ansys的常用命令介绍

ansys的常用命令介绍

/PREP7 前处理的一些常用命令：

   ET，1，SOLID45 定义单元类型

   KEYOPT,1,2,1 单元选项（OPTION）

   MP,EX,1,100 定义材料参数，1为材料号

   tb， 材料表（定义塑性、超弹性等）

   *dim,rr,array,3，2 定义数组rr为3行2列

   k,1,X，Y，Z 定义KEYPOINT1坐标

   LSTR，1，2 由1、2点生成线

   lesize 划分网格，尺寸定义

   NUMMRG,KP, , , ,LOW 压缩节点号

   asel ， 选择面

   r， 定义实常数

   wpro,,-90, 旋转工作平面

   esln,s 选择与节点相关的单元

   emodif,all,real,i 修改单元实常数

   amesh 对面划分网格

   type,2
   mat,2
   real,1
   esys,0 （或 aatt） 激活单元类型2，材料号2，实常数1，单元坐标系

   vsweep,all,,, 扫掠网格

   csys,4 激活坐标系4
/prep7
numstr,kp,100 !define the following keypoint number start with with the 100
l,1,2,4 !如果CSYS=0则生成直线,如果CSYS=1则生成弧线,这个命令与当前的坐标系统有关而楼上师兄的 LSTR 则始终生成直线.
                  
lsel , !取线
wprof,,12 !移坐标
alsv !拾取一选定实体上的所有面
nsla !同理,拾取一选定面上的所有节点
aatt,1,1,1 !等效于楼上的 MAT,1 TYPE,1 REAL, 1对面定义属性

mshke,0
                         !网格格划分进行限定:采用FREE进行划分;网格形状为 四 边形或六面体
mshape,1,2d
vmesh ,2 !划分实体网格,后面的参数是实体编号如:2
/solu !进入求解过程
antype,static !选择求解类型为静力分析
asel,s,loc,x,
nsla
d,all,uy,,,,,roty,rotz !对选定的面上的所有节点施加UY ROTY ROTZ 的对称约束.
allsel !恢复全部选择等效于:ASELL,ALL ESEL,ALL NSEL,ALL
asel,s,,,1
sfa,all,1,press,1000 !对选定的面1施加均布力1000
allsel
/stat,slou !显示求解状况
solve
/post1 !进入后处理
set,list !列出求解的步数及相关信息
set,last !读取最后一步结果
plns,s,eqv,,1 !绘出节点的等效应力云图
plns,epto,eqv !绘出节点的等效应变云图
/post26 !进入时间后处理器
plvar,2 !对以定义的变量2用曲线绘出

/exit,save !退出并存盘

------------------------------------------------------
BEGINNER'S GUIDE TO ANSYS COMMANDS
The symbol '*' corresponds to the following:

* --> k, l, a, v, e, n, cm, et, mp, r where ==>
k --> Keypoints
l --> Lines
a --> Area
v --> Volumes
e --> Elements
n --> Nodes
cm --> component
et --> element type
mp --> material property
r --> real constant
$ --> d, f, sf, bf, ic, where ==>
d --> DOF constraint (ux... in Structural, Temp in thermal,
f --> Force Load ( Heat in thermal)
sf --> Surface load on nodes
bf --> Body Force on Nodes
    
More Commands can be generated by sensible combinations of " $* " family of commands. See the following list of $* possible options
      
$* --> dk --> DOF constraints on KP (Vx,Vy,Pres... in CFD)
dl --> DOF constraints on Lines
da --> DOF constraints on Areas
fk --> Force on Keypoints
sfl --> Surface load on Lines
sfa --> Surface load on Areas
sfe --> Surface load on element faces
bfk --> Body Force on Keypoints
bfl --> Body Force on Lines
bfa --> Body Force on Area
bfv --> Body Force on Volumes
bfe --> Body Force on Elements
ic --> Initial Conditions ",

p" --> If ",p" was issued at the end of the Command(in Input Window) the GUI based picking menu will be activated. Useful for listing, plotting, meshing, deleting, etc..

**********************************************************

1. Listing of picked Entities:
COMMAND SYNTAX: *LIS,p & $*LIS,p
A few Combinations of this command are:

klis,p --> List KP
llis,p --> Lists Lines
alis,p --> Lists Areas
vlis,p --> Lists Volumes
elis,p --> Lists Elements
nlis,p --> Lists Nodes
cmlis,p --> Lists components
cslis,p --> Lists user created local co-ordinate systems
dlis,p --> Lists DOF constraints specfied on nodes
dalis,p --> Lists DOF constraints applied on Areas
flis,p --> Lists force on Nodes
sfllis,p --> Lists Surface Load on lines
bfalis,p --> Lists body force load applied on Areas
iclis,p --> Lists Initial condition on Nodes
    
If ",p" was not issued, all entites currently selected will be listed.
For certain commands ",p" cannot be issued. See the below mentioned commands
    
etlis --> Lists the different element types defined
mplis --> Lists whatever Material properties
rlis --> Lists whatever real constants
cslis --> Lists all co-ordinate systems
cmlis --> Lists all components

*********************************************************

2. Plotting of Entities: COMMAND SYNTAX: *plo KPLO / LPLO / APLO / VPLO / EPLO / NPLO / CMPLO /

**********************************************************

3. deleting of Entities:
COMMAND SYNTAX: *DEL,p & $*DEL,p
KDEL,p / LDEL,p / ADEL,p / VDEL,p / EDEL,p / NDEL,p / CMDEL,p / DDEL,p /
DKDEL,p / DADEL,p / FDEL,p / SFDEL,p / SFEDEL,p / SFADEL,p / SFLDEL,p /
BFADEL,p / ......
The syntax for this command is very similar to LISTING command.

**********************************************************

4. distance between two entities:
COMMAND SYNTAX: *DIS,p
ndis,p --> Distance between two nodes
kdis,p --> Distance between two KPs

**********************************************************

5. Meshing of geometries:
COMMAND SYNTAX: *MES,p
KMES,p / LMES,p / AMES,p / VMES,p

**********************************************************

6. Size settings for Lines and Areas before meshing :
COMMAND SYNTAX : *size,,p Lesiz,p / Aesize,p

*********************************************************

7. Clearing Meshes of already meshed geometries:
COMMAND SYNTAX: *CLE,p KCLE,p / LCLE,p / ACLE,p / VCLE,p

**********************************************************

8. BOOLEAN Operations: Intersect
COMMAND SYNTAX : *IN* AINA,p / VINV,p / LINL,p / AINV,p / LINV,p / LINA,p

**********************************************************

9. BOOLEAN Operations: GLUE
COMMAND SYNTAX : *GLUE VGLUE,p / AGLUE,p / LGLUE,p

**********************************************************

10. Boolean Operations: SUBTRACT/DIVIDE:
COMMAND SYNTAX: *sb*,p See the following examples to understand how this works:
asba,p --> Subtract Area from Area
asbl,p --> Divide Area by line
vsba,p --> Divide volume by Area
lsbw,p --> Divide line by Workplane
vsbw,p --> Divide volume by Workplane
asbw,p --> Divide area by Workplane
vsbv,p --> subtract Volume by another volume
More combinations exist. The user needs to explore them for themselves --> forms a part of learning

**********************************************************

11. Boolean Operations: Overlap:
COMMAND SYNTAX: *OVLAP,p AOVLAP,p / VOVLAP,p

**********************************************************

12. Concatenation of Lines / Areas --> for map meshing
COMMAND SYNTAX : *ccat,p
LCCAT,p --> Concatenation of Lines for Map meshing Area
ACCAT,p --> Concatenation of Areas for Map meshing Volume

*********************************************************

13. Dragging operation
COMMAND SYNTAX : *drag,p
vdrag,p --> Drag areas along a line to create a new volume
adrag,p --> Drag line along a line to create a new area
ldrag,p --> Drag KP along a line to create a new line

**********************************************************

14. Copy Geomtric entities
COMMAND SYNTAX : *GEN,,p
KGEN,,p / LGEN,,p / AGEN,,p / VGEN,,p
Please note that *GEN commands are also used for MOVE operations. The difference lies in the value specified in the 10th field of these *GEN commands. By default it is 0 --> which does the COPY operation. If specfied as 1 --> it does the MOVE operation

**********************************************************

15. Bottom -to- Top modeling commands:
COMMAND SYNTAX : *,p & **,p
k,p ---> Allows user to pick KP in the Workplane
l,p ---> Create lines from existing KP
ak,p ---> Create area from KP
al,p ---> Create area from lines
v,p ---> Create Volume from KP
va,p ---> Create Volume from Areas
e,p ---> Create Elem from existing nodes
en,p ---> Create Elem from nodes

**********************************************************

16. To apply common Boundary Conditions such as DOF constraint, Forces, Surface Loads, Bodyforce Loads and Initial conditions
* --> is meant for the KLAVE entities only (KLAVEN stands for KP, Lines, Area, Volumes & ELem )
16a. DOF constraint :
COMMAND SYNTAX : $*,p ( Please Note: NOT all * are valid)
See the valid combinations below:
D,p --> To apply DOF on nodes
DK,p --> To apply DOF on Keypoints
DL,p --> Apply DOF on Lines
DA,p --> Apply DOF on Areas ( symmetry or Anti-symmetry will be prompted)
****************
16b. FORCE Loading:
COMMAND SYNTAX : $*,p
See the valid combinations below:
f,p --> Forces on nodes
fk,p --> Force on Keypoints
(fa,p or FV,p or FL,p ----> Since force cannot be applied on Lines or Area & volumes... this command does not exist.)
****************
16c. Surface Loads:
COMMAND SYNTAX : $*,p
See the valid combinations below:
sf,p --> Surface Load on a set of Nodes
sfl,p --> Surface Load on Lines
sfa,p --> Surface Load on Area
sfe,p --> Surface Load on Element
(SFk,p and SFV,p do not exist since pressure cannot be applied on a single Kp and neither can it be applied on a volume)
****************
16d. BodyForce Load: COMMAND SYNTAX : bf*,p
See the valid combinations below:
bf,p --> Bodyforce Load on a set of Nodes
bfk,p --> Bodyforce Load on KP
bfl,p --> Bodyforce Load on Lines
bfa,p --> Bodyforce Load on Areas
bfv,p --> Bodyforce Load on Volumes
bfe,p --> Bodyforce Load on Element
****************
16e. Initial conditions:
ic,p --> Initial Conditions on Nodes
(P.S: Initial Conditions can be applied only to nodes. )

***********************************************************

17. To refine a mesh :
COMMAND SYNTAX : *ref,p
kREF,p / kREF,p / aREF,p / eREF,p / nREF,p

***********************************************************

18. To TRANsfer loads from the Solid model to the FE model:
COMMAND SYNTAX : $TRAN
dtran / ftran / sftran / bftran & SBCTRAN
(SBCTRAN --> Transfers all solid model loads to FE model)

***********************************************************

19. Writing / Reading information to a file (ASCII)
COMMAND SYNTAX : *read, & *write,
NWRITE / MPWRITE / ETWRITE / RWRITE / EWRITE / CDWRITE
NREAD / MPREAD / ETREAD / RREAD / EREAD / CDREAD / LDREAD
(Some of these commands ETWRITE/ETREAD , RWRITE/RREAD are undocumented. But they do work) The Commands CDWRITE and CDREAD are used to write/read all FE model related info (w or w/o geometry to ASCII files) Its recommended the user read the online help on these two commands before using them
The LDREAD commands are used to read loads (LD) from other analysis types. For example: Temp from Thermal results file (*.rth) are applied onto Structural elements.