General Mechanical

General Mechanical

Topics related to Mechanical Enterprise, Motion, Additive Print and more.

how to apply pressure boundary conditions to the nodes with table form.

    • TYUST10086
      Subscriber

      the pressure curve was given, and i want to apply this pressure data to the specific nodes, thank you.

    • Erik Kostson
      Ansys Employee
      use the nodal pressure load object as shown below:

      All the best

      Erik
    • TYUST10086
      Subscriber
      Thank you for your kind answers. the simulation was performed in ANSYS APDL experiment. as show below Fig.1
      Fig.1
      the red arrows shows the pressure conditions and the results shows the applied pressure values are constant values, as shown in Fig.2
      Fig.2
      while I applied the following command to apply the given pressure data (for simplification, I defined two points ) to the nodes: 1, 3,4,5,6,7,8,9,10,11
      *DIM,eqps,TABLE,2,1,1
      *TREAD,eqps,fps,TXT,,1
      FLST,2,10,1,ORDE,3
      FITEM,2,1
      FITEM,2,3
      FITEM,2,-11
      SF,P51X,PRES, %EQPS%
      the results was wrong, as illustrated in Fig.2 . which should not be constant. thank you.


    • Erik Kostson
      Ansys Employee
      HI

      It is just a visual thing - you can display a table.
      Just look on the reactions (@fixed nodes) when it is solved in POST1/ and see that it is changing with time - make your table like 0 , 5E8, 0.5 s, 5E8 Pa, and 1.5 s1E9 Pa, and 2 say s 1.9E9.

      The reaction should change for different time say @ 0.5 s compared to 2 s.


    • TYUST10086
      Subscriber
      the static structural mechanical analysis simulation was performed in ANSYS APDL environment. I have upload the corresponding APDL command. The displayed applied table pressures should not be constant. I have seen some similar results as shown below: its values were different, thank you very much.


    • Erik Kostson
      Ansys Employee
      HI

      Ansys employees are not allowed to download files - perhaps other members can help you looking at the files (we can not)

      I think you talk about variation along a dimension not time.

      I am not sure if it works , but in the *dim table you need to tell it it is a position table by default it is a time table - see *dim for more info.

      Thank you

      Erik
    • TYUST10086
      Subscriber
      yes, you are right. I want to apply the variational pressures along the selected nodes dimension. as below
      /PREP7
      ET,1,PLANE182
      !*
      KEYOPT,1,1,0
      KEYOPT,1,3,2
      KEYOPT,1,6,0
      !*
      MPTEMP,,,,,,,,
      MPTEMP,1,0
      MPDATA,EX,1,,2e11
      MPDATA,PRXY,1,,0.3
      K,100,,,,
      K,101,12,,,
      K,101,12,-3,,
      K,101,12,,,
      K,102,12,-3,,
      K,103,0,-3, FLST,2,4,3
      FITEM,2,100
      FITEM,2,101
      FITEM,2,102
      FITEM,2,103
      A,P51X
      TYPE,1
      MAT,1
      REAL,
      ESYS,0
      SECNUM,
      !*
      FLST,5,1,4,ORDE,1
      FITEM,5,2
      CM,_Y,LINE
      LSEL, , , ,P51X
      CM,_Y1,LINE
      CMSEL,,_Y
      !*
      LESIZE,_Y1,1, , , , , , ,1
      !*
      FLST,5,1,4,ORDE,1
      FITEM,5,1
      CM,_Y,LINE
      LSEL, , , ,P51X
      CM,_Y1,LINE
      CMSEL,,_Y
      !*
      LESIZE,_Y1,1, , , , , , ,1
      !*
      MSHAPE,0,2D
      MSHKEY,1
      !*
      CM,_Y,AREA
      ASEL, , , ,1
      CM,_Y1,AREA
      CHKMSH,'AREA'
      CMSEL,S,_Y
      !*
      AMESH,_Y1
      !*
      CMDELE,_Y
      CMDELE,_Y1
      CMDELE,_Y2
      !*
      ESIZE,0.5,0 CM,_Y,AREA
      ASEL, , , ,1
      CM,_Y1,AREA
      CHKMSH,'AREA'
      CMSEL,S,_Y
      !*
      !*
      ACLEAR,_Y1
      AMESH,_Y1
      !*
      CMDELE,_Y
      CMDELE,_Y1
      CMDELE,_Y2
      !*
      FINISH
      /SOL
      FINISH
      /PREP7
      FINISH
      /SOL
      !*
      ANTYPE,0
      !*
      !*
      NLGEOM,0
      NROPT,AUTO, ,
      LUMPM,0
      EQSLV, , ,0, ,DELE
      MSAVE,0
      PCGOPT,0, ,AUTO, , ,AUTO
      PIVCHECK,0
      PSTRESS,0
      TOFFST,0,
      !*
      FLST,2,1,4,ORDE,1
      FITEM,2,3
      !*
      /GO
      DL,P51X, ,ALL,0
      !
      *DIM,eqps,TABLE,2,1,1
      *TREAD,eqps,fps,TXT,,1
      !
      FLST,2,10,1,ORDE,3
      FITEM,2,1
      FITEM,2,3
      FITEM,2,-11
      /GO
      !*
      !*
      SF,P51X,PRES, %EQPS%
      OUTRES,ALL,ALL,
      !*
      TIME,1
      AUTOTS,1
      NSUBST,50,200,50,1
      KBC,0
      !*
      TSRES,ERASE
      LSWRITE,1,
      SOLVE

    • Erik Kostson
      Ansys Employee
      So you need to have a position table not time like you have now.

      See the *dim command and the options there (time,x,y,z).

      An example is below where the load varies along Z:

      --
      /PREP7
      !*
      ET,1,SOLID185
      !*
      !*
      MPTEMP,,,,,,,,
      MPTEMP,1,0
      MPDATA,EX,1,,200E9
      MPDATA,PRXY,1,,0.3
      /REPLOT,RESIZE
      BLOCK,0,1,0,1,0,1,
      VMESH,ALL

      *DIM,my_conv,table,3,1,1,Z! 3 rows, One Column, function of Z
      !
      ! Zero out the ÔÇ£zerothÔÇØ row values for neatness
      my_conv(0,1)=0.0
      !
      ! Enter the Z locations
      my_conv(1,0)=0! start loc
      my_conv(2,0)= 0.5! 0.5 m
      my_conv(3,0)= 1! 1 m
      !
      ! Enter force
      my_conv(1,1)=0
      my_conv(2,1)=100.0
      my_conv(3,1)=200.

      NSEL,S,LOC,Y,0
      sf,ALL,pres,%my_conv%
      ALLSEL,ALL
      NSEL,S,LOC,Y,1
      d,all,all
      OUTRES,ALL,ALL
      /SOLU
      solve
      --
Viewing 7 reply threads
  • The topic ‘how to apply pressure boundary conditions to the nodes with table form.’ is closed to new replies.