Cantilever wih a Shell Element

[SandeepNagaraj]

Hi all!!

I am trying to solve a simple cantilever with a point load at the free end and understand feap commands before I go further. I am getting stuck with this file and not able to compute the results. It would be really helpful if someone could help me out with this. The following is my input file.

***********************************
FEAP * * Cantilever beam with point load(Shell Element)
0 0 0 3 2 4

PARA
 l = 500
 b = 40
 hd = 10
 vd = 2

BLOC 1
 CART hd vd 0 1 1 0 0
 1 0 0
 2 l 0
 3 l b
 4 0 b

EBOUN
 1 0.0 1 1 1
 
FORC
 11 0.0 0.0 -1000

MATE 1
 SHEL
 ELAS ISOT 200000.0 0.25
 THIC 30
 
END
INTE
STOP
***********************************

Thank you!!

[FEAP_Admin]

If you really want to use the shell in 3D (ndm=3) then you need to (1) generate the geometry in 3D and (2) set the number of dofs to 6 (ndf=6).
You also need to restrain the displacements and the rotations at the clamped end.

[SandeepNagaraj]

Hello Admin!!
I tried to build the 3d mesh, and set the dof to 6 and also have constrained the appropriate nodes and also distributed the load equally.
Im still not able to solve it.
Kindly help me.
**********************************************************
FEAP * * Cantilever beam with point load(Shell Element)
0 0 0 3 6 4

PARA
 l = 500
 b = 40
 w = 30
 hd = 5
 vd = 3
 ud = 2

BLOC 1
 CART hd vd ud 0 1 1 0 0
 1 0 0 0
 2 l 0 0
 3 l b 0
 4 0 b 0
 5 0 0 w
 6 l 0 w
 7 l b w
 8 0 b w

EBOUN
  1 0.0 1 1 1 1 1 1
  7 0.0 1 1 1 1 1 1
 14 0.0 1 1 1 1 1 1
 21 0.0 1 1 1 1 1 1
 25 0.0 1 1 1 1 1 1
 31 0.0 1 1 1 1 1 1
 37 0.0 1 1 1 1 1 1
 43 0.0 1 1 1 1 1 1
 
FORC
  6 0.0 0.0 -500 0.0 0.0 0.0 0.0
 30 0.0 0.0 -500 0.0 0.0 0.0 0.0

MATE 1
 SHEL
 ELAS ISOT 200000.0 0.25
 THIC 30
 
END
INTE
STOP
**************************************************

[Prof. R.L. Taylor]

You have a couple of errors.  You can find some of them by looking at the output file and sometime in the log file.  Check them carefully after you run a problem.

!. Your shell has no thickness:  THICK,,30

2. Shells are 3-d bodies but only surfaces.  You are generating solid elements In your BLOC command only input the first 4-nodes.  Also telling feap what element you will use is a help in the block command.

        BLOCk
            CART .....
                QUADrilateral 4
                     1  0.0   0.0
                      .....

tells feap you are using 4-node quadrilaterals (the only thing shells can understand).

Your load may not be in the direction you want -- use plot commands to see the mesh boundary conditions and loads (or look in the output file to make sure they are in directions where you expect them

[SandeepNagaraj]

Dear Admin,

Thank you very much for your time and kind suggestions.

I will incorporate your suggestions and get back to you. I hope this should not be a problem.

Thanks again.

Regards,
Sandeep N.

[SandeepNagaraj]

Dear Admin,
Iv incorporated the corrections as you have suggested and found them to work. Iv confirmed the results with Hand calculations. The following is the content of the new input file. I hope they are in the right form.
**********************************
FEAP * * Cantilever beam with point load(Shell Element)
0 0 0 3 6 4                  ! 3d

PARA
 l = 500                     ! Length of the beam
 b = 40                  ! Breadth of the beam   
 hd = 15                    ! No. of elements - Horizontal direction
 vd = 3                     ! No. of elements - Vertical direction 

BLOC 1
 CART hd vd
  QUAD 4
   1 0 0
   2 l 0
   3 l b
   4 0 b
 
EBOUN                       
  1 0.0 1 1 1 1 1 1         ! Fully restraining all dof
 
CFORC
Node  500 0.0 0.0 0.0 -1000 0.0 0.0 0.0 0.0  ! Load of 1000kN -ve Y-direction

MATE 1
 SHEL
 ELAS ISOT 200000.0 0.25
 THIC,,30                   ! Shell thickness
 
END
INTE
STOP
**********************************
Thank you for the help.

Regards,
Sandeep N.