ansys的常用命令介紹

/PREP7 前處理的一些常用命令：

   ET，1，SOLID45 定義單元類型

   KEYOPT,1,2,1 單元選項（OPTION）

   MP,EX,1,100 定義材料參數(shù)，1為材料號

   tb， 材料表（定義塑性、超彈性等）

   *dim,rr,array,3，2 定義數(shù)組rr為3行2列

   k,1,X，Y，Z 定義KEYPOINT1坐標(biāo)

   LSTR，1，2 由1、2點生成線

   lesize 劃分網(wǎng)格，尺寸定義

   NUMMRG,KP, , , ,LOW 壓縮節(jié)點號

   asel ， 選擇面

   r， 定義實常數(shù)

   wpro,,-90, 旋轉(zhuǎn)工作平面

   esln,s 選擇與節(jié)點相關(guān)的單元

   emodif,all,real,i 修改單元實常數(shù)

   amesh 對面劃分網(wǎng)格

   type,2
   mat,2
   real,1
   esys,0 （或 aatt） 激活單元類型2，材料號2，實常數(shù)1，單元坐標(biāo)系

   vsweep,all,,, 掃掠網(wǎng)格

   csys,4 激活坐標(biāo)系4
/prep7
numstr,kp,100 !define the following keypoint number start with with the 100
l,1,2,4 !如果CSYS=0則生成直線,如果CSYS=1則生成弧線,這個命令與當(dāng)前的坐標(biāo)系統(tǒng)有關(guān)而樓上師兄的 LSTR 則始終生成直線.
                  
lsel , !取線
wprof,,12 !移坐標(biāo)
alsv !拾取一選定實體上的所有面
nsla !同理,拾取一選定面上的所有節(jié)點
aatt,1,1,1 !等效于樓上的 MAT,1 TYPE,1 REAL, 1對面定義屬性

mshke,0
                         !網(wǎng)格格劃分進(jìn)行限定:采用FREE進(jìn)行劃分;網(wǎng)格形狀為 四 邊形或六面體
mshape,1,2d
vmesh ,2 !劃分實體網(wǎng)格,后面的參數(shù)是實體編號如:2
/solu !進(jìn)入求解過程
antype,static !選擇求解類型為靜力分析
asel,s,loc,x,
nsla
d,all,uy,,,,,roty,rotz !對選定的面上的所有節(jié)點施加UY ROTY ROTZ 的對稱約束.
allsel !恢復(fù)全部選擇等效于:ASELL,ALL ESEL,ALL NSEL,ALL
asel,s,,,1
sfa,all,1,press,1000 !對選定的面1施加均布力1000
allsel
/stat,slou !顯示求解狀況
solve
/post1 !進(jìn)入后處理
set,list !列出求解的步數(shù)及相關(guān)信息
set,last !讀取最后一步結(jié)果
plns,s,eqv,,1 !繪出節(jié)點的等效應(yīng)力云圖
plns,epto,eqv !繪出節(jié)點的等效應(yīng)變云圖
/post26 !進(jìn)入時間后處理器
plvar,2 !對以定義的變量2用曲線繪出

/exit,save !退出并存盤

------------------------------------------------------
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.