like the image below.

What are we looking at here? The green-blue background is our slice, and it’s hiding most of the wing at this point, so we only see the wing tip.

Last but not least, we can specify the vector variables that describe the velocity of the flow around the wing. If we don’t do it in advance, Tecplot 360 will prompt us to choose the variables as we begin adding our streamtraces. However, just so we know where the feature is, let’s do it ourselves now.

Choose Plot→Vector…​ from the menu bar or toggle on Vectors from the Plot sidebar. If you have not enabled vectors to this point, then the Select Variables dialog will appear. We actually don’t have velocity values in our data, but we do have momentum, and the vector field for momentum is the same as for velocity. (Momentum is just velocity times density. In the next segment of this tutorial, you’ll learn a technique you could use to calculate true velocity values.)

Therefore, for our purposes, we can use the momentum variables. So choose Momentum U, Momentum V, and Momentum W for the U, V, and W vector variables, respectively.

When the Select Variables dialog appears as shown here, click OK.

Turn on the Streamtraces checkbox in the Plot sidebar, then click the Streamtrace tool button .

You can now place a line with the mouse and seed streamtraces evenly along the line. To place the line, click and hold the mouse button at the starting point, drag to the end point, and release the mouse button. Try drawing a roughly vertical line along the leading edge of the wing, as shown here.

Tecplot 360 creates streamtraces showing the flow around the wing, as shown below. The streamtraces are generated by simulating the release of massless particles at the slice surface at equally-spaced points along the line (called "seeding") and calculating their path of travel based on the vector variables that describe the flow.

Some of the streamtraces are behind the slice. To see the streamtraces better, let’s change the slice to be 40% transparent. To do this, right-click the slice and choose 40 from the right-most drop down menu in the context toolbar.

Now, rotate the plot in three dimensions to better see the streamtraces and the wing. A possible result is shown below.

By default, streamtraces are simple lines with arrowheads. Ribbons can allow us to see the flow better because they show local twist using a 2D surface. Here’s how to switch to volume ribbons.

The plot should look something like this with the ribbons.

Let’s change them from white to a more attention-grabbing color. We can do this on the Rod/Ribbon page of the Streamtrace Details dialog.

Near the bottom of this dialog, under the Show Shade checkbox, click the button next to Color. Then, in the Color Chooser, click the red swatch.

The plot with red ribbons is shown below:

You can adjust the direction of the lighting to make the ribbons stand out more. To do this, click the sun toolbar icon in the Plot sidebar.

Click or drag around the plot to move the light. As you do so, you will find spots where the ribbons catch a highlight. You can also try rotating the plot to get the best view.

So far, we’ve been looking at flow through the air around the wing: volume streamtraces and ribbons. We can also visualize the flow across the surface of the wing.

Just to be clear, these streamtraces will be calculated using the momentum data from the volume zone around the wing. The wing surface zone does not actually contain momentum or velocity data. The data file we provide for this tutorial has the zones set up to make this work correctly.

We used the slice to specify a plane on which we could draw a line to seed streamtraces in a volume. When creating surface streamtraces, we just seed directly on the surface. So click the Slices checkbox in the Plot sidebar to turn off the slice.

Next, let’s delete the ribbons we’ve created by clicking Delete All on the Placement page of the Streamtrace Details dialog. Then choose "Surface Line" at the top of the dialog.

Let’s rotate the wing again so that we can see across it. (Last reminder: hold Control, or Command on Mac, while dragging with the right mouse button.) We’re going for an angle something like this.

As always, you can use the orientation axis in the upper right corner of the plot to help you stay oriented.

Now, just as we did before when seeding from the surface of our slice, we choose the streamtrace tool in the Plot sidebar, then drag a line across the wing surface, parallel to the leading edge. After Tecplot 360 creates the streamtraces, we end up with something like this.

We made our streamlines thicker so you can see them more easily. For extra credit, figure out how to make yours thicker, too. (The setting you need is on the Lines page of the Streamtrace Details dialog.)

We’re done with streamtraces for now. Turn off the Streamtraces checkbox in the Plot sidebar when you’re done to hide the streamtraces and show just the wing.

Iso-surfaces are great way to visualize a constant value of a contour variable as a surface. In other words, you specify a value, and the iso-surface shows you where the specified variable has that value.

Let’s use it to visualize the shockwave as the wing passes the speed of sound. We do this by creating an iso-surface at Mach 1.

The plot is shown here. We’ve rotated the wing to get a better view.

This iso-surface shows us where the air is moving at Mach 1 around the wing. Try adjusting the Value 1 field using the arrows next to the numeric entry field and watch the plot change in response.

It is often instructive to show more than one iso-surface at more than one value. Let’s add a second iso-surface at Mach 1.2. To do this, change the Draw Iso-Surfaces At menu to 2 Specified Values and enter 1.2 in the Value 2 field.

The dialog options are shown here.

Where’s the second iso-surface? Well, it’s closer to the wing than the first one, so it is hidden. Let’s make the iso-surfaces partly transparent so we can see the second one inside the first (and also, dimly, the wing surface inside the second).

To do this, right-click the iso-surface in the plot, then turn on transparency by clicking the rightmost icon in the toolbar. Our iso-surfaces are both in the same group, so they both become transparent.

Now you can see the Mach 1.2 iso-surface inside the Mach 1 iso-surface. Rotate the plot and see! This is the shock surface where the transition between subsonic and supersonic is happening. Here’s our final iso-surface plot.

The last exploration technique we’ll explore is probing. Probing shows the values of all variables at a location you click in the plot. Simply choose the Probe tool from the toolbar at the top of the screen.

Now, click points of interest in your plot. The Probe sidebar, which pops out along the right edge of the screen, displays the variable values at each clicked location.

You can also copy variable names, values, or both from the probe results by selecting the desired information and right-clicking, or by pressing Control-C (Command-C on Mac OS X).

As with any sidebar, you can move the Probe sidebar to another edge of the workspace, combine it with another sidebar, or even tear it off and move it outside the main Tecplot 360 window—to a different monitor, if you want.

As before, a Tecplot 360 layout (.lay) file containing a snapshot of the final result of this tutorial segment is in OneraM6wing/finallayouts/ExtenalFlowVideo2.lay in the examples folder in your Tecplot 360 installation folder.

We’ll be continuing from where we left off with segment 1 of this tutorial, not from segment 2. Load the layout OneraM6wing/finallayouts/ExtenalFlowVideo1.lay in the examples folder in your Tecplot 360 installation folder and follow along.

Choose File→Load Data from the Tecplot 360 menu, then open the experimental data file. This is a Tecplot ASCII file named Onera_Experimental.dat and can be found OneraM6wing folder in your Tecplot 360 examples directory. (If you can’t see this file, choose All Files in the menu at the bottom of the dialog.) The experimental data file we’ve included is a slightly modified version of data provided by NASA. For more information, see turbmodels.larc.nasa.gov/onerawingnumerics_val.html.

If you used All Files, the Choose Loader dialog appears after you select the file to ask what format the data is in.

Choose Tecplot Data Loader and click OK.

Next, Tecplot 360 asks whether you want the new data to replace the existing data, or to append the new data.

In the Load File(s) dialog, click Append data to active frame.

The Variable Load and Combine dialog should appear after appending the data. This dialog gives the user options to combine certain variables as well as the option to not add certain variables. Variables that are automatically combined are colored blue. Manually combined variables are colored green. Anything else is colored black. Notice that Pressure_Coefficient has been automatically combined.

For this example, we will load all of the variables from the Experimental dataset. Select Add All and then select OK to close the Variable Load and Combine dialog.

To verify that the data was loaded correctly, open the Data Set Information dialog by choosing Data→Data Set Info from the menu. Notice the seven new zones: Section 1 - 0.2, Section 2 -0.44, and so on. These zones contain the experimental data from the pressure taps placed along the wing.

You’ll also notice several new variables, starting at variable #19: TapNumber, X/L, Y/b, Z/L, and Cp Error.

We want to compare the experimental data with our simulation data at a pressure tap location. However, the experimental data is, as we mentioned, normalized: instead of using a Y that ranges from 0 to the span length, as in the simulation data, it uses a Y over b (Y/b) that ranges from 0 to 1.

If we open the Data Spreadsheet dialog (Data→Spreadsheet), choose our WingSurface zone, and scroll over to see the "Y/b" variable, we can see that our simulation data does not contain this information. It is only in the experimental data set.

However, if you use the Zone menu to switch to one of the experimental data zones, such as Section 1 - 0.2, you will see that it has values for this variable.

Therefore, we will need to calculate this variable for our simulation data. We can do this using an equation.

Close the Data Spreadsheet dialog, then open the Specify Equations dialog by choosing Data→Alter→Specify Equations. We know that the span of the wing, b, is 1.19 from publicly-available information about the Onera M6 model. So, in the Equation(s) field, enter:

We only want to calculate this variable in our simulation zones, since it already exists in our experimental zones, so make sure only FluidVolume and WingSurface are selected in the Zones to Alter list. (Hold down the Control key, or Command on Mac, while clicking zones to toggle them on and off.) The Specify Equations dialog should appear as shown below.

Click Compute to calculate the Y/b value for our simulation zones.

Finally, let’s check our work by probing at the wing tip.

We should expect a value of 1 for Y/b. However, since the wing tip is beveled, the Y/b value will actually be slightly greater than 1. Everything is exactly as it should be. Mission accomplished!

Let’s go ahead and change the Y axis to Y/b. Choose Plot→Assign XYZ from the Tecplot 360 menu bar. Then, in the Select Variables dialog, choose "Y/b" for the Y-axis variable, as shown here. Click OK. to save this change.

The wing may rotate in the workspace when you change the Y variable. This is normal.

Our experimental data contains information only at the locations of the pressure taps on the wing. For this example, we’ll compare the simulation data with the experimental data from the pressure tap at Y/b = 0.65. We will create a slice of the simulation at this location and extract that slice to a new zone.

All the simulated surface data along the wing at the location of the pressure tap, in other words, will be copied into a new two-dimensional zone. Here’s how.

Our new slice zone is zone 10 and is named "Slice Y=0.65." You can verify this in Data Set Information, if you like.

Now we can normalize the X dimension of our slice to the chord, in order to match the experimental data. We’ll do this using the same Specify Equations dialog we used to normalize the Y dimension. In the experimental data, this is stored as the variable X/L. (If you’re curious, you can verify this in the Data Spreadsheet dialog, as we did previously with Y/b.)

The equation we’ll need is:

There’s a twist that we need to address before we actually perform this calculation. The equation uses the MAXX and MINX intrinsic variables. These variables are provided by Tecplot 360 and refer to the maximum and minimum values of X in all active zones. We want the maximum and minimum X for just our slice, so as to calculate the chord, so we need to temporarily deactivate all other zones while we perform this calculation.

So open the Zone Style dialog by clicking the Zone Style button in the Plot sidebar.

Right-click the Show Zone checkbox for the extracted slice zone and choose Show Selected Only.

The checkboxes next to all zones except the slice zone toggle off. Your plot also disappears; don’t panic!

Now, choose Data→Alter→Specify Equations and enter our equation in the Equation(s) field. For convenience, here it is again:

Since we need this calculation only for the slice, make sure our new slice zone, listed at the bottom of the Zones To Alter list as "10: Slice Y=0.65" is the only zone selected.

Now you’re ready to click Compute.

After the calculation is complete, go back to the Zone Style dialog and turn the disabled zones back on by selecting all rows (Control-A, or Command-A on Mac, is a handy keyboard shortcut for this), then toggling on the Show checkboxes for any disabled zone. This toggles on all selected zones.

You can now close both the Zone Style and Specify Equations dialogs.

We’re ready to create an XY plot of the slice. We’ll put it in its own frame: frames are the Tecplot 360 way of showing multiple plots on a page.

First, click the frame tool in the Tecplot 360 toolbar.

Next, use it to draw the new frame in the workspace. The placement and size don’t matter, since we’ll have Tecplot 360 set it up nicely for us in a moment. Click and hold the mouse button somewhere in your plot, then drag down and to the right to create the frame. Release the mouse button when a rectangle is visible in the plot.

The new frame might look something like this.

Next, choose Frame→Tile Frames in the Tecplot 360 menu bar. The Tile dialog appears, as shown here.

Click the bottom right button in the Tile Frames dialog to stack the frames on top of each other in the workspace. Then close the Tile dialog.

Your plot now looks something like this.

Now, using the drop-down menu at the top of the Plot sidebar, change from Sketch to XY Line.

The Create Mappings dialog appears. In this dialog, we’ll set the X-Axis to our X/L variable, our Y-Axis to Pressure_Coefficient, and the Zone to our extracted slice zone. The desired settings are shown here.

Click OK to create the plot, which is shown here.

If you’re familiar with Cp plots, you’ll notice something odd about our current plot! The problem is that the Y axis is reversed from what it should be. Fortunately, this is easily corrected.

Our plot now looks like this. Much better.

We’re in the home stretch now! Let’s add the experimental data to our plot. First, open the Mapping Style dialog by clicking the Mapping Style button in the Plot sidebar.

A line map is the Tecplot 360 way of associating (mapping) a variable with a visual style for each line in your plot. Tecplot 360 created our first line map for us when we switched to XY Line mode. The Mapping Style dialog is used to manage the line maps in our XY Line plot.

We want to show both the simulation and experimental data in our plot, so we’ll need to create a second line map for the experimental data. The easiest way to do this is to copy the existing simulation data line map and modify it to display the experimental data.

The Mapping Style dialog and the plot should now appear as shown here.

As you can see, there’s a slight problem here: both the simulation and the experimental data have the same appearance, making it impossible to distinguish them. We can address this by using different colors for the two zones.

Additionally, the simulation data is continuous, while the experimental data, having been measured at specific points along the wing, is discrete. Therefore, we will display the experimental data using a symbol at each measurement location rather than as a line.

Finally, we have uncertainty information for the experimental data, which we can display using error bars.

All of these appearance changes can be managed using the Mapping Style dialog. Let’s get to it.

Scenic Detour: Line Map Context Menu and Toolbar

Earlier in this tutorial sequence, we suggested you right-click on your 3D plot to discover a quick way to make changes to your zone style—without a trip to the Zone Style dialog. Try right-clicking on a line in your plot to reveal the line map context menu and toolbar (shown at right). Then try to do the next step, adding error bars, using the context menu rather than the Mapping Style dialog.

The experimental data includes an error variable calculated from data NASA provides about the Onera M6 wing, namely that the measurement error for the pressure taps was found to be ±0.02. Let’s add error bars to the plot to visualize this information.

The Error Bars page should now look as follows.

You can now close the Mapping Style dialog. The plot should look as follows.

As a finishing touch, we can add a legend to the plot. Choose Plot→Line Legend from the Tecplot 360 menu to open the Legend dialog, then toggle on the Show Line Legend checkbox.

Let’s also choose View→Nice Fit to Full Size to make the plot look a little less crowded against the axes.

The final plot (including both frames) is shown below.

Naturally, a Tecplot 360 layout package (.lpk) file containing a snapshot of the final result of this tutorial segment is in OneraM6wing/finallayouts/ExtenalFlowVideo3.lpk in the examples folder in your Tecplot 360 installation folder.

Start Tecplot 360 from the Start menu (Windows), by typing tec360 in a terminal window (Linux), or by double-clicking the application icon in the Applications folder (Mac). We will show the Windows version of Tecplot 360 in this document, but the product looks substantially the same on other platforms.

To begin loading the surface plot data, click Load Data at the top of the Welcome Screen. (You may also choose Load Data from the File drop-down menu in the menu bar, or click the folder icon, second from the left, in the toolbar. These other methods are convenient when the Welcome Screen isn’t visible.)

The Load Data dialog appears.

Navigate to the examples/SimpleData directory located in the installation folder of Tecplot and select the DuctFlow.plt file. After opening this file, you’ll see a 3D Cartesian plot like the one below.

Currently we are looking at an empty box surrounded by orange dashed lines. These lines represent the boundary of the volume zones with no style applied. To understand what we are looking at, let’s look at the Surface tab of the Zone Style dialog:

For performance reasons, the default option for Surfaces to Plot is set to "none" on volume zones. When you have a volume zone where you’d like to see the surface data then change this option. Note that if surface zones are in the dataset, they would be shown in the Zone Style dialog as "N/A".

Now let’s turn on Contour from the Plot sidebar. To show contours, however, Tecplot 360 must represent this on some sort of surface. Since this data only contains volume zones, a Question dialog appears asking to display the surfaces of volume zones. Alternatively, enabling the mesh, contour, shade, vector or scatter layer option on the plot sidebar will ask you if you want surfaces turned on for active zones.

Turning on the surfaces of volume zones can be a resource-heavy operation as it requires loading the entire volume zone and calculating which cells represent the outer surface.

Clicking Yes on the Question dialog allows Tecplot 360 to change the Surfaces to Plot option in the Zone Style dialog. The volume surfaces will now be contoured by the first variable that is not an axis variable.

If the Zone Style dialog was closed previously, open it again by clicking the Zone Style dialog in the Plot sidebar.

Navigating to the Surfaces tab, you’ll see that the Surfaces to Plot heading has changed to Boundary cell faces which allows us to see the contour of surfaces of exposed boundary cells.

The resulting plot should look similar to what is shown below. Since we did not change the Contour variable, the plot is displaying the U Vector variable.

Start Tecplot 360 from the Start menu (Windows), by typing tec360 in a terminal window (Linux), or by double-clicking the application icon in the Applications folder (Mac). We will show the Windows version of Tecplot 360 in this document, but the product looks substantially the same on other platforms.

To begin loading the wind turbine data, click Load Data at the top of the Welcome Screen. (You may also choose Load Data from the File drop-down menu in the menu bar, or click the folder icon, second from the left, in the toolbar. These other methods are convenient when the Welcome Screen isn’t visible.) The Load Data dialog appears.

Navigate to the windturbineblades folder where you extracted the data files. Select all the files in this directory, for example by clicking the first one and then clicking the last one while holding the Shift key, then click Open. (If you can’t see the files, choose All Supported Files in the menu at the bottom of the dialog.)

Opening all these data files will take a moment; when Tecplot 360 is finished, you’ll see a 2D Cartesian plot like the one below.

What exactly are we looking at here? This is the full 2D fluid domain, representing the wind turbine’s blades and the air surrounding them. Let’s get a better view:

So we can see this is a cross-section of a three-bladed vertical wind turbine. The white areas are the blades, as you can intuit from their airfoil shape. You can even infer the direction of rotation: counterclockwise.

Let’s take a closer look at the data we’ve loaded. Choose Data Set Info from the Tecplot 360 Data menu to open the Data Set Information dialog, shown here.

From here, we can see that there are more than a thousand zones in this data set. Each zone represents a region of the simulation at a particular point in time.

The number of zones may seem like a lot if you’re not used to working with transient data, but if you do the math, this is only nine zones per time step. And indeed, if you look at the zone list here, you can see that the zone names repeat every nine entries: zone 1 and zone 10 are both named dom-1, zone 2 and zone 11 are both named dom-5, and so on.

So we have:

If you click through the zones while keeping an eye on the Time Strand field in the panel below the zone list, you will discover that the zones that have the same names also have the same time strand. Time strands are how Tecplot 360 links the zones representing the same region throughout time.

You can also see the solution time of each zone above the time strand as you click on in the zone list. As you would expect, zones 1-9 have the same solution time, as do zone 10-18, and so forth. Thus, each set of nine zones represents the same point in time.

Let’s close the Data Set Information dialog and open the Zone Style dialog (below) by clicking the Zone Style button in the Plot sidebar.