VisualCFD OPERATING INSTRUCTIONS
The Governing Equations that form the basis of every VisualCFD analysis are derived from the Euler equations for inviscid and compressible subsonic and supersonic flow . The Euler equations are three-dimensional and time dependent but have been modified for 3-D axisymmetric and 2-D planar flow. The methodology quickly captures shock waves within 1 to 2 spacial cells depending on the flux differencing scheme used.

1) DEFINE BASIC PROPERTIES

In the Fluid properties section define the following parameters.
a) Insert , the ratio of specific heats of the fluid medium being investigated. The variable permits the user to specify any type of fluid medium for analysis. The default value of is 1.4 for air. Any value for may be inserted for the analysis of any type of fluid medium.

b) Select the flight altitude for the analysis. The selection of flight altitude establishes the free-field pressure and density of the fluid. Any incremental altitude from sea level to 150,000 feet may be defined as the flight altitude for the project.

c) Select the basic "Units" of the project. This selection determines the system of units that will be used to define the length dimensions (diameter, length) of the model to be generated.

d) Insert the Free-Stream Mach number for the flow field being investigated. The Free-Stream Mach number is the ratio of free-stream velocity to the local speed of sound (C). The default value is Mach 2.0, but can be set to Mach numbers in the compressible subsonic (0.3M - 0.8M), transonic (0.8M - 1.2M), supersonic (1.1M - 5.0M) and hypersonic (> 5.0M) ranges. The value inserted for Free-Stream Mach number is converted and displayed as velocity in mph and velocity in the basic units of the program. The basic units of the program were established earlier when "Units" were selected in step 1(c).

e) Insert the angle of attack, of the model in free flight. Angle of attack is defined as positive for flow approaching from below and in front of the model in free flight. Standard vector analysis convention for the definition of the angle of attack and physical location on the surface of the model is used in VisualCFD. Positive or negative angles of attack may be inserted for . However, because the geometry is axisymmetric the results for positive and negative angle of attack are identical when the solution is converged.

2) DEFINE MODEL GEOMETRY

In the Generate Geometry for CFD Analysis section define the shape of the body under investigation. The geometry of the model is defined by selection from up to five basic shapes provided by VisualCFD in any linear combination and then providing the dimensions required for each section. Specifically, the user may select Nose Cone, Body Tube-1, Transition, Body Tube-2 and Boat Tail transition sections in any combination by selecting the cross-box corresponding to the section required by the geometry. The user combines these geometrical shapes to construct the geometry of the model under consideration. The user may also select one of five nose cone shapes that include Conical, Tangent Ogive, Sears-Haack with power series shape control, Elliptical and Parabolic. In addition, the user can specify the Transition and Boat Tail sections as either Tangent Ogive, Elliptical, Parabolic, and Conical with power series shape control. The Conical section with shape control index = 1 produces a pure conical section while any other index produces a power series shape as in previous versions of VisualCFD. A simple pull-down menu selects the shape for use in the definition of the geometry. The geometry definition for the project is complete when the dimension box of each visible cross-sectional shape is defined. In addition, transition shapes have a power series shape control for defining very unusual 3-D axisymmetric shapes and 2-D shapes.

Parabolic Nose Cone Geometry: VisualCFD uses the standard mathematical equation for a parabola aligned with the x-axis to define the geometry of a Parabolic nose cone as follows: y^2 = 4 * P * x. Where, P is the focus of the parabola that opens to the right and x and y determine the shape of the parabolic nose cone. P is determined from the point (x = Lnose, y = Dnose / 2), where P is calculated from the equation above. Therefore, P = y^2 / (4 * x) = (Dnose/2)^2 / (4 * Lnose) = Dnose^2 / (16 * L nose) and y [x] = 2 * sqr(P * x), is the equation that determines the shape of the Parabolic nose cone. The other nose shapes are derived in a similar manner.

Transition Section Geometry: The equation to define the geometry of a conical transition with shape coefficient in VisualCFD is a follows: y[x] = D1/2 + (x/LT)^n * (D2 - D1)/2. Where D1 is the diameter before the transition, D2 is the diameter after the transition, LT is the length of the transition, x is measured from the start of the transition and y[x] describes the vertical height of the surface from the centerline. n is the shape coefficient when equal to 1.0 allows the equation to describe an ordinary conical transition section. The other transition shapes are derived in a similar manner.

VisualCFD Geometry Import Feature. The user can import up to 1,000 X-Y airframe geometry points from a text file previously saved using the TXT delimiter. When initially reading a shape first click File then Import Shape to input the previously saved airframe geometry. Then, in VisualCFD define the flow and mesh parameters and save the project file by clicking File then Save Project As. Subsequently, to run a project and its associated shape the shape file is imported first and then the project file is opened. Running a previously saved shape-project is performed by first clicking File then Import Shape and finally by clicking Open Project. Please wait for the shape and mesh parameters to be generated before performing each step. The data has the following format. First line: Total number of X-Y point locations. Second and subsequent lines: X, Y airframe locations separated by commas. A VisualCFD shape file defines the upper contour of an axisymmetric airframe geometry starting from nose-tip to the end of the airframe. Please see an example of using a shape file for the analysis of a supersonic spherical blunt-body.

3) MESH GENERATION

The Mesh control parameters section is used to define the parameters that control the spacing and distribution of the mesh around the body. To achieve a successful CFD solution the user needs to define the mesh or system of grids defining the flow field around the model under investigation. In many cases an inappropriate selection of parameters in this section will cause VisualCFD to fail almost immediately often in less that 5 iterations after the user clicks the SOLVE button. For example, the mesh distribution appropriate for a successful supersonic flow CFD analysis is probably completely inappropriate for a successful subsonic flow CFD analysis. However, by following a few simple conventions a good solution can be achieved after a few attempts.

The step-by-step instruction to generate a mesh for the CFD analysis follows:
a) Define the solution domain as either 3-D axisymmetric flow or 2-D planar flow by selecting the option button corresponding to either Axisymmetric Flow (3D) or Planar Flow (2D). The outline of the shape to the right of the menu represents half of the model and the bottom X-axis of the coordinate system is the centerline of the flow field under investigation. For 2-D flow starting with VisualCFD version 3.5.1, only the upper cross-section (above the centerline) is displayed and resultant force and moment coefficients are based on the shape above the x-axis (centerline).

b) Include base drag effects by selecting either the NASA TR R-100 method or the Hoerner Drag method using the two option buttons. The NASA TR R-100 method is based on the three-dimensional Base-Pressure Coefficients (Cp) data displayed on page 10 of the report. The base pressure coefficient (Cp) verses Mach number curve is used to define base pressure drag (CDB) as a function of Mach number and base geometry. This method has proven highly accurate for subsonic, transonic and supersonic flow of projectile-like bodies in compressible flow. The second option, the Hoerner Drag method is based on the theory presented in Fluid Dynamic Drag, by S.F. Hoerner. This method is better suited for subsonic and transonic flow to Mach 1.5 but has proven accurate to Mach 4 on occasion. For more discussion about these two methods please refer to section 7e of the instructions.

c) Select the number of cells along the X-axis or flow direction as either 40 cells, 50 cells or 60 cells. This parameter represents the total number of cells that are distributed along the X-axis of the flow field under investigation. How the grid points are distributed in the X-direction is determined by the distance before the nose tip and the total number of grids before the nose tip. Grid clustering is achieved by manipulating the distance before the nose tip and the total number of grids before the nose tip.

d) Select the number of cells along the Y-axis or up direction as either 10 cells, 20 cells or 30 cells. This parameter represents the total number of cells that are distributed along the Y-axis of the flow field under investigation. How the grid points are distributed in the Y-direction is determined by the distance of the first point up from the surface. Grid clustering near the surface of the model is required to capture the rapidly changing flow field pressure and flow field density around a subsonic and supersonic model under investigation. Make the value of the distance of the first point up from the surface as small as possible without depriving the rest of the flow field of the number of grid points necessary to achieve convergence to a proper solution.

e) Select the number of grid points in the circumferential direction of the model as either 4 cells, 5 cells or 10 cells. For best results the default value of 10 cells in the circumferential (3-D direction or thickness (2-D) direction works best. However, faster execution time can be achieved by using 4 or 5 cells.

f) Insert the number of grid points before the tip of the nose cone from as few as 3 grid points to as high as 10 grid points. Selection of the number of grids before the nose cone and the distance from the origin to the tip of the nose cone determine proper grid clustering. Manipulate these two values to yield a smoothly changing grid distribution that is small near the nose cone tip and increases slightly toward the rear of the model where fewer grid points are required.

g) Define the Aspect Ratio of the flow as either 1:1, 2:1, 3:1 or 4:1 by selecting 1, 2, 3, or 4 from the pull down menu for Aspect Ratio. The selection of Aspect Ratio is one way to cluster the grid points near the surface of the model away from a region where the grids are being wasted. Normally, an Aspect Ratio of 1:1 is fine for most analyses but 2:1 may be useful in some cases and in extreme situations an even higher Aspect Ratio may be necessary.

h) Insert the distance before the tip of the nose cone from the origin of the flow field. For supersonic flow the X-distance from the origin to the tip of a pointed nose cone can be small because the shock wave is attached to the nose cone tip and the region before the nose cone is not effected by the flow field around the model. In the case of supersonic attached-shock flow, the distance to the nose cone tip can be very small because the region before the nose cone is essentially free-field or the fluid conditions at infinity. However, a blunt nose cone requires a much greater distance from the origin to the tip of the nose cone because a detached shock wave is present. Also, subsonic flow requires a larger distance before the nose cone tip not because of any shock wave but because the physical information is being transmitted upstream from the nose cone. More distance is required to capture the bow wave of any subsonic flow field. For subsonic or blunt supersonic flow the distance before the nose cone tip is on the order of to 1 body diameter. For supersonic attached-shock flow the distance from the origin to the tip of the nose cone can be very small possibly on the order of 0.15 inches or the default value for this distance in the program.

Selection of the number of grids before the nose cone and the distance from the origin to the tip of the nose cone determines grid clustering. Manipulate these two values to yield a smoothly changing grid distribution that is small near the nose cone tip and increases slightly toward the rear of the model where fewer grid points are required.

i) Clustering Mesh in the Y-Direction: Insert the distance of the first grid point up from the surface of the model. Y-grid clustering near the surface of the model is required to capture the rapidly changing flow field pressure distribution and flow field density distribution around a subsonic and supersonic model under investigation. Make the value of the distance of the first point up from the surface as small as possible without depriving the rest of the flow field of the number of grid points necessary to achieve convergence.

k) For two-dimensional flow insert the total width of the body for Total model width for 2-D flow. This entry is used for 2-D flow and is subdued or non-active for 3-D axisymmetric flow.

4) SOLUTION CONTROLS

To control how VisualCFD solves the flow around the body, define the following parameters in the Solution control parameters section.
a) Select one of the flux differencing schemes listed in the Flux Differencing Method sub-section. Accurate solutions of flows dominated by shock waves have been obtained by using a class of algorithms referred to as upwind or flux-split. These methods utilize finite volume differencing procedures that analyze the flow field in directions determined by the signs of the characteristic speeds or eigenvalues of the fluxes. These methods have been shown to yield similar results for subsonic, transonic and supersonic flow. However, the Steger and Warming flux-vector split scheme has been shown to capture shock waves in as few as two mesh points. By comparison, the Roe flux-difference methods have been demonstrated to capture shock waves over a range of as few as zero mesh points.

Therefore, for supersonic flow, better resolution of shock wave formation may be achieved using the Roe flux-difference-split method. In addition, the Roe flux-difference-split method is less dissipative than the Steger Warming flux-vector-split method and reaches a converged solution slightly slower than the Steger Warming method. The best overall flux differencing method is the Roe flux-difference-split - Flux limit method 3 and is the default flux-splitting method used in VisualCFD. This method gives the best results over the entire speed range from subsonic flow to hypersonic flow.

b) Insert the numerical order of the CFD analysis. For best results use the default numerical order, 2 for subsonic flow, transonic flow, supersonic flow and hypersonic flow. In general, the lower the numerical order the less converged a solution is compared to higher numerical order solutions at the same total number of iterations. However, a lower numerical order may be capable of arriving at a solution, even an incorrect one, while a higher order solution may not be able to even start iteration due to numerical instability.

c) Insert the total number of iterations. Typically a solution is considered converged when the pressure change per iteration reaches the level of approximately 1.0E-4 or about 3 orders of magnitude less that the initial pressure change residual. The other residuals will converge less slowly. Convergence to an engineering solution (5% error) is dependent on Mach number, angle of attack and model geometry and typically takes about 100 to 500 iterations using the default settings.

d) Insert the CFL or Courant number. The CFL variable is used to determine the maximum time step allowed for local time stepping. Local time stepping uses the maximum allowable value of for rapid convergence to a steady state solution. The CFD solution is not time accurate but convergence is greatly accelerated for a steady state solution. On the other hand, minimum time stepping allows calculations to be time accurate but converge very slowly to a steady state solution. Most engineering solutions of streamlined bodies do not require time accuracy when computing Cd, CL and the other coefficients of high speed flow. However, vortical flow analysis requires time accuracy to determine the vortex pattern as it changes around the body with time. Most high speed analyses of streamlined bodies do not exhibit changing vortical patterns and therefore time accuracy is not required. The default value of CFL for a local time stepping analysis is 10.0 but typically CFL should range from 2.0 to 10.0 depending on the angle of attack, Mach number and model geometry or nose bluntness. Simply reduce the CFL if convergence appears to be a problem.

e) Click SOLVE to start the CFD analysis. After completion of the analysis the user may plot results to graphically analyze the data. However, if the solution is not converged the user may restart the analysis simply by clicking the SOLVE button again. If no modifications are made to model geometry and flow field parameters, VisualCFD starts where it left off with the last iteration of the previous analysis. The iteration counter picks up where it left off and continues counting and terminates when the new solution is completed. This process may be repeated until convergence is achieved or the desired level of convergence is reached.

f) Convergence Plot Controls are provided to give the user some feel for the level of convergence of the CFD solution. By clicking Hide/Show Curve Plots the user may hide or show the plots of convergence residuals as they change from iteration to iteration. The most important residuals to watch are the Pressure Change Per Iteration, Maximum Density and Maximum Energy. A solution is converged when the residuals are reduced three or four orders of magnitude (1.0E-03) and stay at that level for about 20 iterations. However, the most important convergence criterion for an engineering solution is the Pressure Change Per Iteration residual. This residual represents the overall flow field change in pressure (P/Pinf) between iterations. When the pressure residual reaches 1.0E-03 an engineering solution has probably been achieved and convergence has been attained.

5) FIN GEOMETRY (OPTIONAL)

To add fins to the model enter the Free-Form Fin Geometry screen by clicking on the Add fins to body icon on the main toolbar. Then, perform the following operations.
a) A gray outline of the body will appear along with bold red X and Y lines that form the x-y coordinate system of the fin definition screen. To define the fin plot region size, number of fins, fin thickness, and fin cross-sectional shape click the fifth icon from the left on the tool bar at the top of the screen to expose the View Fin Parameter screen. First, the Plot-Region of the fin must be defined before the user can drag the points into position. The fin plot region is defined as a box that will enclose the fin and all the shape points that will define the fin shape. The "Plot-Region location from nose tip" is the first entry in the Plot-Region Dimensions section. The "Plot-Region height and width" are defined in the next data entry in the Plot-Region section. The first data entry specifies where the Plot-Region is positioned down the axis of the body and the next data entry specifies the size of the Plot-Region used to define the fin geometry.

b) Next, in the Fin Cross-Section Dimensions section, insert the Total number of fins, Maximum fin thickness and if required by the cross-section-type the location of the Maximum (fin) thickness location as a percent of the fin chord length. At this point if all dimensions are properly defined a simple outline of the fin shape, not to scale, is presented in the Fin Plot-Region section.

c) To define a specific fin cross-sectional shape select one of the seven options listed in the pull down menu at the upper right of the Free-Form Fin Geometry screen. The fin cross-sectional shapes available include: Double Wedge, Symmetrical Double Wedge, Double Wedge: TMAX=FN(X/C), Biconvex Section, Streamline Airfoil: X/C=50%, Round Nose Airfoil: X/C=50%, and Slender Elliptical Foil. Depending on which cross-sectional shape is selected a different leading edge factor (KLE) will be computed for supersonic flow. For subsonic flow the KLE is ignored and the drag and lift coefficients are based on subsonic derivations.

d) The KLE Leading edge factor, Fin area, Reference area of the model, fin Sweep angle, Average chord and Semi-span are computed and displayed in the Cross-Section Dimension Results section.

e) Click back to the Free-Form Fin Geometry screen by re-clicking the View Fin Parameter screen icon and proceed to "drag" the shape points into position to define the fin shape. The SHOW and HIDE plot legend contains an Up-Down control that will increase and decrease the number of shape points from the default of 4 shape points to a maximum of 20 shape points. To expose the Show and Hide plot legend, click the sixth icon to expose or hide the control. A color legend also appears that provides a color guide indicating the Fin Shape (Black), Body Tube Shape (Gray) and X-Y Axes (Red) of the Plot-Region. Two sets of coordinates are available to help the user rapidly position the shape points. The first set of X and Y coordinates indicates the position from the origin (0,0) of the Plot-Region to each point on the screen. The second set of coordinates, XFIN, YFIN indicates the position of the cursor and shape points from the surface of the body itself (XFIN = 0, YFIN = YBODY).

f) A summary of the total drag, lift, axial and normal force coefficients for all fins is displayed in the Fin Drag Coefficients section. These results represent total values for all N fins defined by the user. The Fin drag and lift results are superimposed on the VisualCFD results computed in the main section of the analysis. Methods of superposition and fin interference effects techniques are employed to determine total lift and drag effects of the fins on the body. Fin flow field effects and interference with the body are ignored because a complex 3-dimensional mesh would be required to define the endless variations required for most complex fin designs. However, a good engineering estimate of aerodynamic coefficients of a body with fins is achieved using this fin superposition methodology.

g) A separate Fin CFD analysis is available for determining the pressure distribution (P/Pinf), pressure coefficient distribution (Cp), Mach number distribution (Mn), density distribution (R/Rinf) and temperature distribution (T/Tinf) on the surface of thin fins. This capability is not part of the finite volume analysis output.

b) To generate a surface distribution plot select one of the five fluid dynamic parameters available for plotting in the Surface Parameter Distribution section. The five fluid dynamic parameters include: Cp, P/Pinf, T/Tinf, MACH (Uinf/ Cinf) and R/Rinf. Two plots are available for plotting surface distribution plots. First, fluid dynamic parameter verses meridian location (3-D) or thickness location (2-D) at each axial position on the body. Second, fluid dynamic parameter verses axial position at each meridian location (3-D) or thickness location (2-D) on the body. This section gives the user a complete understanding of how the fluid dynamic parameters vary along the surface of the body in the axial and circumferential directions.

c) The Plot Options command adds eight more options for plots generated in the Surface Parameter Distribution section. These eight options are available in the tool bar at the top of the section. The options include, Open experimental data, Remove data points from plot, Delete X-Y experimental data points, Plot experimental data points, Decrease Y plot scale, Increase Y plot scale, Preview and print results, and finally, Save experimental data. Using these eight commands experimentally derived data can be added to the plots in this section for comparison of VisualCFD results and the experimental data.

Print airframe surface Cp, P/Pinf, R/Rinf and T/Tinf, by specifying the airframe surface location in the Surface Parameter Distribution section. To print axial data set the meridian location from 0.0 degrees to 180 degrees. Then, click File, Print Data and Axial Data to print all the surface data along the meridian from the tip of the nose to the end of the rocket. Print the data on the circumference of the airframe by selecting the axial location in the Surface Parameter Distribution section. Then click File, Print Data, Angular Data to print all the data along the circumference of the rocket at the axial location selected.

d) VisualCFD results for forces and fluid dynamic coefficients are located in the Forces and Coefficients section of the Plot Results screen. The result of forces in the X, and Y directions and pitch moment around the Z axis are labeled as FX, FY, and MZ respectively. The displayed units reflect units initially selected by the user. The drag coefficient (CD) in the direction of flight and lift coefficient (CL) perpendicular to the direction of flight are displayed next. Then, the axial coefficient (CX), normal coefficient (CY), pitch moment coefficient (CM) and base drag coefficient (CDB) are displayed. Finally, the surface friction drag coefficient (CDF) and center of pressure location (XCP) normalized by the total body length are displayed.

In the Forces and Coefficients section CD represents the total drag coefficient of the rocket which includes wave drag for supersonic flight, pressure (profile) drag for subsonic flight, airframe surface friction drag (CDF), airframe base drag (CDB), wave drag of the fins for supersonic flight and friction drag of the fins. For a listing of fin axial coefficient (CX), fin normal coefficient (CY), fin drag coefficient in the direction of flight (CD) and fin lift coefficient perpendicular to the direction of flight (CL), please see the Free-Form Fin Geometry screen.

e) VisualCFD solves the inviscid Euler equations. Therefore, the CFD solution does not include base drag directly in the Euler analysis. If three dimensional viscous effects were modeled directly using the full Navier Stokes equations, total execution time would be on the order of days and not minutes and the accuracy would not be much better. One of following two methods are used to determine airframe base drag (CDB). Base drag is a function of friction drag on the surface of a body where the surface boundary layer acts like a "jet-pump" that serves to reduce the static pressure at the base of the rocket. In other words the jet-pump, placed like a tube around the base of the rocket, mixes with the circulating flow in the base region. High speed mixing of the jet-pump and the base region "pumps" air away from the base thus reducing the pressure at the base of the airframe. The jet-pump's ability to reduce base pressure (Cp_base) and therefore effect base drag coefficient (CDB) depends on the ratio, (Dbase / Dbody)^3 . Where Dbase is the diameter at the base of the boat tail and Dbody is the diameter of the body just before the boat tail transition.

Method 1: From NASA TR R-100 a curve of three-dimensional Base-Pressure Coefficients (Cp_base) verses Mach number has been digitized to allow interpolation between values of Cp_base and Mach number to determine base drag coefficient (CDB) for subsonic, transonic, and supersonic flow. The curve used is displayed on page 10 of NASA TR R-100. The equation describing base drag coefficient is: CDB = Cp_base * (Dbase / Dbody)^3. This method is more accurate than Method-2 when Mach number is greater than 4.

Method 2: The base drag coefficient (CDB) is determined from the surface friction drag coefficient (CDF) using the following empirical relationship for laminar and turbulent flow: CDB = 0.029 / SQRT(Cfb) * (Dbase / Dbody)^3. Where Cfb is equal to the forebody drag coefficient (CDF) and Rn is the Reynolds number. CDB ranges from 0.025 to 0.20 for most conventional designs. Note: For turbulent boundary layer flow CDF can be estimated to be a function of Mach number, Reynolds number and body shape. These relationships are highly accurate for subsonic and transonic flow to about Mach 1.5, but accurate results to Mach 4 have been obtained. This method is described in more detail on pages 3-19 to 3-20 and pages 16-4 to 16-6 of Fluid-Dynamic Drag, by S.F. Hoerner.

f) VisualCFD solves the inviscid Euler equations. Therefore, the CFD solution does not include airframe/fins surface friction drag directly in the analysis. The surface friction drag coefficient (CF) for turbulent flow is determined from the flat plate formula as follows for airframe and fins: CF = 0.455 / LOG10(Rn)^2.58) / MCORRECT * AWET / AREF. For laminar flow the following empirical relationship is used to determine the surface friction drag coefficient for airframe and fins: CF = 1.328 / SQRT(Rn) * AWET / AREF. Where Rn is the Reynolds number based on total body length or fin chord, AREF is the reference area of the body based on the maximum cross-sectional area and AWET is the wetted surface area of the body or fins. The transition from laminar to turbulent flow is determined when the Reynolds number exceeds 500,000 for either the body or the fins. Finally, MCORRECT is the Mach number correction and is given as MCORRECT = (1 + 0.144 *M^2)^0.65.

g) VisualCFD analysis results may be saved and input at a later time using two commands in the File menu. To save the resulting flow properties and aerodynamic coefficients click File then select CFD Results and then select Save CFD Results to save the output file to the hard drive. To input the CFD results at a later time open the project file and shape file (if necessary) that correspond to the CFD analysis output results. Then, click File then select CFD Results and then select Input CFD Results to input the data required to plot and display flow properties around the object. The so called output file is saved using the .OUT extension and has the following format.

OUTPUT FILE (.OUT) FORMAT
FLOW FIELD DIMENSIONS (AXIAL-X, VERTICAL-Y, CIRCUMFERENTIAL OR THICKNESS-Z)
NI, NJ, NK

FLOW PROPERTIES AROUND AIRFRAME
I = 1 To NI: J = 1 To NJ: K = 1 To NK
X(I, J, K), Y(I, J, K), Z(I, J, K), P(I, J, K), RU(I, J, K), RV(I, J, K), RW(I, J, K), R(I, J, K)
NEXT K: NEXT J: NEXT I

AIRFRAME PRESSURE COEFFICIENT AND PRESSURE RATIO
I = 2 To NI: J = 2 To NK
CPBODY(I, J), PBODY(I, J)
NEXT J

DISTANCE FROM AIRFRAME TIP
XNOSE(I)
NEXT I

FORCES, COEFFICIENTS AND MOMENTS
FX, CX, FY, CY, CD, CL, MZ, CM, XCP

Where, P = P / (r₀₀ a₀₀²), R = r / r₀₀, U = U / a₀₀, V = V / a₀₀, W = W / a₀₀ and a₀₀ = (g P₀₀ / r₀₀)^1/2. Bold variables are dimensional flow field quantities and "oo" refers to free field flow. More detail of the Euler Governing Equations are available here and in the AeroRocket reference books.




7) VisualCFD VALIDATIONS AND TEST CASES BACK TO LIST
CASE #1: Drag coefficient (CD) as a function of Mach number for the V-2 rocket at 4 degrees angle of attack. Data from Figure 5-3 on page 126 of Rocket Propulsion Elements. Reference: Rocket Propulsion Elements, Sixth Edition, George P. Sutton.



V-2 rocket surface contour plot, AOA = 4 degrees, Mach number = 2.0



BACK TO LIST
CASE #2: Results from VisualCFD have been compared to free-flight data. Experimental data from the NACA report "FLIGHT INVESTIGATION AT MACH NUMBERS FROM 0.8 TO 1.5 TO DETERMINE THE EFFECTS OF NOSE BLUNTNESS ON THE TOTAL DRAG OF TWO FIN-STABILIZED BODIES OF REVOLUTION" by Roger G. Hart was used to validate the program from Mach 0.8 to Mach 1.5.




BACK TO LIST
CASE #3: Wave-drag coefficient verses Mach number for a 10% thick double-wedge wing section. 2-D VisualCFD results were compared to wind tunnel measurements from the following reference. Reference: Fluid-Dynamic Drag, by S.F. Hoerner, figure 9, page 17-10. Please note: VisualCFD frictional drag has been subtracted from total drag (CD) to compute double-wedge wave-drag based on wing area. The following formula was used to determine wave drag based on wing area from VisualCFD drag based on frontal area. Cd = CD * S_frontal / S_wing. To determine total force in the x-direction simply double FX from VisualCFD version 3.5.1. Also, drag (Cd) is nearly identical in VisualCFD version 3.5.1 as predicted in previous versions.




BACK TO LIST
CASE #4: 3-D Axisymmetric cone-cylinder-flare and NACA Report 1135 conical shock wave location analysis. Mach Number = 2.81, Angle of Attack = 0.0 Degrees, 60 X 30 X 10 Mesh, Solution Time 10 Minutes.

Cone Cylinder-Flare, Mach number field contour plot.



BACK TO LIST
CASE #5: The following X-30 NASP pressure (P/Pinf) contour plots were generated by a 2-D centerline analysis. Twenty separate VisualCFD analyses were performed at Mach 0.2, Mach 0.4, Mach 0.7, Mach 1, Mach 1.125, Mach 1.25, Mach 1.5, Mach 2, Mach 3, and Mach 5, angle of attack = 0.0 degrees at 150,000 feet. Each upper and lower analysis used a 60 X 30 X 4 clustered mesh for a total solution time of 3 hours for each Mach number. Cd verses Mach number results are presented below verses AeroWindTunnel results for the X-30 NASP. Also, presented below is an X-30 NASP Cd verses Mach number curvefit approximation generated from the VisualCFD results. These CFD analyses used imported 2-D shapes for the upper and lower halves of the X-30 NASP and were analyzed separately then combined in the color contour plots below. From the comparison of Cd verses Mach number of AeroWindTunnel and 2-D VisualCFD results it is evident the 2-D assumption is most valid for supersonic flow, M>1. This analysis requires VisualCFD 3.5.1

X-30 NASP CFD results for Mach 0.7, Mach 1, and Mach 1.25 at angle of attack = 0.0 degrees at 150,000 feet.
X-30 NASP CFD results for Mach 1.5, Mach 2 and Mach 5 at angle of attack = 0.0 degrees at 150,000 feet.
AeroWindTunnel (blue) vs. 2D VisualCFD results (red)	Curve Fit of 2D VisualCFD Cd vs. M Results (blue)	Theoretical 2D wave drag for M>1 vs. 2D VisualCFD results

BACK TO LIST
CASE #6: The following case illustrates the prediction of drag coefficient (Cd) verses Mach number for the Mars Phoenix entry capsule. VisualCFD was used to model the Mars Phoenix entry capsule for Mach numbers 0.25, 0.75, 1.0 and 1.5 at zero degrees angle of attack. Streamlined shapes like the V-2 rocket described in CASE 1 and the HART missile described in CASE 2 are capable of being operated well beyond Mach 10 using VisualCFD. However, blunt shapes with severe back-side transitions like the Mars Phoenix entry capsule are limited to subsonic and at most transonic (Mn < 1.5) flow conditions using VisualCFD because of the limited number of mesh points presently available. For speeds beyond Mach 1.5 more finite-volume cells are required to capture the time-dependant density variations that occur in separated base flows. In practice millions of cells are required to accurately model the separated flow in the base region for supersonic and hypersonic flow resulting in run times exceeding many days on a personal computer. However, VisualCFD models subsonic and transonic base flow quickly and for the Mars entry capsule converges to a solution within 45 minutes for the range of Mach numbers selected. In the Mars Phoenix entry capsule example presented below, only 400 iterations were required using a CFL equal to 5 to achieve convergence. In addition, VisualCFD predicts the time-dependant response of the flow field in the base region of the Mars entry capsule. To receive via email the subsonic and transonic VisualCFD project files for this example please contact John Cipolla at john@AeroRocket.com.


VisualCFD analysis of the Mars Phoenix entry capsule after 400 iterations at Mach 0.75 and zero degrees angle of attack. This is a full size screen shot of VisualCFD 3.6 with an image of the Mars capsule inserted.


HyperCFD analysis of the Mars Phoenix entry capsule using the modified surface inclination approximation method. Supersonic only.


VisualCFD and HyperCFD drag coefficient (Cd) verses Mach number results compared to empirical
data and equations derived by S.F. Hoerner in his book, Fluid Dynamic Drag.
 

8) TECHNICAL SUPPORT
For VisualCFD technical support please contact John Cipolla/AeroRocket at john@AeroRocket.com.

9) PURPOSE OF VisualCFD, AeroCFD and HyperCFD
VisualCFD is not a replacement for either AeroCFD or HyperCFD but is a sophisticated tool based on complex finite-volume CFD theory and is priced accordingly. First, AeroCFD is a model rocket Computational Fluid Dynamics (CFD) program whose operational speed allows rapid looping analyses that produce Cd, CN, CM and XCp as a function of angle of attack or velocity. AeroCFD is based on panel method techniques that are better suited for subsonic analyses of model rockets. AeroCFD is economically priced for the model rocketeer. Second, HyperCFD is a surface inclination CFD program better suited for the analysis of supersonic and hypersonic flight of high power rockets. Finally, VisualCFD at the low price of only $200 is an extremely accurate 2-D and 3-D CFD program. VisualCFD is based on the solution of the compressible Euler equations and is a sophisticated CFD program for the definition of aerodynamic characteristics of fin stabilized flight vehicles in subsonic, transonic and supersonic flow. However, VisualCFD is easy to use and represents a real price breakthrough.

10) VISUALCFD REVISIONS
VisualCFD 3.6.0.1 (September 15, 2009)
1) When operating VisualCFD in Windows Vista (32 bit and 64 bit) the instructions accessed by clicking Help, Operating Instructions then VisualCFD Manual displays the error, File not found, Error displaying VisualCFD Instructions. The fix for this problem is to make a shortcut copy of ShowHTML.exe located in the directory C:/Program Files (x86)/VisualCFD/ and locate the shortcut copy on the desk top.

VisualCFD 3.6.0.1 (November 14, 2008)
(1) Made contour plotting more flexible by making it possible to input different number of contour levels for line contours and filled contours when superimposing line contours on filled contour plot regions.
(2) Made VisualCFD more robust by solving the Run-time error '5': Invalid procedure call or argument error that occurred when VisualCFD models have base areas of subsonic recirculation and separated flow. The Mars Phoenix entry capsule described in CASE 6 is an example of CFD models having severe rear transitions where program stability will be enhanced by these modifications.

VisualCFD 3.5.0.1 (November 18, 2007)
(1) In versions prior to 3.5.0 VisualCFD 2-D forces and moments were based on the combined upper-shape and reflected lower-shape. However, VisualCFD never determined forces and moments on the lower cross-section for 2-D flow. Therefore, starting with this version only the upper-shape is displayed for 2-D analyses. This is valid because z-coordinates for 2-D flow are in the thickness direction while the equivalent dimension for 3-D flow is the Theta or circumferential direction. For these reasons 3-D axisymmetric analyses will continue to display the total upper and lower cross-sections while 2-D analyses will display only the upper cross-section. Also, in this version the following forces and moments will be now be displayed: FY, MZ, CL, CY, CM, and XCP in addition to FX, CD, CX, CDB, and CDF as before for 2-D flow. For 3-D flow all these force and moment coefficients will continue to be displayed as usual.

VisualCFD 3.5.0.0 (November 12, 2007)
(1) Previously, the angle of attack for 2-D flow was limited to zero degrees. This artificial limit has been removed allowing angle of attack for 2-D flow to be greater than (flow approaching from below the centerline) or less than (flow approaching from above the centerline) zero degrees.
(2) Improved overall speed response for 2-D and 3-D flows.

VisualCFD 3.0.0.2 (February 27, 2006)
(1) Titles below PLOT 1 and PLOT 2 were reversed relative to the axes specified in the Surface Parameter Distribution section.
(2) Added the Blunt Body example to the VisualCFDProject.zip example file.

VisualCFD 3.0.0.1 (October 22, 2005)
(1) Added the ability to cluster the mesh around the airframe by specifying the X-grid spacing at the tip of the airframe and at the end of the airframe. For Imported shapes only. This capability is vital for defining blunt shapes where the standard library of shapes is intended for pointed nose cones only.
(2) Solved the Run-time '94' error that occurred when alternating between standard geometry and import shapes or when reading incorrect project files. Fixed.
(3) Added the VisualCFDProject.zip file to the installation file where five example projects are installed to the VisualCFD directory.
(4) Corrected the built-in instructions locator to correctly link to the on-line VisualCFD instructions. Added several other links.
(5) Clarified various command buttons with the addition of tool-tip descriptions.

VisualCFD 2.8/2.9
(1) Added the ability to Import complex airframe shapes having up to 1,000 X-Y points for generation of more complex airframe designs.

VisualCFD 2.7
(1) Added the ability to generate Transition and Boat Tail sections having Tangent Ogive, Elliptical, or Parabolic shapes in addition to Conical shapes with shape control.

VisualCFD 2.6
(1) Added the ability to generate filled contour plots on the windward and leeward sides of the fin for subsonic and supersonic flow.
(2) Mesh did not update when the Distance before the nose tip was modified. The user needed to enter the Fin Geometry screen to see the alteration. Fixed.

VisualCFD 2.5
(1) Sears Haack nose cone models sometimes did not load correctly causing an error while reading the Project Data file. Fixed.
(2) Non-existing lines appear after reading Project Data files describing models with large inlet lengths. The phantom lines appeared in front of the actual model shape. Fixed.

VisualCFD 2.4
(1) Contour plots color levels may be edited and modified depending on the users preferences.

VisualCFD 2.3
(1) Added surface contour plots for Mach number, P/Pinf, T/Tinf and R/Rinf.

TOP OF INSTRUCTIONS or TOP OF PAGE

| MAIN PAGE | PRODUCTS | CONSULTING | MISSION | RESUME |