【转帖】Building the Finite Element Model -转自--达摩BigGreen BBS

edodo

发信人: Mars (Momotalo), 信区: MathTools
标  题: Building the Finite Element Model[ANSYS]
发信站: 达摩BigGreen BBS (Sat May 25 15:04:29 2002), 站内信件
  
Building the Finite Element Model
  
Building the model
Building the model takes a large portion of user's time, though it  
may only take a small portion of CPU time.  
Before you start building the model, you enter the Begin-level  
commands which start with "/":  
Specify the jobname.  
specify the graphics driver, the title, the units, and others.  
And then you enter the model building phase with the /PREP7  
command:  
Define Element Types  
Define Element Real Constants  
Define Material Properties  
Define Model Geometry  
  
Specifying the jobname  
The file name prefix - the jobname - can be specified in two  
ways:  
   ansys -j name        at the execution, or
   /FILENAME,name       within the program.
   
If you don't specify a job name, all files are given the default  
prefix name FILE.  
  
Specifying the graphics driver, the title, the units, and others
These commands start with "/" as the following:  
   /SHOW,X11C          ! Use X-windows for display
   /FILNAM,PLATE       ! Specify prefix of file names
   /TITLE,An Aluminum Plate with a Hole
   /STITLE, ....       ! Up to 4 subtitles
   /UNITS,BIN          ! British units: lbs, in, etc. for ref. only
  
   /PREP7              ! Enter preprocessing phase
   /SOLU               ! Enter loading and solution phase
   /POST1              ! Review the results
   /EXIT               ! Exit ansys program
   
  
Defining Element Types  
There are over 80 different element types defined in ANSYS  
element library. Element type is identified by the element  
category and a unique number: BEAMn,PLANEn,  
SOLIDn,SHELLn,LINKn, etc. The number n remains the same  
as STIFFn. ET,1,42 and ET,1,PLANE42 are the same.  
   ET
   ETCHG
   ETLIST
   ETDELE
   TYPE
  
Many element types also have additional options, known as  
KEYOPTs and referred to as KEYOPT(1), KEYOPT(2), etc.  
KEYOPT  
Element types can also be defined by the control panel; so can  
the element options and the real constants.  
  
Defining Element Real Constants  
Element real constants are properties that are specific to a  
given element type, such as cross-sectional properties of a  
beam element. Not all elements require real constants. As with  
element type, each set of real constants is given a reference  
number. While defining the element, you can point to the  
appropriate real constant reference number using REAL  
command.  
   R
   RMODIF
   RMORE
   RLIST
   RDELE
   REAL
  
Defining Material Properties  
Depending on the application, material properties may be  
linear, nonlinear, or anisotropic. As with element type and real  
constants, each set of material properties is given a material  
reference number, and you point to the appropriate material  
reference number using the MAT command.  
1. Linear Material Properties  
Linear material properties may be constant or temperature  
dependent, and isotropic or orthotropic.  
   MP
   MPLIST
   MPDELE
   MAT
  
   MP,EX,1,2E11       ! Young's modulus for material 1 is 2E11
   MP,DENS,1,7800     ! Density for material 1 is 7800
   MP,KXX,3,43        ! Thermal conductivity for
                      !   material 3 is 43
  
Temperature dependent material properties may be defined by  
a property-versus-temperature function in the form of a  
polynomial with MP command, or by MPTEMP and MPDATA  
commands.  
   MP,xyz,C0,C1,..C4
  
   
  
   MPTEMP
   MPTGEN
   MPDATA
  
   MPTEMP,1,1600,1800,2000,2325,2326,2335 ! 6  
temperatures from loc 1
   MPTEMP,7,2345,2355,2365,2374,2375,3000 ! 6 more from  
location 7
   MPDATA,ENTH,4,1,53.81,61.23,68.83,81.51,81.55,82.31 !  
corresponding
   MPDATA,ENTH,4,7,84.48,89.53,99.05,112.12,113.0,137.4 !  
Enth values
   MPDATA,ENTH,4,6,83.09  ! Change loc 6 ENTH value to  
83.09
   MPTEMP,7,2340 ! Modify 7th temperature to 2340, retain  
others
   MPDRES,ENTH,4 ! Restore what is changed into virtual  
space
  
To define a different set of temperature for the next material  
property, you first erase the current temperature table by  
MPTEMP without any arguments and then define the new  
temperature using MPTEMP or MPTGEN command.  
   MPTRES        ! Restore temperature table from virtual space
   MPWRITE       ! Write from database to a coded file
   MPREAD        ! Read from a coded file to database
   MPPLOT
   MPLIST
   
An MPPLOT Display  
2. Nonlinear Material Properties  
There are many changes in nonlinear material properties. NL  
and KNL commands are no longer used; data tables are used  
instead. TB command defines the type of data table: bilinear  
kinematic (BKIN), anisotropic elastic (ANEL), B-H curve (BH),  
etc. TBEDIT command (with menu on only) brings up a matrix  
of boxes for data entry. For non-menu mode, use TBPT to  
enter x, y data (stress-strain curves, B-H curves, etc.) and  
TBDATA to enter tabular data (creep constants, failure criteria,  
etc.)  
   TB,BH,2       ! activate B-H table for material ref. 2
   TBTEMP
   TBPT
   TBDATA
   TBPLOT
   TBLIST
  
   TBCOPY
   TBDELE
   
3. Anisotropic Elastic Material Properties  
Some element types accept anisotropic elastic material  
properties, which are usually in matrix form - SOLID64(3-D  
anisotropic solid), PLANE13(2-D couple-field solid),SOLID5 and  
SOLID89(3-D couple-field solids). Please refer to Element  
Reference Manual for details.  
   TB
   TBDATA
   TBLIST            ! Be sure to verify your input
  
   TB,PIEZ,3         ! piezoelectric constants(6x3)
   TBDATA,3,-6.1,,,-6.1
   TBDATA,9,15.70
   TB,ANEL,3         ! [C(6x6)] matrix for NEPEC
   TBDATA,1,12.80E10,6.8E10,6.6E10}
   TBDATA,7,12.8E10,6.6E10
   TBDATA,12,11.0E10
   TBDATA,16,2.1E10,0.0,0.0,2.1E10,0.0,2.1E10
   
  
Defining the Model Geometry  
There are two different methods to generate a model: top-down  
solid modeling and bottom-up direct generation. With top-down  
solid modeling, you describe the geometric shapes of the  
model, establish controls over the size and desired shape of  
elements, and then instruct the ANSYS program to generate all  
nodes and elements automatically.  
By contrast, with bottom-up direct generation method, you  
define the location of every node, and the size, shape, and  
connectivity of each element. Although some automatic data  
generation is possible ( such as FILL, NGEN, EGEN, etc.), the  
direct generation method requires you to keep track of all node  
numbers as you develop your finite element mesh.  
You can combine top-down and bottom-up modeling  
techniques in building your model. In top-down solid modeling,  
free and mapped meshing are available; also concatenation of  
lines or areas greatly improves meshing. Elements are  
reordered automatically; use NOORD command to prevent  
reordering.  
Top-down solid model is usually more powerful and versatile  
than bottom-up direct generation, and is commonly the  
preferred method.  
Top-down solid modeling with Boolean operation greatly eases  
the preparation of many models. The following examples show  
the difference between meshing a plate with a hole using  
Boolean operation and without Boolean operation.  
  
Top-down modeling  
Geometric primitives  
Boolean operations  
Concatenation  
  
Top-down solid modeling with Boolean operation:
   /PREP7
   /TITLE,Plate with a Hole using Top-down Solid Modeling
   ! This plate is modeled with quarter symmetry
   ET,1,PLANE42   ! Use PLANE42 as element type 1
  &nbspCIRC,.5       ! Define a circle primitive, center at origin, with
                  ! radius of 0.5
   RECTNG,0.0,6.0,0.0,4.0
                  ! Define a rectangular primitive
   /PNUM,AREA,1
   APLOT
   ASBA,2,1       ! Boolean subtract operation: area 2 minus  
area 1
                  ! yields a new area
   KLIST
   KSEL,S,KP,,1,2 ! Select keypoints on circle
   KESIZE,ALL,.1  ! Set element size to 0.1
   KSEL,INVE      ! Invert selection to select keypoints at rec.  
corners
   KESIZE,ALL,0.4
   AMESH,3        ! Mesh area 3
   ACLEAR,3       ! Clear the meshed area
   ESHAPE,2       ! Use quadrilateral element shape only
   LCCAT,6,7      ! Concatenate lines 6 and 7
   AMESH,3        ! Mesh area 3 again
   SAVE           ! Save the db file
   FINISH         ! Exit PREP7
   
  
Top-down Boolean Meshing Results - 1  
Top-down Boolean Meshing Results - 2  
  
Equivalent program without Boolean operation:  
   /PREP7
   /TITLE,Plate with a Hole without using Boolean operations
   ! This plate is modeled with quarter symmetry
   ET,1,PLANE42   ! Use PLANE42 as element type 1
   K,1,0.5        ! Define keypoints
   K,2,6
   K,3,6,4
   K,4,,4
   K,5,,0.5
   CSYS,1         ! Cylindrical CS for keypoint 6
   K,6,0.5,45
   /PNUM,KPOI,1   ! Show keypoint numbers on display
   KPLOT
   L,1,6,10       ! Define circular line segments
   L,6,5,15
   CSYS           ! Switch to Cartesian CS for area definition
   L,1,2,30,4     ! Define radial line segments
   L,6,3,30,4     !   with 4:1 spacing ratio
   L,5,4,30,4
   L,2,3,10       ! Define line segments
   L,3,4,15
   /PNUM,LINE,1   ! Show line numbers on display
   LPLOT          ! Dis[lay line segments
   A,1,2,3,6      ! Define areas
   A,6,3,4,5
   AMESH,ALL      ! Generate nodes and elements
   SAVE           ! Save the db file
   FINISH         ! Exit PREP7
   
  
Non-Boolean Meshing Results  
  
A bottom-up modeling example with automatic data  
generations:
   /PREP7
   ET,1,PLANE42     ! Use PLANE42 as element type 1
   N,1,0,0          ! Node 1 at (0.0,0.0)
   N,5,12,o         ! Node 5 at (12.0,0.0)
   FILL,1,5         ! Fill in nodes 1 through 5
   NGEN,6,10,1,5,1,1,2,0
                    ! Generate nodes from an existing, given pattern
   E,1,2,12,11      ! Define the first element with four nodes  
1,2,12,11
   EGEN,4,1,1       ! Generate 4 add'l elements by incrementing  
the
                    !   nodes of the first element by 1.
   EGEN,5,10,1,4,1  ! Generate 5 sets of add'l elements by  
incrementing
                    !   the nodes of the 1-4 elements by 10.
   SAVE             ! Save the db file
   FINISH           ! Exit PREP7
  
  
A bottom-up modeling results
  
Mesh Generation  
Regions of steep gradients in solution variables usually require  
finer mesh. In direct generation method, users may define  
denser points in these regions and connect them to form finer  
meshes. In solid modeling method, the mesh density can be  
experssed in either of two ways:  
Element size  
Number of element division  
The following commands specify element size or number of  
division:  
   ESIZE,size,ndiv
   KESIZE,kpt(s),size
   LESIZE,line(s),size,angsize,ndiv,space
   LDVA
   
Free meshing allows a mixing of different element shapes and  
provides an easier transition from a fine mesh to a coarse  
mesh, and vice versa. It is the default meshing. To control  
element shape, use ESHAPE command.  
Meshing an area or a volume with mapped mesh (ESHAPE,2)  
must observe the following restrictions:  
Lines must have eaqual number of division on opposite sides.  
Number of division must be even if three sided.  
KCLEAR,LCLEAR,ACLEAR, and VCLEAR commands delete  
the nodes and elements. To refine a mesh, the nodes and  
elements should be first deleted by one of these commands.  
General meshing gudelines:  
Avoid rapid transitions in element sizes which can cause  
meshing failure or numerical instabilities.  
Mesh areas/volumes before generating symmetry reflection or  
transferring. It takes less CPU time.  
Five sided aread can be split into two area or use LCCAT  
command to concatenate lines to become four sided.  
  
Parametric Design and Macros  
Parametric design allows users to build the model in terms of  
parameters(variables). Generally these variables are defined at  
the beginning of the program, and ANSYS commands use  
these variables in lieu of actual values. When the design  
needs to be modified, users just change the values of the  
corresponding variables and rerun the program.  
Ansys parametric design language now permits 8-character  
names. Names may contain letters, numbers, and the  
underscore(_). Don't use the underscore as the first character.  
A macro is a sequence of ANSYS commands stored in a file or  
a macro library. The macro can be used anywhere in an  
ANSYS program.  
A macro can be created inside ANSYS program using  
*CREATE and *END commands. It can also created in a file or  
a library with an editor. If a macro file has a .MAC suffix, the file  
name can be used as an ANSYS command. For example,  
ELLIPTQ.MAC is stored in /ansys50a/docu and ELLIPTQ is a  
valid ANSYS command. Users can stored their macros in a file  
or in a macro library a directory and use *ULIB to refer the  
file/library if it not in user's home or current directory.  
Up to 29 parameters and values can be passed to a macro.  
Inside a macro, ARG1,ARG2,...,ARG29 are reserved local  
variables, and while executing the macro, the first field value is  
referred as ARG1 and the second as ARG2, and so on.  
New *ASK command, if included in macros, can be used to  
prompt for input:  
   *ASK,L,LENGTH:,5.0       ! Prompts for length, assigns value
                            ! to L, default value is 5.0
   
New *AFUN command allows you to switch from default  
radians to degrees for trigonometric functions:  
   *AFUN,DEG     ! Angular function units are in degrees
   X=SIN(30)
   *AFUN,RAD
   
*IF-THEN-*ELSEIF-*ELSE-*ENDIF and DO loop are available.  
   *IF,A,LT,B,THEN
   . . .
  
   *ELSEIF,B,LT,C,THEN
   . . .
  
   *ELSE
   . . .
  
   *ENDIF
  
   *DO,I,1,3
   . . .
  
   *ENDDO
   
Using a wide range of features, such as macros, if-then-else  
branching, do-loops, vector and matrix operations, and Fortran  
functions, users can write a versatile ANSYS program.  
A Macro Example  
   ! ELLIPT by Hai C. Tang in  tang/ansys
   ! Creates an elliptic area
   ! *USE,ELLIPT,A,B,N
   ! where x**2/a**2 + y**2/b**2 = 1
   ! and the whole elliptic arc is divided into N parts
   ! equally by the angle at origin
   *SET,A,ARG1
   *SET,B,ARG2
   *SET,N,ARG3
   *AFUN,DEG
   THETA=360.0/N
   K,,A
   *GET,KMIN,KP,,NUM,MAX
   *DO,I,1,N
   ANGX=I*THETA
   X=A*COS(ANGX)
   Y=B*SIN(ANGX)
   K,,X,Y
   **GET,KMAX,KP,,NUM,MAX
   L,KMAX-1,KMAX
   *ENDDO
   *GET,LMAX,LINE,,NUM,MAX
   LMIN=LMAX-N+1
   NUMMRG,ALL
   LSEL,S,LINE,,LMIN,LMAX
   AL,ALL
   LSEL,ALL
  
An ANSYS program Using Macro  
   /PREP7
   ET,1,42
   R,1,.25
   MP,EX,1,1e7
   $*$USE,ELLIPT,.05,.2,36
   /pnum,kp,1
   RECTNG,,3,,2
   /pnum,area,1
   aplot
   asba,2,1
   kesize,10,.01
   ksel,s,kp,,1,5
   kesize,all,.04  
   ksel,s,kp,,38,40
   kesize,all,.2
   ksel,all
   amesh,3
   save
   FINISH
   /SOLU
   lsel,s,line,,41,42
   dl,all,3,symm
   lsel,all
   sfl,38,pres,-100
   solve
   FINISH
   /POST1
   PLNSOL,S,EQV
   
  
Mesh Refinement  
High gradient areas generally require finer meshes. Meshes  
can be refined with:  
Adaptive meshing  
User adjustment  
Adaptive meshing automatically evaluates mesh discretization  
error in each element and determines if a particular mesh is fine  
enough. If it is not, the element is refined with finer meshes  
automatically.  
Users can also revise the mesh by modifying the mesh controls  
after they have reviewed the results of initial runs. Only the  
meshes in the regions of steep gradients need to be revised.  
Usually this is less CPU intensive and is more applicable to the  
situation that requires only minor adjustments.  
Consider the solution for the semi-infinite plate with an elliptic  
crack in last example. Clearly the steep gradient is located near  
the crack tip, and only the tip area need to be refined. So let's  
binarily bisect tip element m times with the following formula;  
m = log(b/a + 1)  
  
A Mesh Refinement Example
   ! *USE,ELLIPTQ,A,B,N
   *SET,A,ARG1
   *SET,B,ARG2
   *SET,N,ARG3
   *AFUN,DEG
   THETA=90.0/N
   K
   *GET,KMIN,KP,,NUM,MAX
   K,,A
   L,KMIN,KMIN+1
   *GET,LMIN,LINE,,NUM,MAX
   *IF,A,GT,B,THEN
   M=LOG(A/B+1)
   ANGX=THETA/2**(M+1)
   *DO,I,1,M
   ANGX=ANGX*2
   X=A*COS(ANGX)
   Y=B*SIN(ANGX)
   K,,X,Y
   *GET,KMAX,KP,,NUM,MAX
   L,KMAX-1,KMAX
   *ENDDO
   *ENDIF
   *DO,I,1,N-1
   ANGX=I*THETA
   X=A*COS(ANGX)
   Y=B*SIN(ANGX)
   K,,X,Y
   *GET,KMAX,KP,,NUM,MAX
   L,KMAX-1,KMAX
   *ENDDO
   *IF,A,LT,B,THEN
   M=LOG(B/A+1)
   ANGM=THETA
   *DO,I,1,M
   ANGM=ANGM/2
   ANGX=ANGX+ANGM
   X=A*COS(ANGX)
   Y=B*SIN(ANGX)
   K,,X,Y
   *GET,KMAX,KP,,NUM,MAX
   L,KMAX-1,KMAX
   *ENDDO
   *ENDIF
   ANGX=N*THETA
   X=A*COS(ANGX)
   Y=B*SIN(ANGX)
   K,,X,Y
   *GET,KMAX,KP,,NUM,MAX
   L,KMAX-1,KMAX
   L,KMAX,KMIN
   *GET,LMAX,LINE,,NUM,MAX
   NUMMRG,ALL
   LSEL,S,LINE,,LMIN,LMAX
   AL,ALL
   LSEL,ALL
  
A Mesh Refinement Example
   /PREP7   
   ET,1,42  
   R,1,.25  
   MP,EX,1,1e7  
   ELLIPTQ,.05,.2,9
   /pnum,kp,1   
   RECTNG,,3,,2
   /pnum,area,1
   aplot   
   asba,2,1
   ksel,s,kp,,11,13
   kesize,all,.005   
   ksel,s,kp,,9,10
   kesize,all,.001   
   ksel,all
   kesize,2,.02
   ksel,s,kp,,15,17
   kesize,all,.2   
   ksel,all
   amesh,3  
   save
   FINISH   
   /SOLU   
   lsel,s,line,,18,19   
   dl,all,3,symm   
   lsel,all
   sfl,15,pres,-100
   solve   
   FINISH   
   /POST1 PLNSOL,S,EQV
  
Graphics Display  
The first command in an interactive ANSYS run, /SHOW  
specifies the graphics device driver. The most common drivers  
at NIST are:  
   X11,X11C, etc       X-windows based
   3D                  For local run only
   
3D has local graphics functions that work only the workstation  
actually running the ANSYS program. X-windows allow users to  
run ANSYS on a network connected remote machine and to  
instantaneously display the results on a local workstation or a  
X-terminal.  
ANSYS has two types of commands that control a display:  
Graphics action commands:  
   xPLOT                displays elements/volumes/areas/lines
   x = E,V,A,L,K,N         /keypoints/nodes,respectively
   PLNSOL               plots nodal solution
   PLESOL               plots element solution
   etc.
   
Graphics specification commands:  
   /PNUM,label,key          specifies if numbers of label are  
shown
   /PBC,item,component,key  specifies if constraints or loads  
are shown
   /PSYMB,label,key         specifies if symbols(CS/LDIR etc)  
are shown
   /EDGE,wn,key,angle       specifies if edges are shown
   etc.
   
Selective displays can be made with the nodes and elements  
SELECT utilities - ASEL, NSLA, NSEL, ESEL, etc. If a  
selective command is issued before the PLNSOL command,  
only the results on the selected elements will be displayed. The  
following comands are the frquently used graphics commands:  
   PLNSOL,item,comp           Displays the solution results
                                as continuous contours
   PLDISP,kund,kscal          Displays the displaced structure
   /WINDOW,wn,xmin,xmax,      Defines window size on  
screen
           ymin,ymax,ncopy
   /TYPE,wn,type              Defines type of display
   /FOCUS,wn,xf,yf,zf,ktrans  Defines the location of object
                                to be at the center of the window
   /DIST,wn,dval,kfact        Defines the viewing distance for
                                magnification and perspective
   /VIEW,wn,xv,yv,zv          Defines the viewing direction of
                                the ojbect
   Grph menu button           Interactive graphics for Zoom,
              Rotation, and Translation
   
  
Use of Generic Utilities  
In Revision 5.0, many utility commands are generic and  
consistent for all disciplines, and they are available throughout  
the program. For example, select logic and components are  
available anywhere in the program, at anytime, and button  
menus are also available. The type of selection (reselect,  
unselect, additional select, all, etc.) has been moved to the first  
field on the command, and there are more fields for the basis of  
selection.  
   NSEL
   ESEL
   KSEL
   LSEL
   ASEL
   VSEL
   CMSEL
  
Exiting the PREP7 preprocess  
FINISH command at the end of PREP7 modeling does not  
save the database; issue SAVE command to save the  
database before exiting the process.  
  
ANSYS Example 1  
   Thermal Modeling of a Cryogenic Radiometer
  
   Given:    A radiometer at cryogenic temperature is applied  
with a
       constatnt heat flux at given nodes on the surface  
of a
       2-layer cone whose base is welded to a  
cylindrical tube.
  
   The radiometer is modeled with axial symmetry.
   
ANSYS Program for Example 1  
   /FILNAM,AXSYM1           ! Specify prefix of file names
   /TITLE,Cryogenic Radiometer
   /UNITS,cgs               ! SI units: cm,g,s,K,1e-7 J, etc.
                            !   for reference only
   /PREP7                   ! Begin PREP7 preprocessing phase
   ET,1,55,,,1              ! 2-D 4 node PLANE element, axial sym.
   ! ET,1,PLANE77           ! 2-D 8 node PLANE element
   ! MPTEMP,1,2,5,10,20     ! Temp. at 2,5,10,and 20 K
   MPTEMP,1,0,2.8,7.8,17.8  ! Temp = ABTemp - 2.2 K  
   /COM,Thermal Conductivity, KXX, ABW/cm.K (1E-7  
W/cm.K)
   MPDATA,KXX,1,1,1.69E7,3.10E7,5.74E7,10.75E7  ! MAT 1  
(Cu)
   MPDATA,KXX,2,1,2.2E4,5.0E4,10.0E4,20.0E4     ! MAT 2  
(Paint)
   MPDATA,KXX,3,1,1.57E4,3.69E4,7.96E4,18.3E4   ! MAT 3  
(SS)
   /COM,Specific Heat, C, ABJ/kg.K
   MPDATA,C,1,1,0.355E3,1.8E3,9.0E3,73.0E3      ! MAT 1
   MPDATA,C,2,1,0.144E3,9.23E3,23.1E3,51.0E3    ! MAT 2
   MPDATA,C,3,1,1.0E4,2.4E4,5.0E4,13.0E4        ! MAT 3
   MP,DENS,1,9.08           ! Density for MAT 1
   MP,DENS,2,1.154          ! Density for MAT 2
   MP,DENS,3,8.00           ! Density for MAT 3
   /COM, *** Define Geometry
   R=1.9185                 ! SET  radius, cone1
   R1=1.905                 ! SET  radius, cone2
   R2=1.8995                ! SET radius, cone3
   R3=1.900                 ! SET radius, cylinder I.D.
   H=4.632                  ! SET Height of cone1
   H1=4.600                 ! SET Height of cone2
   H2=4.586                 ! SET Height of cone3
   H3=-5.0E-1               ! SET Height of cylinder (MAT 1)
   H4=-3.50                 ! SET Height of cylinder (MAT 3)
   THK1=R-R1                ! Cylinder thickness and cone disp for  
MAT 1
   THK2=R1-R2               ! Paint displacement in x-dir for MAT 2
   THK3=R1-R3               ! Cylinder thickness for MAT 3
   DH=0.05
   DR=DH*R/H                ! rate of change of copper cone  
radius
   DH1=0.02
   DR1=DH1*R/H              ! rate of change of copper cone  
radius
          ! near the tip
   CSYS,0
   N,1,R,H3                 ! Node 1
   NGEN,11,1,1,,,0,DH       ! Node 1-11
   NGEN,91,1,11,,,-DR,DH    ! Node 11-101
   NGEN,5,1,101,,,-DR1,DH1  ! Node 101-105
   N,150,0,H                ! Node 150 is the tip of cone1
   NGEN,2,200,1,105,1,-THK1 ! Node 201-305
   N,350,0,H1               ! Node 350 is the tip of cone2
   NGEN,2,1,350,,,THK1      ! Node 351 on cone1
   NGEN,2,200,211,305,1,-THK2   &! Node 411-505
   N,550,0,H2               ! Node 550 is the tip of cone3
   NGEN,2,1,550,,,THK2      ! Node 551 on cone2
   NGEN,2,1,551,,,THK1      ! Node 552 on cone1
   N,601,R1,H4              ! Node 601 at cylinder bottom
   NGEN,71,1,601,,,0,DH     ! Node 601-671
   NGEN,2,100,601,671,1,-THK3  ! Node 701-771
   MAT,1               &! MAT 1 is copper
   E,201,1,2,202            ! Elem 1
   EGEN,104,1,1             ! Elem 1-104
   /PNUM,ELEM,1
   E,305,105,552,551        ! Elem 105
   E,551,552,351,350        ! Elem 106
   E,350,351,150,150        ! Elem 107
   EPLOT
   *ASK,KC,' to continue:',0
   *IF,KC,NE,0,THEN
       FINISH
       /EXIT
   *ENDIF
   MAT,2 &! MAT 2 is paint
   E,411,211,212,412       ! Elem 108
   EGEN,94,1,108           ! Elem 108-201
   E,505,305,551,550       ! Elem 202
   E,550,551,350,350       ! Elem 203
   EPLOT
   *ASK,KC,' to continue:',0
   *$IF,KC,NE,0,THEN
        FINISH
        /EXIT
   *ENDIF
  
   MAT,3                   ! MAT 3 is stainless steel
   E,701,601,602,702       ! Elem 204
   *GET,LELM,ELEM,,NUM,MAX ! Find the last element  
number
                ! LELM=204
   EGEN,70,1,LELM          ! Elem 204-273
   EPLOT
   NUMMRG,NODE
   SAVE
   FINISH
   
  
ANSYS Example 2  
   /TITLE, Full NIST Piezo Shaker, Case A with Damping
   /PREP7
   ET,1,SOLID5              ! 3-D Multi field solid element
   /COM, *** Material properties for Piezoelectric
   /COM, *** ceramic PZT-5 -- CLEVITE CORP
   MP,DENS,3,.000722
   /COM, *** Permittivity (X,Y and Z Directions)
   MP,PERX,3,3.8853E-10
   TB,PIEZ,3                ! [E] = Piezoelectric matrix
   TBDATA,3,-.00511
   TBDATA,6,-.00511
   TBDATA,9,.00972
   TBDATA,11,.00795
   TBDATA,13,.00795
   MP,MURX,3,1              ! Create dummy properties to avoid
   MP,KXX,3,1               !   warning messages
   /COM     *** B4C - Boron Carbide Properties (table)
   MP,DENS,2,.000345
   MP,EX,2,54.E6
   MP,NUXY,2,.345
   /COM     *** Adhesive Properties
   MP,DENS,4,.00016
   MP,EX,4,15.E5
   MP,NUXY,4,.38
   /COM     *** WC - Tungsten Carbide Properties (base)
   MP,DENS,5,.00163
   MP,EX,5,99.E6
   MP,NUXY,5,.3
   DMPRAT,.01
   HAA=1.002                ! Height of top of lower adhesive layer
   HP=1.202                 ! Height to top of piezoelectric layer
   HAB=1.204                ! Height to top of upper adhesive layer
   RB=.75
   HBA=.9
   RT=.6
   HT=1.6                   ! Height to table surface
   HS=HT-.2                 ! Height to base of stud hole  
   
   /COM, *** Define Geometry
   DH=.10                   ! Element high
   DANG=11.25               ! 11.25 Degrees
   DR=0.075                 ! Radical length of element
   CYCS,1
   N,1,RB
   NGEN,33,1,1,,,0,DANG
   NGEN,8,100,1,33,1,-DR
   ND1=701
   *DO,I,1,2
    N2I=2**I
    ND2=ND1+32
    NGEN,2,100,ND1,ND2,N2I,-DR
    ND1=ND1+100
   *ENDDO
   ND1=ND1+98
   N,ND1,0
   NGEN,10,1000,1,ND1,1,0,0,DH
   NGEN, 2,1000, 9201, 9000+ND1,1,0,0,DH
   NGEN, 2,1000,10201,10000+ND1,1,0,0,0.002
   NGEN, 3,1000,11201,11000+ND1,1,0,0,DH
   NGEN, 2,1000,13201,13000+ND1,1,0,0,0.002
   NGEN, 5,1000,14201,14000+ND1,1,0,0,DH
   NEGEN=32
  
   MAT,5                    ! WC - Tungsten Carbide (base)
   E,1,2,102,101,1001,1002,1102,1101
   EGEN,NEGEN,1,1
   EGEN,7,100,1,NEGEN,1
   ND1=701
   *DO,I,1,2
    N2I=2**I
    N2IM1=N2I/2
    NEGS=NEGEN/N2I
    ND2=ND1+100
    ND3=ND1+1000
    ND4=ND2+1000
    ND2=ND1+100
    ND3=ND1+1000
    ND4=ND2+1000
    E,ND1,ND1+N2IM1,ND2,ND3,ND3+N2IM1,ND4
    E,ND2,ND2+N2I,ND1+N2IM1,ND4,ND4+N2I,ND3+N2IM1
    
E,ND1+N2IM1,ND1+N2I,ND2+N2I,ND3+N2IM1,ND3+N2I,ND
4+N2I
    *GET,LELM,ELEM,,NUM,MAX    ! Find the last element  
number
    EGEN,NEGS,N2I,LELM-2,LELM,1
    ND1=ND1+100
   *ENDDO
   ND2=ND1+98
   ND3=ND1+1000
   ND4=ND3+98
   *DO,I,1,8
    E,ND1,ND1+N2I,ND2,ND3,ND3+N2I,ND4
    ND1=ND1+N2I
    ND3=ND3+N2I
   *ENDDO
   *GET,LELM,ELEM,,NUM,MAX    ! Find the last element  
number
   EGEN,9,1000,1,LELM,1
   NELM=LELM-64
   *GET,LELM1,ELEM,,NUM,MAX   ! Find the last element  
number
   EGEN,2,1000,LELM1-NELM+1,LELM1,1
  
   MAT,4                      ! MAT 4 is the bdhesive glue
   *GET,LELM1,ELEM,,NUM,MAX   ! Find the last element  
number
   EGEN,2,1000,LELM1-NELM+1,LELM1,1
  
   MAT,3                      ! MAT 4 is the bdhesive glue
   *GET,LELM1,ELEM,,NUM,MAX   ! Find the last element  
number
   EGEN,3,1000,LELM1-NELM+1,LELM1,1
   *GET,LELM1,ELEM,,NUM,MAX   ! Find the last element  
number
  
   MAT,2          ! MAT 2 is B4C - Boron Carbide (table)
   *GET,LELM1,ELEM,,NUM,MAX     ! Find the last element  
number
   EGEN,5,1000,LELM1-NELM+1,LELM1,1
   /PNUM,ELEM,1
   EPLOT
   NUMMRG,NODE
   SAVE
   FINISH
   
  
FLOTRAN Example 1  
   /TITLE,Flow through a Curved Channel
   /UNITS,SI               ! SI units
   /PREP7                  ! Begin PREP7 preprocessing
   ET,1,55                 ! Plane55 Element type
   ! Define pipe dimensions
   D=20                    ! channel width
   R=0.5*D
   RI=40                   ! Radius of curved center line of channel
   D4=D*4                  ! Four times channel width
   RR=R*R
   V0=200
   K,1,,-R
   K,2,,R
   K,3
   L,1,2
   /pnum,line,1
   /pnum,kp,1
   /pnum,area,1
   /pnum,node,1
   lplot
   LESIZE,1,,,16,-4
   ESHAPE,2                ! Quadrilaterals only
   /triad,off              ! turn off coordinate traid at origin
   KPLOT
   K,4,D4+RI
   K,5,D4+RI,D4*2+RI
   L,3,4
   L,4,5
   LFILL,2,3,RI
   LESIZE,2,,,32,0.5
   LESIZE,3,,,48,2.5
   LESIZE,4,,,32
   LPLOT
   ADRAG,1,,,,,,2,4,3
   APLOT
   AMESH,ALL
   
Flow through a Curved Channel
  
FLOTRAN Modeling - Example 2
    /TITLE,Flow through a Curved Pipe
    /UNITS,SI  
    /PREP7
    ET,1,55
    ET,2,70
    ! Define pipe dimensions
    D=20                  ! Pipe diameter
    RI=40                 ! Radius of curved center line of pipe
    D4=D*4                ! Four times diameter length
    RR=(0.5*D)**2
    V0=200
    PCIRC,0.4*D,,0,90
    PCIRC,0.4*D,0.5*D,0,90
    NUMMRG,ALL
    /PNUM,line,1
    /PNUM,area,1
    /PNUM,kp,1
    RR=(0.5*D)**2
    V0=200
    PCIRC,0.4*D,,0,90
    PCIRC,0.4*D,0.5*D,0,90
    NUMMRG,ALL
    /PNUM,line,1
    /PNUM,area,1
    /PNUM,kp,1
    LPLOT
    TYPE,1
    LESIZE,1,,,8
    LESIZE,2,,,8,2
    LESIZE,3,,,8,0.5
    LESIZE,5,,,4,2
    LESIZE,7,,,4,2
    APLOT
    ESHAPE,2
    AMESH,ALL
    ARSYM,X,ALL
    NUMMRG,ALL
    ARSYM,Y,ALL
    NUMMRG,ALL
    NUMCMP,NODE
  
    /pnum,node,1
    /triad,off
    TYPE,2
    K,23,,,D4+RI
    K,24,D4*2+RI,,D4+RI
    L,3,23
    L,23,24
    lplot
    LFILL,13,16,RI
    LESIZE,13,,,16,0.25
    LESIZE,18,,,32
    LESIZE,16,,,24,5
    /VIEW,1,1,1
    VDRAG,ALL,,,,,,13,18,16
    NUMMRG,NODE
    ASEL,S,TYPE,,1
    ACLEAR,ALL
    /pnum,node,0
    /pnum,kp,0
    /pnum,elem,0
    /triad,on
    EPLOT
    VSEL,S,TYPE,,2
    NSLV,S,1
    
  
Flow through a Curved Pipe
  
Hai Tang, last updated December 12, 1995  
  
--
☆ 来源:．大绿 BBS.Dartmouth.Edu．[FROM: Mars.bbs@bbs.Dartmou]