Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert) ANSYS Fluent Tutorial Developing Laminar Flow in a 2D Channel 1 How to use This Tutorial? As you read it also perform each step on your own computer. Do not skip any detail. You are advised to finish all the steps in one sitting so start working on it when you have enough time to finish. Take notes about things that you cannot follow and let the course instructor know about them. Also let him know if you notice any mistakes. Do not forget that the aim of the tutorial is not really solving the selected problem in the most accurate and efficient way. The aim is to show you how to setup and solve a problem in ANSYS Fluent. The typical three stage procedure (pre-processing, solution, post-processing) is also not that different in other commercial software. When you finish all the steps you can go back and try changing problem definition parameters, try different mesh generation or solution settings, perform extra post-processing, etc. Choices are endless. You ll also see many general CFD related discussion, important notes, questions and to do items inside the tutorial. Problem Definition Consider a 2D channel of length 1 m and height 0.1 m. A fluid with density 1 kg/m 3 and viscosity 0.0001 Pa-s enters the channel at a uniform speed of 0.025 m/s. We want to simulate the developing laminar flow in the channel. 0.025 m/s No slip 0.1 m p = 0 1 m We are interested in how the velocity profile and the pressure changes as the flow develops. Reynolds number based on the inlet speed and channel height is Re = ρu inh μ = (1)(0.025)(0.1) 0.0001 which is a very low value making the flow definitely laminar. = 25 Question: Why do we define the Reynolds number based on channel height, but not channel length? When will this flow turn into turbulent? 1 ANSYS 18.2 student version is used to prepare this tutorial. Some screenshots show 14.5 as the version. Do not get confused by that. Those are the parts where there is not much difference between different versions, so I used old screenshots that I took previously. 1
Step 1: Start ANSYS Workbench. You ll see 2 tabs as Toolbox Project Schematic 2
Step 2: In the Toolbox tab, under Analysis Systems, find Fluid Flow (Fluent) and drag and drop it to the Project Schematic tab. Change the name of the analysis to Tutorial 1. A Fluent analysis is composed of 5 parts Geometry: To draw or export the problem domain Mesh: To generate the computational mesh Setup: To define the problem physics, boundary conditions, solver settings, etc. Solution: To run the analysis Results: To post-process the solution In this tutorial we ll be using the first three, i.e. Geometry, Mesh and Setup. 3
Step 3: In the View menu of the Workbench select Properties to see the Properties tab. In the Project Schematic select Geometry. In the Properties tab change Analysis Type from 3D to 2D. 4
Step 4: To generate the problem geometry, we have three options; Draw it in Space Claim Draw it in Design Modeler Export a geometry already drawn in another CAD software. Space claim is a full featured CAD software. Design Modeler is a simpler tool. We ll use the Design Modeler for our simple rectangular problem domain. In the Project Schematic right click on Geometry and select New DesignModeler Geometry. This will open the Design Modeler window. It has 3 main tabs Tree Outline (Under it there are Sketching and Modeling tabs) Details View Graphics 5
Step 5: At the lower right corner of the Graphics tab find the X, Y, Z arrows and click on the Z arrow to look directly at the XY plane from -Z direction. Step 6: In the Tree Outline tab select the Sketching tab and under Draw select Rectangle. Draw a rectangle of arbitrary size by locating its lower left corner at the origin. Right click on the Graphics tab and select Zoom to Fit. There is also a button for this in the toolbar ( ) 6
Step 7: In the Sketching tab select Dimensions. Select Horizontal and insert a horizontal dimension by selecting left and right sides of the rectangle. Select Vertical and insert a vertical dimension by selecting upper and lower sides of the rectangle. In the Details View tab set the values of horizontal and vertical dimensions to 1 m and 0.1 m, respectively. Select Zoom to Fit. Important Note: Depending on the regional settings of your computer real numbers may require either, or the. as the decimal point. In my computer I need to use,. Note: You may need to adjust the positions of H1 and V1 dimensions. To do this in the sketching tab, select Dimensions and Move. 7
Step 8: From the Concept menu select Surfaces from Sketches. In the Modeling tab, select Sketch 1 under XYPlane. In the Details View tab, press Apply button to set the Base Objects. Click the Generate button of the toolbar to generate a 2D part that will be seen in gray color in the Graphics view. The Tree Outline should look like this, showing the part that we just generated. 8
Step 9: In the Modeling tab you ll see 1 Part, 1 Body under which there is Surface Body. Right click on Surface Body and change its name to Channel. In the Details View change Fluid/Solid to Fluid. Use Ctrl-S to save the project and close the DesignModeler window to go back to the Workbench window. Important Note: When saving your project make sure that the file name and the whole PATH do not contain any Turkish characters. If you go to the folder where you saved the project you will see the Workbench file and two folders. The 2D drawing we created is at Tutorial 1_files > dp0 > FFF > DM > FFF. Very weird names, I know. Note: As you may have noticed, working in the Design Modeler is not very comfortable. You can try Space Claim if you want. It is a more modern CAD software. 9
Step 10 In the Problem Schematic tab of the Workbench double click on Mesh to start the Meshing application Meshing application has 3 main tabs Outline Details of Model Geometry Note: When first started Meshing application comes with many Toolbars at the top. You can close the ones that you do not use often from View > Toolbars menu. 10
Step 11: If necessary click on the Z arrow of the Geometry tab to see the channel from -Z direction and select Zoom to Fit. First we ll give names to the inlet, exit and upper/lower walls so that later these names can be used to define boundary conditions and to perform post-processing. Click on the Edge button ( ) of the toolbar in order to be able to select edges. Using the mouse and the Ctrl key select upper and lower walls of the rectangular domain. In the Geometry tab, right click and select Create Named Selection. Give a name Walls to this selection. Select the left side of the rectangular domain, right click and select Create Named Selection. Give a name Inlet to this selection. Select the right side of the rectangular domain, right click and select Create Named Selection. Give a name Outlet to this selection. In the Outline tab, click on the created Named Selections and see if the correct parts of the problem domain are highlighted or not. If not, delete and recreate them. 11
Step 12a: Select Mesh in the Outline tab. Press the Generate Mesh button of the toolbar. With the default parameters, the following coarse structured mesh will be generated. In the Statistics part of the Details tab you can see that the mesh has 63 nodes (cell corners are called nodes) and 40 elements (cells). Note: If you cannot see the mesh, make sure that Mesh is selected in the Outline tab. 12
Step 12b: The mesh generated with the default options seems too coarse to capture correct velocity and pressure variations across and along the channel. The expected fully developed parabolic velocity profile may require more than two cells across the channel to be resolved correctly. It is possible to control the mesh details in many different ways. There are official ANSYS tutorials for mesh generation. A quick way to make the mesh finer in the whole problem domain is to change the change the Relevance Center in the Details tab. Change it to Fine. Press the Update button of the toolbar. A new mesh of 476 elements will be created. Now there are 6 cells across the channel. This may be enough for this simple laminar flow. Note: Relevance Center is a global mesh control parameter, i.e. it affects the whole mesh. It can take three values; Coarse, Medium and Fine. It s also possible to change the mesh locally, e.g. make it fine close to the inlet only, or make it fine close to the top and bottom walls. Note: How can we make sure that a generated mesh is good for a given problem? That s a very good, but hard to answer question. It is the million dollar question of CFD. As you work on different problems and get experienced, you ll start developing a feeling of mesh requirements. 13
Step 12c: If you want to refine the mesh further, change the Relevance parameter to its maximum possible value of 100 and press the Update button. This is another quick way of changing the cell numbers globally. This new mesh has 1000 elements. It has 10 cells across the channel. 14
Step 12d: If you want to make the mesh even finer, right click on Mesh in the Outline tab and select Insert->Refinement. In the Geometry tab select the rectangular domain and press Apply button on the Details tab. Leave the Refinement value at its default value of 1. You can increase it to have more cells. Press the Update button. The new mesh has 4000 cells. It has 20 cells across the channel. There are many other ways to control the cell sizes both locally and globally. But we ll stop here and use this last mesh of 4000 cells. Save the project and close the Meshing window to go back to the Workbench. To Do: After finishing this tutorial you can come back to this step and try to solve it with a coarser mesh (e.g. one of the coarser ones that we generated above) and see how the results are affected by this. 15
Step 13 In the Workbench window double click on Setup to start Fluent. In the Fluent Launcher window, check Double Precision option. With this option floating point numbers are kept in computer s memory in double precision, instead of single precision. This will result in less round-off errors and may improve accuracy and convergence, but also increases memory usage. We almost always use Fluent in double precision. Press OK. Important Note: As far as I could notice, ANSYS software constantly communicates with ANSYS (the company) about licensing. When I tried to launch Fluent I got an error saying The FLUENT application failed to validate the connection and Fluent stopped responding. After I installed all Windows updates, everything turned to normal. 16
In Fluent you can either use the Menu or the Tree tab to setup and solve the problem. I usually use the latter and to save some screen space I minimize the Menu using the Minimize ribbon button ( ). Menu Note: As seen above, Gravity option is not checked. Therefore, weight of the fluid will not be included in the momentum equations. You need to determine whether fluid weight is important or not in a given problem. What do you think, is it important in this case? Why/Why not? 17
Step 14: Inside the Tree, double click on General under Setup. We ll not change the default settings here. Pressure-based solver is preferred for incompressible flows and density based one is used for compressible cases. This problem is time independent (steady). And it is a 2D planar problem. You can click on the Help button to read the technical details about these options. ANSYS Fluent has a good Help. Note: Report Quality button calculates quality measures (such as orthogonality or aspect ratio) of the mesh. For the mesh we created quality is of no concern. 18
Step 15: Double click on Models. Again we do not need to change anything. This is a single phase flow with no heat transfer. Therefore, we do not need to solve for the energy equation. Also the flow is in the laminar regime. All other model settings are Off. Use the Help button to read more about different models. 19
Step 16a: Double click on Materials. Fluent uses air as default fluid and aluminum as the default solid. In this problem we do not have any solid domain. But the fluid is not air, its properties are given in the first page of this tutorial. Double click on air to change the fluid properties. 20
Step 16b: Fluent comes with a database of different fluids. But the one we use in this problem is none of those. So let s create a new fluid. Change Name to myfluid. Enter 1 for density and 0.0001 for viscosity. Press the Change/Create button. Press Yes in the dialog box that asks for Change/Create mixture and Overwrite air? This will replace the default air with the newly defined myfluid. Press Close to close the Create/Edit Materials window. Important Note: Previously in Step 7 we used, as the decimal point. But here in Fluent we need to use.. This is an inconsistency. Beware of that. Important Note: While working in Fluent save your work from time to time. Fluent has no autosave capability. All your unsaved work will be lost in case of power outage or a software crash. 21
Step 17: Double click Cell Zone Conditions There is only one zone here, the channel. It is the name we gave to it in Step 9. Its type is fluid. Double click on channel and make sure that its material is the newly created myfluid. 22
Step 18a: Double click Boundary Conditions. There are four items; inlet, interior-channel, outlet and walls. Interior-channel is the one automatically created by Fluent. The other three are the ones we named previously in Step 11. Select inlet and make sure that its type is velocity-inlet. Note: If you give meaningful names to boundaries of your domain, Fluent can automatically assign correct boundary condition types to them. For example, when Fluent sees the word inlet in a name, it automatically assigns velocity-inlet type to it, which is most probably what you want. But still it is always a good idea to check whether correct boundary condition types are assigned or not. 23
Double click on inlet and change Velocity Magnitude to 0.025 (the value given in the first page of the tutorial). Step 18b: Select outlet and make sure that its type is pressure-outlet. 24
Double click outlet and set Gauge Pressure to 0. Default value is already zero. METU Mechanical Eng. Dept. - ME 485 CFD with Finite Volume Method Note: Fluent works with gauge pressures. As seen below in the Operating Conditions window that is accessed from Cell Zone Conditions, operating pressure is set to 101325 Pa by default, which is 1 atm. When we specify 0 gauge pressure at an outlet, it is with respect to this operating pressure. For incompressible flows the actual pressure values are not important, only the space derivatives of pressure are important. Therefore, selecting another operating pressure or a different exit gauge pressure will only shift all pressure values of the final result up or down by a certain constant. But this will not affect the velocity field at all. But for compressible flows, pressure is a thermodynamic property and its actual value is important. We cannot arbitrarily specify a zero gauge pressure at an outlet of a compressible flow. 25
Step 18c: Select walls and make sure that its Type is wall. Double click on walls. By default it is a stationary wall with no-slip boundary condition. Do not change them. 26
Step 19: We ll skip the Dynamic Mesh and Reference Values parts of Setup. They are not used for this problem. Dynamic Mesh part is used when the boundaries of a problem domain are moving and therefore the mesh inside is also moving. Reference Values part is used to set the reference quantities for computing normalized flow field variables. For example, to calculate the drag force coefficient over a body we need a reference velocity, a reference density and a reference area. No need to change anything under these. This is the end of the Setup process in Fluent. Save the project. 27
Step 20: Under the Solution title double click on Methods. We ll not change the default options. Notes: The default scheme is SIMPLE, which stands for Semi Implicit Method for Pressure Linked Equations. It is one of the most commonly used techniques to solve incompressible flows. We ll study it in our course. The alternatives SIMPLEC and PISO are variations of SIMPLE. PISO is usually preferred for unsteady flows. These three are segregated (sequential) solvers, i.e. continuity and scalar momentum equations are solved one-by-one. In the last alternative Coupled, all governing equations are discretized into a single system of linear algebraic equations and solved at once. It usually consumes more memory, but provides faster solutions. You are advised to use Coupled solver if your computer has enough memory. For the 2D simple problem that we are working on with only 4000 elements Coupled solver will not create any memory issues, but we ll go with the default SIMPLE scheme. Other settings are about how different terms of the governing equations are discretized. As you get more experienced in CFD, you are advised to read the details from the Help. To Do: After finishing this tutorial, you can come back to this step and change the Scheme to Coupled, initialize the problem and solve it again to see how the number of iterations necessary for convergence will be affected by this. This is a small 2D problem and run-time is very short anyway, I know, but that s not the issue here. The issue is to understand how different settings affect the solution. 28
Step 21: Double click on Controls. We ll not change the default settings. Here we set the under-relaxation factors. Navier-Stokes equations are non-linear and they need to be linearized during the discretization step. This linearization makes the whole solution iterative. Conceptually, it is different than the iterative solution of a linear algebraic equation system. But the possibility of divergence and the cure of it are similar. Remember the iterative linear algebraic equation system solution techniques, such as Gauss- Seidel, from ME 310 course. Those techniques work iteratively and there is the possibility of divergence. To reduce that possibility, we can use under-relaxation. What we do here is similar to that. Note: If you face convergence problems, i.e. residuals are not dropping or if the solution totally blows up, you can consider lowering these relaxation values. Lowering them will decrease the possibility of divergence, but will also reduce the rate of convergence, i.e. the residuals will drop slower. 29
Step 22: Under Monitors, double click Residual. Here we can control how the residuals are printed and plotted on the screen. Also we can set the tolerance values for the convergence of each scalar differential equation that we solve. In this 2D problem we solve for continuity, x-momentum and y-momentum equations. By default, tolerance is set to 0.001 for all. It is usually a good idea to reduce these values at least one order of magnitude, i.e. to 0.0001. As you decrease the tolerances, the converged approximate numerical solution that you ll calculate will satisfy the conservation equations better. But lower tolerances will result in doing more iterations to get a converged result and therefore will take more time. Here we ll not change the defaults. 30
Step 23: Other than the residual plot that is created by default, it is also advised to watch the progress of a solution by creating monitor points. Fluent calls this reporting. In our problem the flow will develop from inlet to exit. If the exit velocity profile is not changing anymore during the iterations, we can take it as an indication of a converged steady solution. So we ll monitor the x-velocity component at the mid-point of the exit boundary, i.e. at point (1, 0.05). Double click on Report Definitions and press the New button. Select Surface Report and Vertex Average. Note that Fluent s reporting related terminology is a bit strange. 31
Change the name of this report to exit-velocity. Change the Field Variable to Velocity and select X Velocity. Select Report Plot to generate a plot of the monitored data during the solution. Also select Print to Console so that the monitored data can also be seen as numbers. To select the monitoring point press the New Surface button and select Point. Note: As seen above it is also possible to select Report File to write the monitored data to a file. This way we can open and work on it in any way we want. We re not doing it now. 32
Enter the coordinates as (1, 0.05) and name the point as exit-mid-point. Press Create and close the window. METU Mechanical Eng. Dept. - ME 485 CFD with Finite Volume Method Now you are back to the Report Definition window and under Surfaces, the newly created exit-mid-point appeared. Select it and press OK. 33
Since we selected the Report Plot option while setting up the monitoring details, a new Report Plot called exit-velocity-rplot appeared under Monitors -> Report Plots. If you want, double click on it change its properties, such how it will appear on the screen, e.g. how many digits the axes numbers will use or how thick and in what color the plotted curve will be. We ll not change the defaults. Notes: In Fluent it is possible to generate monitors not only for points, but also for areas and volumes. For example, you can monitor the mass flow rate at the exit. There are also many built-in monitors, such as those for lift and drag coefficient acting on a body or heat transfer rate passing through a part of the boundary. It is possible to define new stopping criteria for iterations based on the monitored data. To do that you can use Convergence Conditions, seen on the right. We ll not do that here. 34
Step 24: Before we solve the problem we need to initialize the unknowns. This is necessary also for steady problems because the solution procedure is iterative and it needs initial guesses to stat the iterations. Double click Initialization. Keep the default Hybrid Initialization option and press the Initialize button. Save the project. 35
Step 25: In the Run Calculation tab set Number of Iterations to 1000 and press the Calculate button. Note: The value 1000 is selected somewhat arbitrarily. If, after the solution, it turns out to be not enough, we can always perform additional iterations, so it is not a problem. During the solution residuals and monitored data will be written in the Console tab as seen below. For this simple 2D problem the solution finished in only a few seconds. It converged in 43 iterations (Iteration numbers can be a bit different if you use a different version of ANSYS). As soon as the residuals of all three equations (continuity, x-velocity and y-velocity) drop below the specified tolerance (0.001), solution is considered to be converged and stopped. The final value of the x-velocity at the mid-point of the exit plane is reported as 0.0368 m/s. Residuals Monitored data at the exit-mid-point 36
During the solution two plots are generated, one for the residuals and one for the monitored data. Residual plot looks like this. Note that these are scaled (normalized) residuals. See Fluent s Help to see what exactly they correspond to. At this point it is enough to know that they are a measure of how good the calculated approximate solution satisfies the equations that are solved. There is one curve for each of the solved equations. White curve is for continuity equation and it is the one that converges slowest. Tolerance that we set The plot for the monitored velocity at the exit plane is given below. Although it is hard to read the numbers in this view, it starts from an initial value of ~0.025 (which is the inlet speed. Fluent used it to initialize all velocities) and reaches a value of ~0.037. But looks like that the curve is still in rise, that s it did not reach steady state yet. It s almost there, but not exactly. 37
Step 26: To make sure that steady state is reached at convergence, let s decrease the convergence tolerances and perform additional iterations. Go back to the following Residuals Monitor window and reduce the tolerances by 100 times, to 10-5. Under Run Calculation press Calculate. Note that we did not initialize the problem, meaning that the new solution will continue from where the previous one stopped. This is what we want. The new solution will converge in a few seconds with a total of 132 iterations. All residuals will drop down to the specified tolerance and the new monitored data plot will be as follows, which shows a better steady state convergence. The converged x-velocity at the mid-point of the exit plane is now 0.0373 m/s (as seen in the Console tab), not that much different than the previously calculated one. Converged to steady state. Not changing anymore. 38
Step 27: We have two options to do post-processing and generate plots. Do it inside Fluent. That s what we ll do here. Fluent s built in visualization capabilities are enough for us for this problem. Use the CFD-Post application that comes with Fluent. For this, close Fluent, go back to ANSYS Workbench and double click on the Results part of the analysis. You can perform more advanced visualizations and generate better looking plots with CFD-Post, but it has its own learning curve. Let s draw some contour plots. Under Results, double click Contours. In the Contours window check the Filled option, set Contours of parameter to Velocity and Velocity Magnitude and deselect all the Surfaces. Press the Save/Display button to see the velocity magnitude contours. 39
Following velocity magnitude contour will be generated. Developing and fully developed regions can be distinguished. The legend is not shown here, but red color shows high speed and blue shows low speed. As the flow develops, fluid particles close to the walls slow down (blue color) due to the no-slip boundary condition and those close to the channel centerline speed up (red color) to conserve mass. Developing region (roughly) Fully developed region Notes: To zoom in/out use the mouse wheel. To zoom into a specific region use Ctrl + Left mouse button. To pan (move the plot around) use Ctrl + Right mouse button. Important Note: You can save the generated plots using the Save Picture button ( ) on the left of the contour plot. While doing this make sure that White Background option is checked. When you put post-processing images in your homework report, do it this way and if necessary open the saved image in an image editor software (simplest is Microsoft Paint) and crop unwanted details. Let s also see what the pressure is doing by creating another contour plot. Double click Contours and this time select Pressure and Static Pressure. Contour plot is given below. In the developing region iso-contour lines are curved but in the fully developed part they are straight and vertical. This is expected because in the fully developed region streamlines are straight and parallel and from Me 305 course we know that pressure variation across such straight lines are hydrostatic (as if the fluid is not moving). When the fluid weight is not accounted for this means at each cross section pressure need to be constant, and it is. Note: If you do not check the Filled option when creating a contour plot, iso-contour lines will be shown. It might be a better option for the above pressure plot. 40
Step 28: To plot the streamlines double click Pathlines. For this steady problem streamlines and pathlines are the same. To release the streamlines from the inlet select inlet as shown below. Press Save/Display. Streamline plot is as follows. Following version shows a close up view of the inlet part. Close to the inlet there are nonzero v velocity components as expected. As the fluid slows down due to no-slip at the walls it rushes into the centerline, increasing the centerline speed. 41
To Do: In many plots including the above one, we do not want to see the default blue background color of Fluent. Can you change it to white? To Do: At the bottom left corner of the Pathlines window there is a Pulse Mode option. If you change it to Continuous and Press the Pulse button, you can see a nice animation of pulsed streamlines. Try it. 42
Step 29: Let s have a look at how the centerline velocity changes. Under Plots double click XY Plot. First let s generate a line that ll represent the centerline. Press New Surface button and select Line/Rake. In the Line/Rake Surface window enter the end points of the centerline as (0.0, 0.05) and (1.0, 0.05). Rename the line as center-line and press the Create button. Close the window 43
Now you are back at the Solution XY Plot window Select Velocity and X Velocity for the variable to be plotted. Select center-line from the Surface list. Press Save/Plot. x velocity changes along the centerline as follows. It starts from the inlet value of 0.025 m/s and smoothly rises to the fully developed value of 0.073 m/s (it is hard to read it from this plot but we monitored for that value previously and we know it precisely). Entrance length is roughly about 0.3 m, i.e. 3 times the channel height. Developing region (roughly) Fully developed region 44
Let s also plot the pressure variation along the centerline. METU Mechanical Eng. Dept. - ME 485 CFD with Finite Volume Method Double click XY Plot and this time select Pressure and Static Pressure. Also select the already available center-line. The result is shown below. Other than the short region close to the entrance pressure drop is linear. It is expected based on the known analytical solution of this laminar 2D problem (see your ME 305 notes/book). Note: The total pressure drop along the centerline is 0.003 Pa. It is a very small value due to the short channel length, low speeds and low viscosity value. To Do: Calculate the slope of the pressure drop (dp/dx) in the fully developed region and see if it matches with the analytical solution or not? To Do: Analytical solution is available only for the fully developed region, not the developing part. What is so difficult in the developing part that it is hard to solve (if possible at all) analytically? Important Note: In most of the visualization plots given of this document, axes numbers are hard to read. In your homework reports you need to include figures with readable text. Pay attention to this detail. 45
Step 30: As a final visualization let s plot the x-velocity profile at the exit plane. Double click XY Plot. Select Velocity and X Velocity for the variable to be plotted. Select the already available outlet from the Surface list. Change the Plot Direction as shown below (this is necessary because now we plot something against the vertical y axis. Kind of puzzling, I know) Press Save/Plot. Note: As seen above there is the Write to File. With this option you can write the numerical values of the extracted data and study it whenever you want. If you want, you can plot it with another software like Excel or MATLAB. 46
The generated exit velocity profile is shown below. As expected the fully developed velocity profile is parabolic. Analytical solution of the fully developed part of this problem would give the maximum centerline value of the parabolic profile as 1.5U inlet = (1.5)(0.025) = 0.0375 m/s. What we calculated here is 0.0373 m/s, which is only 0.5% off. To Do: The horizontal axis name shown above is Position (m), which is not very informative. It would be better if it says y (m). Can you change that? Also it would be better if we interchange horizontal and vertical axes variables of this plot, i.e. velocity on the horizontal axes and y coordinate on the vertical axes. Can you change that? Note: All the plots we generated can be seen under Results. You can right click and edit them as you want. 47