AeroCFD®
7.0
New Copyright © 19992018 John Cipolla/AeroRocket INSTRUCTION MANUAL DESIGNED FOR SLENDER MISSILES WITH FINS  MAIN PAGE  SOFTWARE LIST  AEROTESTING  MISSION  RESUME 

SUMMARY OF FEATURES 
INDEX OF INSTRUCTIONS
1) DEFINE
BASIC PROPERTIES
2) DEFINE MODEL GEOMETRY
3) MESH GENERATION
4) SOLUTION CONTROLS
5) FIN GEOMETRY (OPTIONAL)
6) PLOT RESULTS
7) AERODYNAMIC DEFINITIONS
8)
CLICK HERE
FOR REVISIONS
BASIC EQUATIONS FOR AeroCFD
The
Governing Equations that form the basis of every AeroCFD
analysis are derived from the Euler equations for inviscid
and compressible subsonic and supersonic flow. The Euler
equations are threedimensional and time dependent but have been
modified for 3D axisymmetric and 2D planar flow. The methodology
quickly captures shock waves within 1 to 2 adjacent cells depending
on the flux differencing scheme used.
1) DEFINE BASIC
PROPERTIES
BACK
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 freefield 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 FreeStream Mach number for the flow field being
investigated. The FreeStream Mach number is the ratio of freestream
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 FreeStream
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
AeroCFD. 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
BACK
The
Generate
Geometry for CFD Analysis section defines the shape of
a body under investigation. The geometry of the model is defined
by selection from up to five basic shapes provided by
AeroCFD
in any linear combination and then providing the dimensions required
for each section. Specifically, the user may select Nose Cone,
Body Tube1, Transition, Body Tube2 and Boat Tail transition
sections in any combination by selecting the crossbox 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, SearsHaack 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 AeroCFD. A simple
pulldown 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 crosssectional shape is
defined. In addition, transition shapes have a power series shape
control for defining very unusual 3D axisymmetric shapes and
2D shapes.
Parabolic Nose Cone Geometry:
AeroCFD
uses the standard mathematical
equation for a parabola aligned with the xaxis 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
AeroCFD 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.
AeroCFD Geometry Import Feature. The user can import up
to 1,000 XR 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 AeroCFD 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 shapeproject 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 XR point locations. Second and subsequent lines: X, R airframe
locations separated by commas. A AeroCFD shape file defines the upper contour
of an axisymmetric airframe geometry starting from nosetip to the end of
the airframe. Please see an example of
using a shape file for the analysis of a supersonic spherical bluntbody.
3) MESH
GENERATION
BACK
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
AeroCFD
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 stepbystep instruction to generate a mesh for the CFD analysis
follows:
a) Define the solution domain as either 3D axisymmetric flow
or 2D 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 Xaxis of the coordinate system is the centerline
of the flow field under investigation. For 2D flow starting with AeroCFD version
3.5.1, only the upper crosssection (above the centerline) is displayed and
resultant force and moment coefficients are based on the shape above the
xaxis (centerline).
b) Include base drag effects by selecting either the NASA TR
R100 method or the Hoerner Drag method using the two
option buttons. The NASA TR R100 method is based on the
threedimensional BasePressure 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
projectilelike 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 Xaxis or flow direction
as either 40 cells, 50 cells, 60 cells, 70 cells, 80 cells, 90 cells or 100
cells. This parameter represents
the total number of cells that are distributed along the Xaxis
of the flow field under investigation. How the grid points are
distributed in the Xdirection 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 Yaxis or up direction
as either 10 cells, 20 cells, 30 cells, 40 cells or 50 cells. This parameter represents
the total number of cells that are distributed along the Yaxis
of the flow field under investigation. How the grid points are
distributed in the Ydirection 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 (3D
direction or thickness (2D) 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 Xdistance 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 attachedshock flow, the
distance to the nose cone tip can be very small because the region
before the nose cone is essentially freefield 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 attachedshock 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 YDirection:
Insert the distance of the first grid point up from the surface
of the model. Ygrid 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.
j) Clustering Mesh in the XDirection:
Cluster the mesh in regions where flow gradients are highest by specifying the
Xgrid spacing at the tip of the airframe and the Xgrid spacing
at the end of the airframe. The airframe Xgrid clustering feature applies to
Import Shape definitions only. For clustering grids near the tip of Import
Shapes insert a nonzero value for Distance of first Xgrid from airframe tip.
For clustering grids near the end of Import Shapes insert a nonzero value for
Distance of last Xgrid from airframe end. Inserting 0.0 for the Xgrid distribution from the tip of
the airframe will cause the Xgrid distance from the end of the airframe to be
ignored. 
4) SOLUTION
CONTROLS
BACK
To control how
AeroCFD 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 subsection. Accurate solutions of flows dominated
by shock waves have been obtained by using a class of algorithms
referred to as upwind or fluxsplit. 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 fluxvector split scheme has been
shown to capture shock waves in as few as two mesh points. By
comparison, the Roe fluxdifference 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 fluxdifferencesplit
method. In addition, the Roe fluxdifferencesplit method
is less dissipative than the Steger Warming fluxvectorsplit
method and reaches a converged solution slightly slower than
the Steger Warming method. The best overall flux differencing
method is the Roe fluxdifferencesplit  Flux limit method 3
and is the default fluxsplitting method used in
AeroCFD.
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 1.0E4 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,
AeroCFD
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 (1.0E03)
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 1.0E03 an engineering solution
has probably been achieved and convergence has been attained.
5) FIN GEOMETRY
(OPTIONAL)
BACK
To add fins to the model enter the
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 xy coordinate system of the fin definition
screen. To define the fin plot region size, number of fins, fin
thickness, and fin crosssectional shape click the fifth icon
from the left on the tool bar at the top of the screen to expose
the Fin Parameter screen.
First, the PlotRegion 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 "PlotRegion location from
nose tip" is the first entry in the PlotRegion Dimensions
section. The "PlotRegion height and width" are defined
in the next data entry in the PlotRegion section. The first data
entry specifies where the PlotRegion is positioned down the axis
of the body and the next data entry specifies the size of the
PlotRegion used to define the fin geometry.
b) Next, in the Fin CrossSection Dimensions section, insert the
Total number of fins, Maximum fin thickness and if required by
the crosssectiontype 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 PlotRegion section.
c) To define a specific fin crosssectional shape select one of
the seven options listed in the pull down menu at the upper right
of the Fin Geometry
screen. The fin crosssectional 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 crosssectional
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 Semispan are
computed and displayed in the CrossSection Dimension Results
section.
e) Click back to the Fin
Geometry screen by reclicking the
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 UpDown 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 XY
Axes (Red) of the PlotRegion. 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 PlotRegion 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
AeroCFD
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 3dimensional 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.
SPECIAL NOTE: Defining fins in
AeroCFD
is easy but the following sequence must be followed.
1) In the Fluid Dynamic Properties section define Angle of attack
greater than zero. If Angle of attack = 0.0 then fin CL will be exactly zero.
2) In the toolbar click the Generate geometry for CFD analysis icon to
define the Body Tube Shape where the fins will be attached.
3) In the toolbar click Add fins to body to enter the Fin
Geometry screen.
4) In the toolbar click View fin parameter screen to define the Plot
Region Dimensions and Fin CrossSection Dimensions of the fins.
If plot region data is not defined correctly the program cannot generate
reliable fin geometry. Read
all definitions carefully to avoid strange results.
5) In the toolbar click View fin parameter screen and modify the number
of points defining the fins and then specify the freeform shape of the fin by pulling each
red
circle into position on the Body Tube Shape which is the gray line in the
Fin Geometry screen.
6) In the toolbar click the Return to main analysis arrow and SOLVE the
CFD analysis after the flow field mesh is defined.
6) PLOT RESULTS
BACK 
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 (3D) or thickness location
(2D) at each axial position on the body. Second, fluid dynamic
parameter verses axial position at each meridian location (3D)
or thickness location (2D) 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 XY 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 AeroCFD
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)
AeroCFD
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 Fin Geometry screen.
e)
AeroCFD
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 "jetpump"
that serves to reduce the static pressure at the base of the rocket. In other
words the jetpump, placed like a tube around the base of the rocket, mixes with
the circulating flow in the base region. High speed mixing of the jetpump and
the base region "pumps" air away from the base thus reducing the pressure at the
base of the airframe. The jetpump'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 R100 a curve of threedimensional
BasePressure 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 R100. The equation describing base drag coefficient
is: CDB = Cp_base * (Dbase / Dbody)^3. This method is more accurate than
Method2 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 319 to 320 and pages 164 to 166 of FluidDynamic
Drag, by S.F. Hoerner.
f)
AeroCFD
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
crosssectional 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)
AeroCFD
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 (OPTIONAL)
FLOW FIELD DIMENSIONS (AXIALX,
VERTICALY, CIRCUMFERENTIAL OR THICKNESSZ)
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 / (r_{00}
a_{00}^{2}), R
=
r
/
r_{00}, U = U / a_{00}, V = V / a_{00}, W = W / a_{00}
and a_{00} = (g P_{00} /
r_{00})^{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) AERODYNAMIC
DEFINITIONS
BACK
1) Mach Number, Mn = V / C, is the ratio of flow velocity (V)
at a point in the flow to the speed of sound (C) at that same
point in the flow.
2) Reynolds Number, Rn = V L / v, is the ratio of dynamic forces
(Velocity * Length) to friction forces (Kinematic viscosity) at
a point in the flow.
3) Drag Coefficients, CD = D / q S, is the drag force (D) in
the flow direction divided by the dynamic pressure (q) and the
reference area (S).
4) Lift Coefficient , CL = L / q S, is the lift force (L) perpendicular
to the flow direction divided by the dynamic pressure (q) and
the reference area (S)
5) Drag Coefficients, CX = X / q S, is the drag force (X) in
the axial direction of the rocket divided by the dynamic pressure
(q) and the reference area (S).
6) Lift Coefficient, CY = Y / q S, is the lift force (Y) perpendicular
to the axial direction of the rocket divided by the dynamic pressure
(q) and the reference area (S).
7) Normal Force Coefficient, CN = N / q S, is the normal force
(N) perpendicular to the axis of the rocket divided by the dynamic
pressure (q) and the reference area (S).
8) Pitch Moment Coefficient, CM = M / q S L, is the pitch moment
(M) acting around the tip of the nose cone divided by the dynamic
pressure (q), reference area (S) and the reference length (L).
A negative pitch moment (CM) indicates that a positive angle of
attack will cause a restoring moment (M) tending to return the
rocket to equilibrium flight. Having a negative CM when AOA is
"positive" is a "good" thing. It means the
rocket is stable! In other words the rocket will try to
return to its stable equilibrium position (zero degrees AOA) when
a disturbance, like a gust of wind, acts on the rocket.
9) Rocket Cp location, Xcp = XCp/L, is the nondimensional location
of the center of pressure. XCp/L is computed by dividing the dimensional
location of the center of pressure (XCp) by the reference length
(L) of the rocket, normally the total rocket length. Center of
pressure is the location or point where the resultant of all distributed
aerodynamic loads effectively act on the body. Center of pressure
can also be computed from: XCp =  M / N, where the M acts around
the tip of the nose cone.
10) Rocket Base Drag Coefficient, Cd_Base is the contribution
to pressure drag caused by the action of the insulating boundary
layer "jetpump" on the surface of the rocket that tends
to "pump" air away from the base of the rocket causing
the static pressure at the base of the rocket to be reduced. Cd_base
= 0.029 / SQRT(Cfb) * (Dbase / Dbody)^3 . Where Cfb is the total
forebody drag coefficient that does not include base drag effects.
This relationship is valid for subsonic and supersonic flow. Cd_Base
ranges from 0.025 to 0.20 for most rockets. Note: For turbulent
boundary layer flow the forebody drag coefficient (Cfb) can be
estimated to be a function of Mach number, Reynolds number and
body shape.
11) Dynamic Pressure, q = 1/2 * Air Density * V^2.
12) CD, CL, CX and CY are related by the equations: CD = CY *
sin(AOA) + CX * COS(AOA) and CL = CY * COS(AOA)  CX * SIN(AOA).
13) Static Pressure = Total Pressure  Dynamic Pressure. Can be
understood to be the pressure between streamlines in the flow.
14) Total Pressure = Pressure that would exist in a flow if the
flow were slowed isentropically to zero velocity. Also called
stagnation pressure for subsonic flow.
15) Dynamic Pressure = 1/2 * Air Density * V^2.
16) Pressure Coefficient, Cp = (P  PINF) / q. Definition of
pressure coefficient. Where P is the pressure anywhere in the
flow, PINF is the freestream pressure and q is the dynamic pressure.
17) Derivative of Normal Force Coefficient, CNa is the slope
of CN verses angle of attack . Specifically, CNa = (CN1  CN2)
/ (AOA1  AOA2).
18) The reference area (S) is the maximum frontal or crosssectional area of
the airframe.
19) The reference length (L) is the total length of the rocket.
NOTE: For more discussion on these topics please read Fluid
Dynamic Drag, by S.F. Hoerner. This is an excellent book and
is easy to understand.
AeroCFD VALIDATIONS
AND TEST CASES
CASE #1: V2
Rocket.
BACK TO LIST
Used AeroCFD to determine drag coefficient (CD)
as a function of Mach number from Mach 0.5 to Mach 5.0 for the V2 rocket operating
at 4 degrees angle
of attack. AeroCFD results compared to data from Figure 53 on page 126 of Rocket Propulsion
Elements. Reference: Rocket Propulsion Elements, Sixth Edition,
George P. Sutton.
V2 rocket surface contour plot, AOA = 4 degrees, Mach number = 2.0
CASE #2: HART Missile.
BACK TO LIST
HART Missile
Results using
AeroCFD compared to freeflight data from 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 FINSTABILIZED BODIES OF REVOLUTION"
by Roger G. Hart. NACA paper used to validate AeroCFD drag coefficient (Cd) from Mach 0.7
to Mach 1.5.
Surface flow field and free field contour
plot for the HART Missile operating at Mach 0.50 and 2 degrees angle of attack.
Surface flow field and free field contour
plot for the HART Missile operating at Mach 1.20 and 2 degrees angle of attack.
CASE #3:
DoubleWedge Wing.
BACK TO LIST
Wavedrag coefficient
verses Mach number for a 10% thick doublewedge
wing section. 2D AeroCFD results
were compared to wind tunnel measurements from the following reference. Reference: FluidDynamic Drag, by S.F. Hoerner, figure
9, page 1710. Please note: AeroCFD frictional drag has been subtracted
from total drag (CD) to compute doublewedge wavedrag based on wing area. The
following formula was used to determine wave drag based on wing area from
AeroCFD drag based on frontal area. Cd = CD * S_frontal / S_wing. To
determine total force in the xdirection simply double FX from AeroCFD version 3.5.1. Also, drag
(Cd) is nearly
identical in AeroCFD version 3.5.1 as predicted in previous versions.
CASE #4:
ConeCylinderFlare.
BACK TO LIST
Used AeroCFD to determine the shock pattern on a ConeCylinderFlare body.
AeroCFD results for the 3D axisymmetric
ConeCylinderFlare and results from NACA Report 1135 were used to determine conical shock wave locations
for the body operating at Mach 2.81, angle of attack = 0.0 Degrees, 100 X 50 X 10 Mesh
and solution time 15 minutes.
Cone CylinderFlare
solution using 100 X 50 X 10 mesh for Mach 2.81. Image illustrates Pressure Ratio contour plot
with NACA 1135 shock pattern.
CASE #5: X30 NASP.
BACK TO LIST
The following X30 NASP pressure (P/Pinf) contour plots were generated
by a 2D centerline analysis. Twenty separate AeroCFD 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. Also, presented below is an X30 NASP Cd
verses Mach number curvefit
approximation generated from the AeroCFD results. These CFD
analyses used imported 2D shapes for the upper and lower halves of the
X30 NASP and were analyzed separately then combined in the color contour plots
below. From the comparison of Cd verses Mach number of AeroWindTunnel and 2D
AeroCFD results it is evident the 2D assumption is most valid for
supersonic flow, M>1. This analysis requires AeroCFD 3.5.1 or higher.


X30 NASP CFD results for Mach 1.5, Mach 2 and Mach 5 at angle of attack = 0.0 degrees at 150,000 feet. 



CASE #6: Mars Phoenix Entry Capsule.
BACK TO LIST
The
following case illustrates the prediction of drag coefficient (Cd) verses Mach
number for the Mars Phoenix Entry Capsule. AeroCFD 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 V2 rocket described
in CASE 1 and the HART missile described in CASE 2
are capable of flow velocity well beyond Mach 10 using AeroCFD. For the Mars
entry capsule
the solution converges within one hour for the range of Mach numbers
selected using a 100 X 50 X 10 mesh. For the Mars Phoenix entry capsule example presented below
400
iterations were required using a CFL equal to 5 below
Mach 1 and 200 iterations using a CFL equal to 0.5 above Mach 1 to achieve
convergence.
AeroCFD analysis of the Mars Phoenix reentry capsule after 250 iterations at Mach 1.50 and zero degrees AOA. This is a reduced size screen shot of AeroCFD 5.2 with an image of the Mars entry capsule inserted. 
AeroCFD 3D composite view of the Mars Phoenix entry capsule. 
AeroCFD drag coefficient (Cd) verses Mach number compared to Fluid Dynamic Drag equations with base drag. 
CASE #7: XA1.0 VTL Rocket.
BACK TO LIST
Used AeroCFD to model the
Masten Space Systems XA1.0 vertical takeoff and landing suborbital rocket for Mach 3.0 and 0.0 degrees angle of
attack.
Vehicle shape developed using a CAD generated SphereConeCylinder TXT format geometry
file. Run time
about 20 minutes.
Surface pressure contour plot at Mach 3.0 
Free Field Mn contour plot and line contour plot at Mach 3.0 (100 X 50 X 10 mesh) 
CASE #8: Supersonic Projectile and Missile Aerodynamics.
BACK TO LIST
Ing. Marcelo Martinez of Nostroma Defense located in Alta GraciaCordoba,
Argentina used AeroCFD to generate the following slides for the
projectile and missile system illustrated below. AeroCFD results used with
permission. Marcelo Martinez stated: An interesting application of AeroCFD for
aerodynamics of rocket bodies to create a data base of rocket geometries.
Another application of AeroCFD I did last year for a sounding rocket. The
results were very good compared to Missile Datcom and Aeroprediction and we also
used your Euler code to predict aeroloads.
CASE #9:
Slender Missile with Fins Cd and Xcp, Mach 0.2 to Mach 6.
BACK TO LIST
This
section discusses the aerodynamic predictions, tests and
analyses of a slender fin stabilized missile
configuration for Mach numbers that range from 0.20 to
6. Prediction techniques consisted of both empirical and
analytical methods, including a stateoftheart
computational fluid dynamics (CFD) code. Free flight
tests in the USAF Aeroballistics Research Facility were
conducted on subscale wind tunnel models to obtain an
aerodynamic baseline to which the CFD predictions could
be compared. This section summarizes these results and
validates AeroCFD for the prediction of drag
coefficient (Cd) and center of pressure location (Xcp)
for the flight regime, which extends from Mach 0.20 to
Mach 6.
This section summarizes the results from the paper,
Aerodynamic Test and Analysis of a Slender Generic Missile
Configuration published by the AIAA Atmospheric Flight
Mechanics Journal in 1989 and authored by John Cipolla.
Slender missile with fins geometry (inches) defined for
the AeroCFD analysis.
Free Flight data measured using the
USAF Aeroballistic Research Facility (ARF)
Freeflight center of pressure
location and
drag coefficient of a slender missile with fins compared to AeroCFD.
TECHNICAL SUPPORT
For
AeroCFD
technical support please
read the online instructions.
PURPOSE OF AeroCFD
and HyperCFD
AeroCFD is a sophisticated
Computational Fluid Dynamics (CFD) computer program based on 2dimensional and
3dimensional finitevolume theory and is price break through at only $50 for a
perpetual license. AeroCFD is based on the solution
of the compressible Euler equations and is a sophisticated program for the
definition of aerodynamic characteristics of fin stabilized flight vehicles in
subsonic, transonic and supersonic flow.
HyperCFD on the other hand is a surface
inclination CFD program better suited for the analysis of supersonic and
hypersonic flight of high power rockets and is unique because results are
achieved immediately for a limited library of shapes.
PROGRAM REVISIONS
AeroCFD
7.0.0.1
(February 1,
2017)
1)
Greatly increased speed and efficiency for defining fins
resulting in faster model generation time. This made AeroCFD easier to use.
2) Improved the appearance and functionality of the AeroCFD graphical user
interface.
3) Reduced the price of AeroCFD to $25.
AeroCFD
6.2.0.1
(January 1,
2016)
1)
Greatly enhanced computational speed for Windows 8,
10 and other enhancements. Verified compatibility with Windows 10.
AeroCFD
5.2.0.1
(January 5,
2015)
1) On the Fin Geometry screen AeroCFD
now displays individual fin axial force (FX) and individual fin normal force (FY) in pounds
and Newtons depending on UNITS selected. Fin subsonic, transonic and supersonic
aerodynamic coefficients and associated fin forces are especially accurate
because the analytical methods are derived using a twodimensional finite
difference numerical method modified in the transonic regime by methods
presented in AIRCRAFT DESIGN: A
CONCEPTUAL APPROACH, by Daniel P. Raymer.
2) For Free Field contour plots an outline representation of the fins are
displayed to illustrate fin location and that a finite difference CFD analysis
has been performed successfully.
AeroCFD
5.1.0.2
(August 10,
2013)
1)
Changed program name from VisualCFD
to AeroCFD.
VisualCFD
4.1.0.2
(October 15,
2011)
1)
Minor display
modification.
VisualCFD
4.1.0.1
(January 05,
2011)
1) Added the capability to define upper
and lower spectrumplot limits for Free Field filled contour and
Free Field line contour plots.
This capability is especially useful for idealizing complex threedimensional vehicles
like the HTV3X and X30 NASP as twodimensional models. For
twodimensional analyses of nonsymmetrical bodies the upper and lower
airframe contour plot limits need to be identical for
accurate flow field evaluation.
2) For previous versions of VisualCFD when printing Axial Data and
Angular Data for twodimensional models the caption and values in the
thickness directions were incorrectly labeled Angle and values presented
in degrees instead of being labeled Z and width values from
0.0 to Total model width.
VisualCFD
4.1.0.0
(November 05,
2010)
1) Increased
the maximum number of cells in the axial direction from 60 to 100 and
increased the maximum number of cells in the transverse direction from 30 to 50.
Therefore, VisualCFD 4.1 increases the maximum number of discrete
finitevolumes available for CFD analysis from 18,000 cells to 50,000 cells.
Greatly improves the computational power of VisualCFD without increasing run
times.
2)
For VisualCFD
4.1 the online instructions are accessed by clicking Help then Online
Instructions then selecting either Windows XP or Windows 7 or VISTA.
These commands will connect the user to the online VisualCFD Instructions. Previously when operating under Windows 7 and
Windows VISTA the message, Error displaying Online Instructions was displayed
when trying to access the online instructions.
This occurred because under Windows XP,
ShowHTML.exe is located in c:/Program Files/VisualCFD but for Windows 7 and Windows VISTA the routine is located in c:/Program
Files (x86)/VisualCFD.
3) Made the VisualCFD command screen crisper in appearance and more in line with
techniques used for Nozzle and AeroSpike.
4) Improved the appearance and resolution of the Welcome and System
Requirements splash screens.
5) For a limited time (two months) upgrading to VisualCFD 4.1 is FREE for original
purchases made after January 30, 2009.
Please contact
AeroRocket
for more details...
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 Runtime 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.
3) When operating earlier versions of 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 temporary 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
3.5.0.1 (November 18, 2007)
(1) In versions prior to
3.5.0 VisualCFD 2D forces and moments were based on the combined uppershape
and reflected lowershape. However, VisualCFD never determined forces
and moments on the lower crosssection for 2D flow. Therefore, starting with this
version only the uppershape is displayed for 2D analyses. This is valid
because zcoordinates for 2D flow are in the thickness direction while the
equivalent dimension for 3D flow is the Theta or circumferential direction. For
these reasons 3D axisymmetric analyses will continue to display the total upper
and lower crosssections while 2D analyses will display only the upper
crosssection. 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 2D
flow. For 3D 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 2D flow was limited to zero degrees. This artificial limit has been
removed allowing angle of attack
for 2D 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 2D and 3D 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
Xgrid 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 Runtime '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 builtin instructions locator to correctly link to the online
VisualCFD instructions. Added several other links.
(5) Clarified various command buttons with the addition of tooltip
descriptions.
VisualCFD
2.8 and 2.9
(November 20, 2004 and January 7, 2005)
(1) Added the ability to Import complex airframe shapes
having up to 1,000 XY points for generation of more complex airframe
designs.
VisualCFD
2.7 (January 29, 2004)
(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
(August 21, 2003)
(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
(August 3, 2003)
(1) Sears Haack nose cone models sometimes did not load correctly
causing an error while reading the Project Data file. Fixed.
(2) Nonexisting 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
(2002)
(1) Contour plots color levels may be edited and modified depending
on the users preferences.
VisualCFD
2.3
(2002)
(1) Added surface contour plots for Mach number, P/Pinf, T/Tinf
and R/Rinf.
TOP
OF INSTRUCTIONS
or TOP OF PAGE

MAIN
PAGE
 SOFTWARE LIST 
AEROTESTING 
MISSION

RESUME 