Getting Started Manual
Tecplot 360 2024 Release 1

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→Variables from the menu bar. The Select Variables dialog appears. 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, as shown here.

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.

Here you’ll see nine entries: one for each time strand. (The asterisk next to each zone number indicates that it’s not a single zone, but a group of zones having the same time strand.) In this way, the Zone Style dialog lets you make changes to the "same zone" throughout time all at once, as you’ll usually want to do, instead of having to make those changes separately at each time step. So although there are technically hundreds of zones in the data, Tecplot 360 lets you style them as though there were only nine.

We’re done with the Zone Style dialog, so close it.

Right-click the plot to display the context toolbar and menu, as shown here. These allow you to make changes to the selected zone.

From left to right, the icons are Mesh, Contour, Vector, Shade, and Edge. Click the first icon to turn off the Mesh layer, then the second icon to turn on the Contour layer. (You can do this in the Plot sidebar if you prefer.

Now your screen should be showing you something like the plot below.

Tecplot 360 can help visualize the flow through the wind turbine by adding streamtraces. In the Plot sidebar, turn on the Streamtraces checkbox.

The Select Variables dialog appears to choose the variables that represent velocity through the fluid; the defaults that Tecplot 360 has chosen are correct, so just click OK.

After you’ve accepted the vector variables, choose the streamtrace tool in the main toolbar, or in the Plot sidebar next to the Streamtraces checkbox.

You are now ready to add streamtraces to your plot, a process called seeding. It is convenient to seed a number of equally-spaced points along a line, which is referred to as a rake.

To do this, click in the plot near the top blade of the turbine, then hold the mouse button while dragging down between the two lower blades. Tecplot 360 seeds ten streamtraces at equally-spaced points along the line you placed Tecplot 360 calculates the path of a massless particle forward and backward from each seeded point and draws the path on the plot.

You may seed additional streamtraces by placing additional rakes in the same way, or seed individual points by clicking. A Tecplot 360 layout (.lay) file containing a snapshot of the final result of this tutorial segment is in WindTurbineBlades/FinalLayouts/transient_1.lay in the Getting Started bundle.

Click the Play button in the Plot sidebar to see how pressure and fluid flow change as the wind turbine blades rotate. (Just as we deduced earlier from the blade shape, the turbine turns counterclockwise.)

Scenic Detour: Animation Speed

The animation speed can be limited in the Time Animation Details dialog, which can be reached by clicking the button next to the animation controls in the Plot sidebar.

The maximum animation speed is limited by the speed at which Tecplot 360 can draw an individual frame, which depends a lot on how fast your computer is and how much of the data has already been loaded into memory. However, you can keep animations from going too fast by clicking the Limit Animation Speed checkbox and entering the desired number of frames per second.

To draw the line along which we will extract the pressure data, first click the polyline geometry tool in the Tecplot 360 toolbar. A geometry is a shape that appears on your plot. This particular geometry tool can be used to create both lines and polygons, hence the name polyline.

The line we want to draw is in roughly the same place as the rake we placed for creating streamtraces in the previous lesson. But the polyline tool, since it can be used to create both simple lines and more complex shapes, works differently from that tool.

To place the line:

The line should look roughly like this on the plot. We have made our line thicker so you can see it better. You don’t have to do the same, but if you have a moment, see if you can figure out how.

Let’s see how pressure changes along our line over time by creating an animated plot of the Y coordinate vs. pressure. To do that, choose Extract Polyline Over Time from the Extract submenu of the Data menu.

You will be asked for the number of points to be extracted along that line. The default value, which should be 100, is fine.

Tecplot 360 will take just a moment to go through all the time steps and extract the data along this line. You can open the Data Set Information dialog and see a new zone for each time step, named "Extracted Points," that were created beginning with zone number 1144 and ending with zone number 1270.

Each new zone is assigned the correct solution time and given a time strand to connect it to the others, just as we saw when we inspected the data in our file earlier.

That’s 127 new zones in all, which matches the number of time steps in the file. All of these new zones are assigned to time strand 10, which makes sense because, previously, there were nine variables per time step and thus nine time strands. You can also see that each of the new zones has the same variable names as the previously-existing zones.

So, as we expect, we have extracted the data along the line over time.

Let’s see what the pressure looks like along our extraction line by creating a line plot. We can display this line plot side-by-side with the contour plot and even animate them together.

First, choose the New Frame tool in the Tecplot 360 toolbar. Then hold the mouse button down and drag out a rectangle on the plot. It doesn’t matter where; we will resize and reposition it in the next step.

Your new frame might look something like this.

Let’s get that new frame into position. Choose Tile Frames from the Frame menu, then click the bottom-right button.

This will stretch both frames to the width of the workspace and position them one above the other, as seen here.

Let’s go ahead and zoom out that top frame a bit and reposition it so that we can see the whole wind turbine. To do this, we will use the Zoom and Translate tools in the toolbar.

The top frame should look more like this now.

Now we’ll turn our attention to the bottom frame, where we’ll create a line plot of pressure along the line we placed on the plot earlier.

The plot in the bottom frame should now look a lot like this.

If you try animating the plot by pressing the Play button on the Plot sidebar, you will notice that only the active frame animates. To get both frames animating together, we will link them so they always display the same time step.

To do this, choose Frame Linking from the Frame menu to open the Set Links for Active Frame dialog.

On the Between Frames page, mark the Solution Time checkbox, then click the Apply Settings to All Frames of this Group button. Close the dialog and try animating again!

Scenic Detour: Add Solution Time Caption

It would be nice to be able to see what the solution time is right on the plot, without having to look at the Plot sidebar. This might be of particular utility if you were exporting a video. To do this:

Animate again and watch the solution time change!

We have seen how to create a line plot showing the pressure along a line at each time step. Using animation, we can show how that changes over time. Now we’ll reduce the dimensionality even further by creating a single line plot showing how pressure varies at a single point.

To create this time series plot, choose Probe to Create Time Series Plot from the Tools menu, then click as close to 0, 0 as you can get on the contour plot (top frame). Hint: the X and Y coordinates of the mouse cursor are displayed in the bottom right corner of the Tecplot 360 workspace.

After you click, Tecplot 360 spends a moment gathering the pressure value for that point for all time steps, then displays the time series plot in a new frame overlapping the contour plot.

When you animate, a moving vertical line appears in this plot to indicate the current time step.

All three plots (the contour plot, the pressure line plot, and the time series plot) animate at the same time.

Try using the Tile Frames tool we used earlier to find a good arrangement for your three frames. You’ll probably need to re-position and zoom out on the contour plot again.

Select the bottom frame (containing the time series plot) with the selector (arrow) tool, then choose Fourier Transform from the Data menu. The Discrete Fourier Transform dialog, shown here, appears.

In this dialog, choose Pressure as the dependent variable and make sure the Time Series Plot Zone is selected as the source zone. Using the Plot Placement drop-down menu, choose to tile the new frame with existing frames. Leave everything else the same. Click Transform to perform the Fourier transform.

A new frame appears, showing Frequency (Solution Time)^-1 on the X axis and Amplitude (Pressure) on the Y axis.

Looking at this plot, we can easily see that there is a low-frequency spike at around 5 Hz and a higher-frequency spike at about 77 Hz. This matches what we see in the time series plot: a lower-frequency (high-period) wave overlaid by a higher-frequency (low-period) wave. The combination makes the time series plot look a little jagged.

From watching the animation, we can attribute the lower-frequency pressure changes to the movement of the blades. However, we don’t have an obvious explanation for the higher-frequency changes.

Before going further, let’s have a quick look at what the Fourier Transform actually did to our data set by popping into Data Set Information (choose Data Set Info from the Data menu). Make sure that the Fourier plot frame is selected.

As you can see, Tecplot 360 has created a new Fourier Transform zone based on the Time Series Plot and added three new variables starting with variable 37. (The other zone and the first 36 variables were created when we generated the time series plot.)

The new variables are the frequency, amplitude, and phase output from the Fourier transform. We only selected Pressure as our dependent variable in the transform, but if we had selected more, there would be three new variables for each one we selected.

Let’s see if we can find out what’s causing the higher-frequency changes. To do this, we’ll re-probe well outside the turbine, near the left inlet. Then we’ll create a new time series plot and re-do the Fourier transform.

Zoom out the contour plot so that you see most or all of the fluid domain surrounding the turbine. The blades will be very small in the center of the plot. At right you’ll see we’ve zoomed all the way out. The mouse pointer is placed roughly where we’ll be probing.

Now choose Probe to Create Time Series Plot from the Tools menu again, and click close to the indicated position on the plot. A new time series plot is created.

Right away, you can see that this plot has less obvious order in it.

Since our Fourier transform plot was calculated from the data in the old time series plot, it disappears. But we can re-create it easily. Simply right-click the line in the time series plot to display the context menu and toolbar. Then choose Fourier Transform from the menu.

A new Fourier transform plot is created using the options previously set in the Discrete Fourier Transform dialog. It looks something like the plot below.

Here, the main frequency is the one we previously saw at around 77 Hz. The lower frequency around 5 Hz is no longer there, indicating that we are probing far enough away to avoid the effects of the turbine blades. We can conclude that the 77 Hz frequency is an input boundary condition.

A Tecplot 360 layout (.lay) file containing a snapshot of the final result of this tutorial segment is in WindTurbineBlades/FinalLayouts/transient_2.lay in the Getting Started bundle.

Your Turn

Try analyzing other variables, such as Turbulent Viscosity. By probing near where vortices are shed, you can see how changes in turbulent viscosity are solely due to the motion of the turbine blades. We will delve into this in more detail in the next exercise.

Before we can calculate the new variable, we must make sure that the baseline variables are assigned in the Field Variables dialog. To open this dialog, choose Field Variables from the Analyze menu.

Tecplot 360 has chosen defaults that match what it thinks you want to do:

For this data set, these defaults are correct, so you can just click OK. For other data sets, you may need to choose different variables.

To calculate vorticity magnitude, just choose Calculate Variables from the Analyze menu. This displays the Calculate dialog.

Click the Select button to choose the variable to be calculated. This displays the Select Function dialog.

As you can see, there are literally dozens of variables that Tecplot 360 can calculate for you. Choose Vorticity Magnitude in the list then click OK to return to the Calculate dialog. The default options in the Calculate dialog are acceptable (note that the Calculate on Demand checkbox is checked!) so go ahead and click Calculate.

Tecplot 360 sets up calculate-on-demand for Vorticity Magnitude and adds the variable to the data set, and tells us that’s what it has done via an alert.

We can now close the Calculate dialog.

To actually show our newly-calculated variable on our plot, open the Contour Details dialog by clicking the button next to the Contours checkbox in the Plot sidebar.

The Contour Details dialog appears.

In the Contour Details dialog:

In the Enter Contour Levels dialog:

When the dialog is as shown, click OK.

You may now move the Contour Details dialog to the side to get a good look at the plot. However, leave it open; we will have need for it again soon.

The contour plot should now look something like this.

This plot is good, but we can make it better by only coloring areas with vorticity above a critical value, improving the impact of locations of higher vorticity.

Back in the Contour Details dialog, set the contours to cut off below a value of 7. This field is in the lower right portion of the dialog.

This makes our vortices stand out by eliminating all contouring below 7. You might experiment with slightly lower and higher values to see more or less. Now we must remove the legend as it is overlapping a region of interest on our plot.

One last trip to the Contour Details dialog. Switch to the dialog’s Legend page, change the alignment to horizontal, and activate the Resize Automatically checkbox.

You can close the Contour Details dialog. Switch to the Selector arrow tool, select the legend by clicking on the box around it, and drag the legend to the top center of the plot.

Using the translation tool in the toolbar, move the wind turbine blades a little to the left, so we can see more of the vortices being shed.

You can see our final vorticity plot below.

A Tecplot 360 layout (.lay) file containing a snapshot of the final result of this tutorial segment is in WindTurbineBlades/FinalLayouts/transient_3.lay in the Getting Started bundle.

Click the Play button in the Plot sidebar to begin animating the plot.

You’ll notice that the first time through, the animation is a little slow. This is because Vorticity Magnitude is a calculate-on-demand variable, as we discussed earlier. It takes a moment to calculate this variable the first time each time step is plotted.

After the first time through, the animation will repeat. Since the Vorticity Magnitude variable has already been calculated for each time step, it does not need to be calculated again, and the animation moves much more quickly and smoothly the second and subsequent times through.

To begin loading the connecting rod data, select 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 downloaded and extracted ConnectingRod folder, open the menu on the bottom right of the dialog, and select All Supported Files. Load the D3PLOT file.

Your loaded data only shows an orange dotted box, select Contour on the Plot sidebar, select Yes on the question dialog that appears, and your plot should look similar to the above picture. Refer to Understanding Volume Surfaces to learn about the Surfaces to Plot option.

Press the play button, , on the plot sidebar and notice the machine parts in motion. If the animation is too fast, press the button above the animation slider and select the checkbox next to Limit animation speed to, limiting the animation to 12 frames per second.

The resulting animation is now slower the next time the play button is pressed. Close the Time Animation Details window.

Open the Data Set Information window by selecting Data>Data Set Info…​ and notice how the data is configured. Each Zone pertains to a different time step and has the same variables. In the variables box, notice that the stress components for each direction are included in the dataset (variables 10-15) thus allowing the ability to calculate the Von Mises stress.

Next, select Tools>FEA Post-Processing to open the FEA Post-Processing Window. Under the Derive Variables section derive "Von Mises Stress/Strain" from "Stress" (the Stress variables shown below). Click Add to Data Set. Now on the Data Set Information page, Von Mises Stress appears as variable 33. Close the FEA Post-Processing dialog and close the Data Set Information dialog.

To begin contouring, select the button next to the Contour checkbox on the plot sidebar to open the Contour & Multi-Coloring Details dialog. Currently, X Acceleration is the contour variable of the first contour group. Change the contour group variable to Von Mises Stress by selecting the drop-down box at the top of the dialog.

Tecplot 360 allows up to eight contour groups, each with their own contour variable and levels. This allows multiple contour surfaces to be plotted at the same time. In this tutorial, only one contour surface needs to be plotted.

Next, select the Set Levels…​ button and change the minimum level to be 0, maximum level to be 900, and the number of levels to be 21. The resulting Enter Contour Levels dialog should look like the picture below. Select OK and Close the Contour & Multi-Coloring Details dialog for now.

Currently, the crankshaft and cylinder are in the way of viewing the connecting rod. Since the data set consists of one zone and many time steps, Value Blanking will allow the connecting rod to be seen more clearly. Select Plot>Blanking>Value Blanking from the toolbar to open the Value Blanking window. Under the Blank when section change the blanking constraints to be when Von Mises Stress is equal to 0. Select both the Include Value Blanking checkbox as well as the Active checkbox to enable the current blanking constraint. Now only the connecting rod is shown. Close the Value Blanking dialog.

The resulting plot isolates the connecting rod because the Von Mises stress contour values are equal to zero on the crankshaft and cylinder. Though the parts still exist in the data set, they do not give helpful information. In the Value Blanking dialog, multiple constraints can be enabled at once to confine the plot view to very specific areas. For this situation, only one constraint was needed.

When clicking the play button again, the Von Mises Stress ranges between 0 and 900 at different steps in the cycle. The values of interest are when the Von Mises Stress exceeds 800. This is the critical failure threshold. To highlight the critical failure threshold, turn on Color Cutoff located in the Contour & Multi-Coloring Details dialog and cutoff below 800.

Close the Contour & Multi-Coloring Details dialog.

Now when playing the animation, there are two steps that are above the critical failure threshold. Turning on translucency by the checkbox on the plot sidebar can give a better view of the part.

Visualization can be further improved by selecting the 3D Multi Frames option. Select Frame>3D Multi Frames then select the top left option and three extra frames will appear. These frames are extra orthographic projections of the connecting rod and are created automatically. Notice when the play button is pressed again, the frames are automatically linked to each other and all frames animate together.

A Tecplot 360 layout (.lay) file containing a snapshot of the final result of this tutorial segment is in ConnectingRod/FinalLayouts/connecting_rod_1.lay in the Getting Started bundle.

Select Data>Alter>Specify Equations from the menu bar to launch the Specify Equations dialog. Type the following equation into the text field: {maxStress} = IF ({Von Mises Stress}>800, 0, 1).

Press the Compute button at the bottom and an Information popup will appear, "Data alteration successful." Click OK and close the Specify Equations dialog.

Open the Contour & Multi-Coloring Details dialog again by selecting the button next to Contour on the plot sidebar. Change the contour variable to be the variable just created, maxStress. Check that the Contour settings looks similar to the image below. Remember to remove the color cutoff if it was set in the previous section.

If your data does not contain the amount of contour levels as the above picture, select the Set Levels button. This will bring up the Enter Contour Levels dialog. Set the Level Creation mode to "Exact Levels" and set the minimum, maximum, and delta to 0.05, 0.95, and 0.05, respectively. See Step 4: Contour by Von Mises Stress for more information.

Now the regions where the threshold of 800, specified in the if statement, are revealed. However, Tecplot 360 is not only plotting 0 and 1, as expected. By default, Tecplot 360 will interpolate values between cell values. Close the Contour & Multi-Coloring Details dialog.

To minimize interpolation by contouring, open the Zone Style dialog located on the plot sidebar. Select the Contour tab and set the Contour Type to "Primary value flood".

Close the Zone Style dialog and notice that the resulting plot contains only yellow and blue. The blue cells occur when the Von Mises stress threshold is met or being exceeded.

If you are continuing from the previous section, return the Contour variable back to Von Mises Stress (see Step 4: Contour by Von Mises Stress for more information). Then, click Scripting>Play Macro/Script…​ and the Open Macro dialog will appear. Navigate to the connecting rod folder again and select PlotMaxContourOverTime.mcr.

After selecting Open, the macro will automatically run, creating an XY plot of the maximum value of Von Mises stress at each time step. When the play button is pressed, a marker line follows over the XY plot to track the solution time.

A Tecplot 360 layout (.lay) file containing a snapshot of the final result of this tutorial segment is in ConnectingRod/FinalLayouts/connecting_rod_2.lay in the Getting Started bundle.

This first portion of the macro file takes the first contour variable and finds its name. Then, the macro finds the number of time steps in the transient data and creates a zone.

To begin, the first two extended commands in conjunction get the variable name by extracting the variable number by the variable defined in Contour Group 1, then using that to extract the name. The script will then use this as part of the new zones name.

The script then determines the number of time steps using the QUERY.NUMTIMESTEPS which is then used to create an I-ordered zone (rectangular zone where J = K = 1) dimensioned by the number of time steps.

Using the $!VARSET command, a new internal macro variable is created based on the total number of zones. Since the new zone is the last zone created, its index is equal to the maximum number of zones. Then the zone is renamed using the Contour variable name found earlier.

The next step is to populate the zone created in step 2 with the maximum value of Von Mises Stress. The key to this process is using the |MAXC| intrinsic variable which returns the maximum value of the currently active zones.

This portion of the macro loops through all time steps activating the current time step though SET.CURTIMESTEP which ensure that only the zone in current time are active and used in the |MAXC| calculation.

Also in the loop, the $!SETFIELDVALUE command is used to set the point value for the specified variable and zone. In this case we are setting the solution time extracted by the QUERY.TIMEATSTEP and the |MAXC| value to the zone created in step 2.

In preparation for creating a new XY plot the macro performs some simple actions to clean up the plot.

First, the newly created zone’s field map is removed from showing the original plot, since it may affect how it is displayed. Then Frame linking is turned on and the frame is brought to the top.

The next step is to create a new XY plot for the newly created zone with a marker which indicates the current time step of the 3D plot.

The XY position and dimensions are provided to create a new frame. This new frame automatically becomes the new active frame. For this reason, changing the plot type and other commands called after the $!CREATENEWFRAME command only affect the newest frame and not the original.

By default, when the plot type is changed to XY Line, line maps are automatically created. The $!DELETELINEMAPS command must be called in order to create custom line maps. In this case, only one line map is needed. The name and zones are assigned to the newly created line map and it is then activated. By default, line maps will use the first two variables of each zone, hence why only the first two variables were edited in step 3.

To clean up the plot for presentation, the title is set using the XYLINEAXIS commands. The final two lines ensure that the new frame is linking solution time with the previous one and create a marker line to track the current solution time between both frames.

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 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.).

Navigate to your Tecplot 360 Getting Started Bundle folder then the Internal Combustion Engine (ICE) folder. Select all of the .plt files and select Open. The data files are opened and a 3D plot of the Combustion Engine appears in the Tecplot 360 workspace, as shown here:

You may have noticed a dashed orange line when you first loaded your example file. This is the bounding box of the grid volume zone, which represents the air within the engine. 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 is there and can see its dimension. You can choose to hide this line. From the Options menu, select "Show Bounding Boxes for Enabled Volume Zones with No Style". The dashed orange line disappears.

Since most of the data of interest lies within the cylinder, hide the exhaust zones by right-clicking the visible zones and selecting "Hide".

Try to hide as many of the exhaust port zones as possible. After hiding, the plot should look something like this. Do not worry if there are a few zones still active.

To add a slice, toggle on the Slices checkbox in the Plot sidebar.

A slice appears through the volume zone but may be hidden by surfaces. To be able to see the slice through the middle of our engine we must turn on Translucency in the Plot Sidebar as well.

From there the slice can be moved by selecting the slice interactor tool to place the slice interactively. The interactor tool can move the slice by clicking or dragging to a desired location. This can also be achieved by selecting the button next to the Slices checkbox. For now, leave the slice in its default location. The Slice details dialog appears with the current Slice location and orientation.

The Slice Details dialog displays the exact slice position.

Setting the Contour

If you have the Slice Details dialog still open, navigate to the Contour tab. You will see our slice is being contoured by "mass" as this is the variable currently assigned to Contour Group 1. To change the variable in Slice Group 1, click the button next to "Contour" on the Plot sidebar. This will open the Contour Details dialog. This dialog can also be opened by selecting the gear icon next to the Flood By field on the Slice Details dialog.

To change the variable of Contour Group 1, select the "1" button at the top of the Contour Details dialog and select the dropdown list that currently displays mass. Select temp for now. Close the Contour Details dialog.

Back in the Slice Details dialog, you should see the variable under the Contour tab change to temp as well. The contour group changed successfully!

Turning on the Mesh

We also want to see the mesh of our slice so we will turn that on as well. Right-click the slice on your screen to open the context menu and select the Mesh option. Shown below:

The slice mesh can also be turned on via the Other tab of the Slice Details dialog.Select the magnifying glass in the toolbar to zoom in for a better look.

Using the Forward, Back, and Play buttons on the Plot Sidebar, see how the plot changes over time.

The slice gives a good indication of the temperatures in the cylinder through time. However, the slice is not the only tool at our disposal. This data set also contains spray information that may be beneficial for our visualization of the engine. To follow along, be sure your Solution Time in the Plot sidebar is set to the first time step.

Open the Zone Style dialog from the plot sidebar and scroll to the bottom of the Zone list. There you will see a zone called "Spray". We want to style this zone to our specifications. To do this, check the Scatter checkbox from the Plot sidebar.

The plot will update with scatter symbols for every zone. This is not what we want though. We only want to show the scatter symbols for the "Spray" zone. In the Zone Style dialog, select the Scatter tab and highlight every zone except the "Spray" zone, right-click the "Show Scatter" column and select No.

Now the "Spray" zone is the only one showing a scatter plot but displaying as same sized squares. In the Scatter tab, right click the symbol shape and change it to Sphere.

Then we also want to change the symbol size, right click the column for Symbol Size and select the "Select Variable" option.

This will open the Scatter Size/Font menu.

We want to have the Scatter symbols sized by their radius, from the scatter symbol variable dropdown menu, select the variable DP_radius. However the plot still hasn’t updated yet. Finally right-click the symbol size dropdown menu again and select the DP_radius variable. Your Zone Style should look like this and the plot should show scatter spheres sized by radius.

The spray has differing size but it still does not give us much information. Contouring the scatter symbols by temperature would be helpful. Open the Zone Style dialog again to the Scatter tab. Scroll down to the "Spray" zone and then scroll to the right to the Outline Color. Right-click the Outline Color and the Color Chooser menu will appear.

Select Multi 2. This corresponds to the Contour & Multi-Coloring group 2. To change the variable of group 2, we will go back to the Contour Details dialog accessed by the button on the sidebar next to the Contour toggle. For the parcels, we want the color to be contoured by DP_temp. Now you can see how the parcels change temperature and size through time.

You’ll notice after changing the Parcel color that two contour legends appear on screen. This is because the parcels are colored by DP_temp while the slice is contoured by temp. Since both contours are in reference to temperature, we can update the contour levels of both contour groups.

First remove the legend on contour group 2 by right-clicking the legend and selecting Hide. Then in the Levels and Color tab and select the Set Levels button. Enter the level information like below.

Now repeat with group 1. This will update temp and DP_temp to the same scale.

Scenic Detour: Setting Default Scatter style in the Configuration File

If typical workflows include scatter on a single zone changing the default style can save many clicks.

These commands will change the default values for Scatter to "off" and the shape to "Point". This is especially helpful in situations like our example where we only want to turn on one zone’s Scatter points. Note that color contours cannot be set in the configuration file.

The tecplot.cfg file, located in the installation folder, is able to set a default scatter shape and state for simplicity. Open the file in a text editor of your choosing and add the following lines to your configuration file:

For this next step we will use iso-surfaces to visualize a flame front during the ignition phase of our engine. Be sure the slice created in steps 1 and 2 is turned off by unchecking Slices on the sidebar but keep the spray turned on, optionally, with the Point scatter shape. Your data should look something similar to this:

Next, we will turn on the Iso-surface option from the Plot sidebar. Select the checkbox next to "Iso-Surfaces" and then the button (similar to how we opened the Slice details dialog). This will open the Iso-surface Details dialog.

Since we want to visualize a flame front, use the variable temp set to Contour Group 1. Also select the Contour tab on the Iso-surface Details dialog and verify the Iso-surface is being contoured by temp as well.

Back on the details page, set the value of the Iso-surface to be 2000, which represents the flame front.

Pressing the play button on the Plot sidebar to animate through the flame front propagation.

Our visualized data is starting to come together. However, it can be convenient to view data from multiple angles. This will give a better understanding of the data from all sides. This can be easily done by selecting Frame → 3D Multi Frames. For this example, we will use the top-left option.

This will give us orthogonal views of our data set and we can derive a better understanding of our data throughout time.

Now that we have our plot set up as we want it, let’s export our final product to a movie file. Select the button next to the Solution Time to open the Time Animation Details dialog.

This dialog displays more advanced animation options than the Plot sidebar.

From the Time Animation details dialog, select the "Export to File" button next to the VCR buttons. This will open up the Animation Export dialog. The default animation export is MPEG-4. Because of the 3D Multi Frames in our workspace, ensure the region is "All Frames".

You can also choose to export a larger image width than your current view. This is especially helpful if the movie is going to be displayed on a high-resolution screen. For this example, we want our final product to be viewed on a 4K resolution display so we will enter a width of 4096. Select OK and save the final file.

Load area_avg_flow.out from the ICE directory of the Getting Started Guide Bundle. Select File > Load Data. Once prompted, select the CONVERGE Output Loader.

Selecting OK will load the plot in XY Line type.

The plot by default is in XY Line mode which contains pre-loaded XY Line maps. Select the Mapping Style button on the Plot Sidebar to see which Mappings are available. You can see that this file was loaded with many variables premade vs. the Crank Angle. For this example, cange the plot to show Avg_Temp and Mass_Flow_Rate by Crank Angle. Turn off the default map for Crank vs Cycle Number. Turn on Map numbers 2 and 5.

Notice how the plot automatically merges both lines to one Y Axis. The min/max values of Mass_Flow_Rate and Avg_Temp are very different, so putting one of the mappings in a second Y axis will help.

Select the Mapping Style button again on the Plot Sidebar. Scroll to the right to the "Which Y-Axis" column and right click the Avg_Temp row. Then select Y2 as the Y-Axis. The plot will automatically update.

Finally close the Mapping Style dialog to see the final plot. If your plot doesn’t automatically update to the new axis bounds, select Ctrl+F (or use View > Fit to Full Size).

To increase the line thickness, right-click the line to bring up the right-click context menu and update the the thickness as desired. For black and white printing, consider changing one of the lines to dashed.

Select Plot > Axis to open the Axis Details menu (or double click on the axis). From the Axis Details menu, you can see the different tabs to update the plot axes. Notice the X1, Y1, X2 …​ buttons, these control the axis being acted on. For now, we want to update the X1 Grid Lines. Select the Grid tab to update the grid lines for the X1 axis. Select the Y1 button as well to update the Grid options for Y1. In our case, Y1 is the Mass_Flow_Rate.

Select the Show checkboxes under Gridlines and Minor Grid Lines. Notice how the Major Tick labels have the Solid gridlines and the Minor Tick labels have the Dotted Gridlines.

Next select the Y2 button to edit the Grid Lines for Avg_Temp. Like before, show the Gridlines but this time leave the Minor Gridlines off. Also notice that there are no distinguishing differences between the major gridlines. For that reason, we want to update the Gridlines color to "Blue".

Next, we want to update the Axis Labels to be spaced more cleanly. For Avg_Temp, the axis labels are spaced well with 100 points between each step so Y2 will not need to be updated. However, we will update Y1 to a better distribution. From the Axis Details dialog select the Labels tab.

Deselect the Auto Spacing option at the bottom to give us control of the Label Spacing. Then in the Spacing field, update the number to 0.025. Close the Axis Details dialog.

The final plot is shown below:

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 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).

Navigate to your Tecplot 360 Getting Started Bundle folder and then the Ocean folder. Highlight the .nc file and select Open 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 Boston harbor loads in the Tecplot 360 workspace, as shown here, an orange box shows the bounds of the volume data. See Understanding Volume Surfaces.

The orange bounding box represents a volume dataset that is loaded with no style. For more information on Surfaces to Plot see Understanding Volume Surfaces. To see what data has been loaded, open the Data Set Info dialog. From the top of the screen select Data→ Data Set Info. This will bring up a dialog with lists of loaded zones and variables.

In the Zones field, we can see that the NetCDF ocean model has loaded 24 zones. In this case, each zone represents a new timestep of the data so we have 24 timesteps in total. We can also see in the other column the variables that have been loaded from the dataset. Close the Data Set Info dialog for now.

For the first representation of the data, turn on the Contour layer. Select the checkbox next to Contour on the Plot Sidebar.

A pop-up will appear asking about Surfaces to Plot. For now, select "Yes". A contour plot will appear with the default contour variable selected. In this case it is "lon". This is because "lon" is the first, non-XYZ variable in the dataset.

For this plot, change the X and Y coordinates to Lon and Lat. This will make it easier for things like georeferenced images to be placed in the plot (see Insert a Georeferenced Image). To do this, select Plot→Assign XYZ and change the X variable to "lon" and the Y variable to "lat".

The plot will automatically update on pressing OK.

You may have noticed pop-ups that say, "Aspect ratio exceeds ratio limit. The ratio has been adjusted." This is because Tecplot attempts to maintain a visually interesting axis ratio to prevent any one direction from being too small. However, adjust this ratio because the current plot is too tall in the Z direction. Select Plot→ Axis to open the Axis Details dialog.

Towards the bottom of the dialog is the Dependency field. These options can determine XYZ dependency based on your information. The Z-axis needs to be smaller so set the plot "XY Dependent". Select the button next to "XY Dependent" and adjust the Z-axis size factor to be something like "0.000667".

Note that the Z-axis is still exaggerated even at this ratio, but it gives a better understanding of the overall scale.

If you want the map to change to a top-down view, select the rollerball rotate (shown below), click, and drag the screen around to get a top-down perspective.

Another option is selecting "Snap to Orientation view" in the Plot Sidebar and selecting the XY perspective.

From this angle, lighting effects wash out the contour color. For now we can turn off lighting by unchecking the "Lighting" checkbox on the Plot sidebar.

Now the plot should have no lighting effect and the contour data can be seen more clearly.

The contour variable has remained at the default of "lon" up until now, update to a more data relevant variable like "Salinity". To do this, select the button next to Contour on the Plot sidebar. The Contour & Multi-Coloring details menu appears.

Notice the dropdown list at the top of the dialog is set to "lon". Select the dropdown list and all the variables in your dataset appear. Now select "salinity" as your new contour variable. The plot will automatically update.

Also select a new colormap based on the cmocean colormaps, in this case, the "cmocean - haline" colormap which is designed to be used with salinity plots. To change the colormap select the colormap dropdown from the middle of the Contour & Multi-Coloring Details dialog, and select "cmocean - haline" option.

After updating the plot to "salinity" notice the shoreline of Boston harbor within the plot. However, the contours extend out from beyond the shoreline. This dataset has a variable called "wet_nodes" to determine what is wet (denoted by the variable = 1) and what is dry (denoted by the variable = 0).

To hide the dry nodes on the plot where "wet_nodes" is equal to 0. Go to Plot→Blanking→Value Blanking to pull up the Value Blanking dialog.

Then turn on the "Include value blanking" checkbox. This will tell the plot that we want to blank something. Change the Blank when fields to be when "wet_nodes", "is equal to", "Constant" and "0". Then select the "Active" checkbox. The plot will update accordingly. The exact value blanking options are in the image above and final plot should look like this:

Now that the plot is looking good, let’s animate through time. Select the Play button on the Plot sidebar to play the animation. The plot will show the ebbing and flowing of salinity in the Boston harbor.

Note that the first animation takes longer because it needs to load data. The second play through will be faster as the data has already been loaded.

Now we want to save this animation to a movie file. On the Plot sidebar select the button next to Solution time and the Time Animation details dialog will appear. This dialog can give more control over your plot animation but since the default settings are already sufficient, select the "Export to File" button next to the VCR buttons on the Time Animation details dialog.

From the Export dialog, we can select things such as export format, image width, antialiasing, and animation speed. For this instruction, select the MPEG-4 format. This will create a file with an .mp4 extension that is usable by most video viewers. Also, turn on antialiasing as well to get the definition on the shoreline and have smoother lines. Keep everything else the default and click OK.

Next, save the file to a convenient location as "boston_salinity.mp4". Congratulations you’ve created your first Tecplot ocean animation!

This section is a continuation from the previous section. If you are joining partway through, open the Ocean1.lay from the finallayouts directory.

The next portion will use an iso-surface to identify the bathymetry of the dataset and use slices to identify layers through the volume. If you are continuing from the previous portion, remove the georeferenced image and turn off the blanking of siglev.

A vertical transect gives a curved slice extracted through time. We have created a video showing the steps to create the Vertical Transect. It is located here: www.tecplot.com/2018/10/17/vertical-transect.

The Time Average script creates a duplicate zone with the varaibles averaged over time. It is located here: www.tecplot.com/2018/10/17/calculating-average-over-time.

The Shapefile conversion script converts a shapefile into Tecplot .plt format. It is located here: www.tecplot.com/2018/10/17/converting-shapefiles-plt-using-pytecplot.