CFD Solutions Using Pointwise Generated Grids

tamu-B-badgeStudents at Texas A&M University use Pointwise to generate a wide variety of mesh types to support research on various CFD solvers and applications. 


Forrest Carpenter, Raymond Fontenot, and Paul Cizmas
Aerospace Engineering, Texas A&M University

I. Introduction

As a part of our research activities, Pointwise has been utilized by various members of the research group led by Dr. Paul Cizmas at Texas A&M this past year. Pointwise has added value to our research by providing expeditious, quality mesh generation capabilities that would otherwise not be readily present. Having Pointwise allows us to spend less time and energy in generating CFD meshes and more time working on solving our research questions. Pointwise has been used to mesh a number of different geometries spanning a wide range of aerodynamic flow conditions. The different cases for which Pointwise has been applied are now presented.

II. AggiE_Challenge Wind Tunnel Ramp Model

The AggiE_Challenge program at Texas A&M is a unique opportunity for undergraduate engineering students who wish to experience engineering research first hand. Students work on faculty directed research while also receiving credits that are applied towards their degree plans. As a part of one AggiE_Challenge project being administered by faculty in the Aerospace Engineering depart, the students were challenge to design a
shape memory alloy (SMA) actuated model to be place in a supersonic wind tunnel. The students ultimately chose a variable, double-ramp setup which could produce both oblique shocks and expansion waves.

A viscous CFD simulation was requested as a part of the initial sizing process for the SMA torque tubes, and to examine what affects the gaps between the plates would have on the loading. Pointwise was utilized to build a two-dimensional, structured mesh of the
domain. The boundaries of the full computational domain are shown in Fig. 1. A total of 16,680 nodes were used to discretize the domain shown in Fig. 1.

The most challenging aspect of gridding the shown computational domain was in gridding the two small cavities, which represent the space between the hinge and the ramp plates. Figure2 shows two views of the computational grid of the upstream cavity.
The downstream cavity was gridded in the same manner as the upstream cavity, and is therefore not shown for brevity.

The Pointwise generated mesh was used in conjunction with Fluent to simulate the Mach 2 flow over the double ramp system. Both ramps were set at an angle of ten degrees, measured from the tunnel floor. Figure 3 shows a sample of the results obtained from Fluent in the form of Mach number contours. The use of Pointwise allowed for a quick turnaround on fulfilling the CFD request by the undergraduate students, and allowed them to confidently zero in on a final design of their wind tunnel model in a timely manner.


Figure 1. AggiE_Challenge initial supersonic wind tunnel double ramp model CFD domain 


Figure 2. Structured CFD mesh of the hinge cavities found in the initial AggiE_Challenge supersonic wind tunnel double ramp CFD model. (Left) Full cavity mesh. (Right) Cavity mesh detail.


Figure 3. Mach contours of the initial AggiE_Challenge supersonic wind tunnel model

III. NASA Axisymmetric Body 25D

One of the ongoing research projects in our research group is a NASA project with the ultimate goal for the development of an aircraft structure that changes in-flight to minimize the sonic boom signature. Our research group focuses primarily on the near-field simulation of the supersonic flow around the airframe. The first geometry we looked at was the NASA Axisymmetric Body 25D, which had a Mach 1.6 operating condition at an altitude of 15.76 kilometers.

Pointwise was used to generate an inviscid grid on one half of the meridional plane. The domain was aligned to the Mach angle and radially extended fifteen body lengths away. A very fine meridional mesh was created in Pointwise and then sequentially coarsened by removing every other point to create a family of grids. Figure 4 shows the resultant coarse meridional plane mesh, which has been mirrored to fully show the profile of the body. Also shown in Fig. 4 is a detail of the leading edge region. The two-dimensional meridional meshes were then rotated about the x-axis using a from-scratch Fortran code. The purpose of the Fortran code was to account for the collapsed geometries at the leading and trailing edges that result from the rotation. These special geometries are not permitted by our in-house flow solver (UNS3D), and had to be specially treated by splitting the collapsed cells into two pyramidal elements. Figure 5 shows resultant mesh following the rotation, and also includes a detail of the leading edge element structure. Final node counts for the coarse, medium, and fine grids were 403,020, 3,147,883, and 24,880,581 nodes, respectively.

Using Pointwise for this problem allowed for total control of the point distribution in the base meridional mesh. The smoothing functions within Pointwise also allowed for a much higher quality base mesh, than one generated by hand using a simple algebraic mesh. As a result, the solutions obtained from the CFD simulations showed excellent agreement with the data provided by the 2nd AIAA Sonic Boom Prediction Workshop, as illustrated by Fig. 6.


Figure 4. Pointwise generated meridional plane mesh for the NASA Axisymmetric body geometry


Figure 5. NASA Axisymmetric Body computational mesh. (Left) Full computational mesh. (Right) Leading edge element layout. Element types illustrated are hexahedral (grey), triangular prisms (yellow), and pyramidal elements (blue). 



Figure 6. Variation of scaled pressure signal with grid size compared
 against the average sonic boom prediction workshop (SBPW2) data

IV. Conical Body in a Supersonic Flow

The case was developed from a need to quickly resolve some issues pertaining to the CFD boundary conditions that arose during the simulations of the NASA axisymmetric body. The grid generation procedure for this case was identical to that of the axisymmetric body, i.e. Pointwise+Fortran. To that end, Pointwise was used to generate the meridional mesh of a conical body with a 5.58° cone angle. For this case the meridional mesh was rotated only 90° as opposed to 180° for the NASA body. The resultant mesh contained 151,075 points, and can be seen in Fig. 7. Pointwise allowed for a quick turnaround in the mesh generation process to allow for the majority of the time to be spent working out the issues with the flow solver.


Figure 7. Conical body mesh

V. NACA 663018 Airfoil

This was a test case developed for the purpose of testing some adiabatic viscous wall boundary condition modifications that were made to our flow solver, UNS3D. This particular airfoil was chosen for the availability of experimental results at a low enough Reynolds number that the flow would be laminar. The Reynolds number, based on the airfoil chord, for this particular numerical experiment was 40,000.

Pointwise was used to generate the CFD mesh for this test case. A two dimensional C-grid was created around the airfoil and along the wake plane. This two-dimensional mesh was then extruded into the z-direction by one cell to create the “two-dimensional” mesh for our three-dimensional flow solver. In total, the full mesh contained 205,816 nodes. Figure 8 shows the full two-dimensional C-grid and a close up of the airfoil region of the C-grid.


Figure 8. NACA 663018 airfoil Pointwise generated C-grid. (Left) Full C-grid. (Right) Airfoil adjacent grid

VI. Unstructured 2D Domain for Gradient Evaluation Tests

This numerical experiment was completeda s part of the development of higher-order schemes for the implementation of a Large-Eddy Simulation (LES) version of our flow solver, and was designed to evaluate the order of the implemented gradient evaluation methods.

Pointwise was used to generate a two-dimensional, unstructured [0,1] 2 domain with outer node counts from 322 to 2562. Figure 9 presents the grid for the 2562 case. The edges of the domain are buffered with three rows of quadrilateral elements normal to the boundary, and the interior of the domain was discretized using the default unstructured algorithm in Pointwise. The quadrilateral buffer was created to define “ghost” values to complete the stencils used to compute the gradients.

A Gaussian function was used to test the order of the implemented gradient methods. Figure 10 shows the convergence results from this study. It is clear from the figure that the desired order of convergence was obtained as the grid was refined.

Pointwise was instrumental in generating the grids for this numerical experiment. While seemingly simple to make, the grid topology with structure/unstructured cells makes the mesh generation non-trivial. Using Pointwise, and a few clicks of the mouse, a usable grid was created in minutes. This grid generation time would be orders of magnitude faster than if it had been generated “by hand”.


Figure 9. 2562 unstructured two-dimensional mesh for gradient evaluation tests, with a zoomed detail of the bottom left corner of the grid


Figure 10. Order of convergence for the moving least squares (MLS) gradients computed on the unstructured Pointwise grids

VII. Pseudo-3D Inviscid Channel

This test case was developed to measure the amount of dissipation in the aforementioned higher-order version of our flow solver. The grid is shown in Fig. 11. The grid has the dimensions 30 x 60 nodes in the xz-plane and has either 4, 6, or 8 nodes in the z-direction for first/second, third, and fourth order computations, respectively. Figure 12 highlights the different boundary conditions applied in Pointwise to the computational domain. Note that the in-plane boundaries were set as periodic boundaries in an effort to minimize boundary influences due to corners. The grid distribution used was chosen to mimic a grid that would typically be used for a viscous flat plate topology. The freestream Mach number for this case was 0.75. Pointwise made it very easy to quickly create and distribute the grid points in the desired fashion.


Figure 11. Inviscid channel mesh for measuring dissipation in a higher-order flow solver


Figure 12. Boundary condition type placement for the inviscid channel mesh

[Editor’s note: Any and all typographical errors in this article are the fault of the translation of the original article into blog format. They are not the fault of the authors.]

From the editor:

Gain Meshing Flexibility with Pointwise

Do you have CFD computations for which a wide variety of mesh types are needed?

Now would be the time to give Pointwise a try for your CFD meshes. Request a free trial license today.





This entry was posted in Applications, Software and tagged , , , , , . Bookmark the permalink.

Leave a Reply

Fill in your details below or click an icon to log in: Logo

You are commenting using your account. Log Out /  Change )

Google+ photo

You are commenting using your Google+ account. Log Out /  Change )

Twitter picture

You are commenting using your Twitter account. Log Out /  Change )

Facebook photo

You are commenting using your Facebook account. Log Out /  Change )


Connecting to %s