a question about an ANSYS command of applying Boundary conditions

Could you clarify your question?

 One quick thing you can do is: apply the constrainst using the GUI and after that, check the log file and see what Ansys have done.

Mario J Juha

www.eng.usf.edu/~mjuha/

Looking at what you posted, by the time you reach the second select command, Ansys only recognizes all those lines selected by a previous select command.

So insert an ALLSEL command after applying the boundary condition so you make available all the sets of lines for further selection. Hope this helps.

Vgn

Graduate Student

University of Oklahoma

-
Vignesh Ganesan
Computational Mechanics
Universitat Duisburg-Essen
Germany.

Hi Shutao Xing,



Looking at the commands, which is below, are you trying to select the lines from 0 to 0.1 and 0 to 0.9?, if so, your second command will anyway select all the lines from 0 to 0.9.



LSEL,S,LOC,Y,0

LSEL,R,LOC,X,0.1

DL,ALL,,UY



LSEL,S,LOC,Y,0

LSEL,R,LOC,X,0.9

DL,ALL,,UY



you can have look below, S1 is unnecessary if S2 is does the job anyway.



LSEL,S,LOC,Y,0    

!LSEL,R,LOC,X,0,0.1  ![S1]

LSEL,A,LOC,X,0,0.9   ![S2]

DL,ALL,,UY



OR you meant write like this,



LSEL,S,LOC,Y,0

LSEL,R,LOC,X,0,0.1   ![S3]

LSEL,A,LOC,X,0.8,0.9 ![S4]

DA,ALL,,UY



Here, S3 and S4 are different that is S3 is the line from 0 to 0.1 and S4 is the line from 0.8 to 0.9



Or If you want to select 2 or more lines from different location you graphically pick them[GUI] and assign them a component and you can call that component for assigning the boundary condition, for Example,



!Building Component

LSEL,S,LOC,Y,0

LSEL,R,LOC,X,0,0.1   ![S5]

CM,S5,LINE



LSEL,S,LOC,Y,0

LSEL,A,LOC,Z,0.8,0.9 ![S6]

CM,S6,LINE



!Applying Boundary conditions for Selected Components

CMSEL,S,S5

CMSEL,A,S6

DA,ALL,,UY



I guess this might help your case, please write back if you meant something else.



Kind regards,

Vignesh