All Courses
All Courses
Courses by Software
Courses by Semester
Courses by Domain
Tool-focused Courses
Machine learning
POPULAR COURSES
Success Stories
Aim: To simulate an external flow over an Ahmed Body in Ansys fluent. Objectives: To use the split body function in Ansys SpaceClaim to get the required symmetrical geometry of the Ahmed body along its length. Use appropriate enclosures around the Ahmed Body geometry to get the required mesh quality that enables proper…
Kapilesh K
updated on 27 Jun 2021
Aim: To simulate an external flow over an Ahmed Body in Ansys fluent.
Objectives:
Ahmed Body: Generally speaking, if a completely new vehicle is to be designed, the external aerodynamics of the vehicle would have high influence on the aerodynamic drag, fuel consumption, noise production and road handling. Usually, wind tunnel testing of a prototype of the new design is what was used in the earlier days to determine these parameters under consideration. But now, CFD can do the same without having to build a prototype and use expensive wind tunnel setups. However, the computational models are very large and even highly powerful computers may take a few days to get a solution. To reduce this time scale and get a reasonably accurate solution, simplified computational models are to be developed. Hence, to test the legitimacy of the new computational models and accuracy of the results obtained, the newly developed computational models are tested with the Ahmed body.
The Ahmed body is a highly simplified model of a four-wheel vehicle or in other words, it is a simplified car model. There is a lot of experimental data available for this particular geometry for external flows and many numerical analyses on the same is also conducted. Hence, this geometry can be used to validate the accuracy of results generated using a newly developed CFD solvers. At the same time, it is very useful to learn to simulate external flows over a typical car using any pre-existing solvers.
In our study, we are going to be studying the drag and lift coefficients of the Ahmed body. The following are the equations representing the drag and the lift coefficients:
Cd=2Fdρu2A
Cl=2Flρu2A
Where,
Cd --> Drag coefficient,
Cl --> Lift coefficient,
Fd --> Drag force,
Fl --> Lift force,
ρ --> mass density of the fluid,
u --> velocity of the object relative to the fluid,
A --> frontal reference area of the object moving through the fluid.
The CAD model for our simulation case is as follows:
The above pictures show the isometric and front views of the Ahmed Body.
An enclosure of the appropriate dimensions is used to contain the Ahmed body which will be our computational domain. The dimensions of the outer enclosure / our computational domain is as follows:
The length in front of the Ahmed body: 2 meters
The length at the back of the body: 5 meters
The length at the bottom of the body: 0.5 meters
The length at the top of the body: 1 meter
The above picture shows the isometric view of the enclosure around the Ahmed body.
Another inner enclosure within our computational domain is added, so that it can be used in the meshing controls to refine the area of interest.
The above picture shows the inner enclosure within our computational domain.
The interference region with the two enclosures is taken care of, by subtracting the smaller enclosure from the larger enclosure by using the Interference option in the Prepare section. And the inner Ahmed Body will be suppressed for physics as we are only running an external flow simulation and the gird will be generated only around the Ahmed body.
To reduce the element count, and the computation time, only the half the body along its length can be considered for our simulation and symmetry boundary condition can be used on the other side.
The above picture shows the domain after using the split body operation.
It is to be noted that share topology is set to share in SpaceClaim options.
Named Selections:
Inlet: The outer face in front of the Ahmed body is named as inlet.
Outlet: The outer face at the back of the Ahmed body is named as outlet.
Wall: All the faces of the Ahmed body itself is named as the wall.
Symmetry: The outer sides of the domain are named as symmetry.
Mesh: Following are the meshing options used to generate the mesh for our simulation.
A note on y+ :-
In order to capture the data around a body, especially in scenarios like external flows, it is important to maintain the near-wall grid sizes very small. The concept of y+ helps in estimating how small the near-wall mesh size needs to be.
The theoretical basis for estimating the near-wall mesh size based on the appropriate value for y+ is very well described in the following reference link: -
https://skill-lync.com/knowledgebase/boundary-layer-y-plus-wall-functions-in-turbulent-flows-2
For our simulation, the y+ value of 100 is chosen and with the appropriate values for free stream velocity, fluid density, dynamic viscosity, reference length and desired y+ value are given as the input for a y+ calculator found online, and the link to the online y+ calculator is as follows: -
https://www.quadco.engineering/en/know-how/cfd-calculate-wall-distance.htm
The input conditions are defined as follows:
5. Desired y+ is taken as 100
The above picture shows the inputs given and the output obtained in the aforementioned y+ calculator.
Therefore, we get the near-wall element size as 0.001415m
Solution setup: -
The frontal area was estimated using the method explained in the following link:
https://www.afs.enea.it/project/neptunius/docs/fluent/html/ug/node963.htm
The estimation of the rest of the reference values are explained previously.
6.The turbulent models were changed between k-omega and k-epsilon based on the test cases for different grid sizes.
7.The convergence criteria for the scaled residuals were kept at the following setting:
Case 1: Mesh grid one with k-omega turbulence model.
Mesh Gird 1:
The body sizing of the inner enclosure was kept at 0.05m and the following is the representation of the mesh:
The number of nodes and elements are 60832 and 190077 respectively.
The above picture is the representation of the Mesh 1.
The above picture shows the element metrics for Mesh 1.
The solution was initialized using Hybrid initialization and it was converged at 1093 iterations. The following are the plots and results for case 1.
The above plot shows the scaled residuals over the iterations.
The above plot shows the variation of the drag coefficient over the iterations.
The above plot shows the variation of the lift coefficient over the iterations.
The above image shows the velocity contour after the solution reached the convergence criteria.
The above image shows the pressure contour after the solution reached the convergence criteria.
The above image shows the distribution of vectors across the domain
For case 1:
The drag coefficient was found to be: 0.34643372
The lift coefficient was found to be: 0.22526553
Case 2: Mesh grid one with k-epsilon turbulence model.
Mesh grid one is as explained in case 1.
The solution was initialized using Hybrid initialization and it was converged at 947 iterations. The following are the plots and results for case 1.
The above plot shows the scaled residuals over the iterations.
The above plot shows the variation of the drag coefficient over the iterations.
The above plot shows the variation of the lift coefficient over the iterations.
The above image shows the velocity contour after the solution reached the convergence criteria.
The above image shows the pressure contour after the solution reached the convergence criteria.
The above image shows the distribution of vectors across the domain.
For case 2:
The drag coefficient was found to be: 0.35159591
The lift coefficient was found to be: 0.24069559
Case 3: Mesh grid two with k-omega turbulence model.
Mesh Gird 2:
The body sizing of the inner enclosure was kept at 0.035m and the following is the representation of the mesh:
The number of nodes and elements are 90487 and 354061 respectively.
The above picture is the representation of the Mesh 2.
The above picture shows the element metrics for Mesh 2.
The solution was initialized using Hybrid initialization and it was run upto 1200 iterations. The solution did not reach a converged state, but by looking at the plots for the variation in drag and lift coefficients (plots shown below), it was concluded that 1200 iterations was enough to get a stable result.
The following are the plots and results for case 3.
The above plot shows the scaled residuals over the iterations.
The above plot shows the variation of the drag coefficient over the iterations.
The above plot shows the variation of the lift coefficient over the iterations.
The above image shows the velocity contour after the solution was run for 1200 iterations.
The above image shows the pressure contour after the solution was run for 1200 iterations.
The above image shows the distribution of vectors across the domain.
For case 3:
The drag coefficient was found to be: 0.32348533
The lift coefficient was found to be: 0.24186634
Case 4: Mesh grid two with k-epsilon turbulence model.
Mesh Grid 2 is as described in the previous case.
The solution was initialized using Hybrid initialization and it was run upto 1200 iterations. The solution did not reach a converged state, but by looking at the plots for the variation in drag and lift coefficients (plots shown below), it was concluded that 1200 iterations was enough to get a stable result.
The above plot shows the scaled residuals over the iterations.
The above plot shows the variation of the drag coefficient over the iterations.
The above plot shows the variation of the lift coefficient over the iterations.
The above image shows the velocity contour after the solution was run for 1200 iterations.
The above image shows the pressure contour after the solution was run for 1200 iterations.
The above image shows the distribution of vectors across the domain.
For case 4:
The drag coefficient was found to be: 0.31234453.
The lift coefficient was found to be: 0.25320035.
Note: The grid was not further refined because the number of elements that would be generated would exceed the number of elements allowed in the Ansys student license.
Comparison of the different cases:
Ideally, the drag coefficient of the Ahmed Body under consideration is supposed to be 0.33. Keeping that value as the standard, the following comparisons are made with respect to the solutions obtained from the test cases.
Test case no. |
Description |
Drag coefficient |
Error Percentage |
Case 1 |
k-w model with Mesh 1 |
0.34643372 |
4.98% |
Case 2 |
k-e model with Mesh 1 |
0.35159591 |
6.52% |
Case 3 |
k-w model with Mesh 2 |
0.32348533 |
1.97% |
Case 4 |
k-e model with Mesh 2 |
0.31234453 |
5.35% |
From the above tests, the only reasonable conclusion we can infer is that fact that the error percentages are lesser when k-w turbulence model when compared with the k-e turbulence model. The error percentages are less enough to consider the legitimacy of the solutions obtained. Future scope of the same study could be that a finer grid may be used to run the exact same test cases, which would eventually lead to better results.
Note on flow separation and the negative pressure in the wake region:
Before understanding the flow separation and the point of separation, the boundary layer theory is to be understood.
Boundary layer theory: When a fluid flows over a plate, the velocity of the near most layer of the fluid is zero, relative to the plate. And the velocity of the subsequent layers keeps on increasing until the magnitude is equal to that of the free stream velocity. The boundary layer can be viewed as the thin layer of the fluid along the surface of the plate where the effect of viscosity is present, and the vorticity is also seen. The thickness of the boundary layer is said to be the distance between the plate and the layer of fluid until the velocity of the fluid layer has reached to about 99% of the free stream velocity. The following picture depicts the growth of a boundary layer on a flat plate.
The above picture shows the growth of the boundary layer on a flat plate.
Flow separation or boundary layer separation is the detachment of the boundary layer from the surface into a region of recirculating flow immediately a body that is in relative motion with the fluid. When there is a large enough adverse pressure gradient, the boundary layer gets separated and the speed of the boundary layer relative to the surface will be stopped and will have reversed direction. The flow will be detached from the surface and it becomes eddies or vortices. This phenomenon would cause the negative pressure in the wake region and hence, the flow separation results in the reduced lift and an increased pressure drag.
Leave a comment
Thanks for choosing to leave a comment. Please keep in mind that all the comments are moderated as per our comment policy, and your email will not be published for privacy reasons. Please leave a personal & meaningful conversation.
Other comments...
Simulating Rayleigh-Taylor instability in Ansys Fluent.
Aim: The aim of this project is as follows: To discuss about the about the different CFD models that are based on the mathematical analysis of Rayleigh Taylor instability. Perform three different cases of CFD simulation of Rayleigh Taylor instability using Ansys Fluent. Discuss about Atwood number and how it affects the…
20 Oct 2021 08:21 AM IST
Simulating Conjugate Heat Transfer (CHT) analysis in an exhaust port using Ansys Fluent.
Aim: To simulate a conjugate heat transfer analysis in an exhaust port. Objectives: To set the mesh for exhaust port geometry with the appropriate y+ considerations and it is a conforming mesh between the solid and fluid components. To set up the test case in Ansys Fluent with appropriate boundary condition, run the solution…
29 Sep 2021 02:52 AM IST
Simulating an external flow over an Ahmed Body in Ansys Fluent.
Aim: To simulate an external flow over an Ahmed Body in Ansys fluent. Objectives: To use the split body function in Ansys SpaceClaim to get the required symmetrical geometry of the Ahmed body along its length. Use appropriate enclosures around the Ahmed Body geometry to get the required mesh quality that enables proper…
27 Jun 2021 05:27 PM IST
Week 2 - Flow over a Cylinder.
https://skill-lync.com/projects/to-study-the-flow-over-a-cylinder-and-von-karman-vortex-street-in-ansys-fluent The above link leads to the project file that solves for the given assignment.
10 Jun 2021 06:45 AM IST
Related Courses
Skill-Lync offers industry relevant advanced engineering courses for engineering students by partnering with industry experts.
© 2025 Skill-Lync Inc. All Rights Reserved.