Coupling Shell/Sold elements

[pepette]

Hi all,

I am using Ansys classic to model the mecanical behavour of a membrane. The assembly is composed by a strongback (it looks like a square mesh), in this part, a thick film of polymer is glue and a pressure is applied.
So to model with Ansys the mechanical behavour, I use solid element for the strongback and shell element for the membrane. My problem is to model the contact between the membrane and the strongback. I would like to know if it is better to use the CP command or the contact wizard?

The aim of this study is to know the influence of stiffness of the strongback.

Thank you for your help

 

[meshparts]

I would try two variants:

1. No contacts and no cp's. Just Mesh the area with shels and then the volume with tets

2. Contact elements with friction

Then compare the results. I assume that the first variant will give similar results with variant 2.

Regards,
Alex

 

[doatis]

You could also try using the SOLSH190 elements. They are 8-noded brick elements with a shell formulation. Then, all you have to do is glue the volumes together, and the DOFs will be transferred across through the shared nodes.

Hope this helps,
Doug

 

[pepette]

If I do not use some CP's or contact elements, the membrane is not supported any more by the strongback. Probably I do not understand waht you mind...sorry for my english...

This is my apdl file with a simple geometry and with no contacts and CP's, it probably help you to understand my problem.

Regards,

FINI
/CLEAR
/TITLE,
/PREP7
!______________________________________________________________
!!!!Parametres
*SET,e,0.003
*SET,em,0.000015
*SET,p,350000
*SET,a,0.052
*SET,l,0.003
*SET,b,0.005
!______________________________________________________________
!------------------------------------------!
! MATERIAU 1=PP Pa !
!------------------------------------------!
!MATERIAU 1=316LN Pa
UIMP,1,EX, , ,193E9,
UIMP,1,DENS, , ,8000,
UIMP,1,NUXY, , ,0.272,
ET,1,solid95

!MATERIAU 2=Film PP
UIMP,2,EX, , ,100E9,
UIMP,2,DENS, , ,8000,
UIMP,2,NUXY, , ,0.49,
ET,2,SHELL93
R,2,em, , , , , , !epaisseur membrane
!------------------------------------------!
! Geometry !
!------------------------------------------!
RECTNG,a/2-e/2,a/2+e/2,0,a,
RECTNG,0,a,a/2-e/2,a/2+e/2,
AADD,1,2
VOFFST,3,b,,
RECTNG,0,a,0,a,

ESIZE,e,0,
MSHAPE,1,3D
MSHKEY,0
VSWEEP,1

AATT,2,2,2,0,
*DO,i,0,3
LESIZE,37+i,,,19,
*ENDDO
MSHAPE,0,2D
MSHKEY,0
AMESH,15
!------------------------------------------!
! Loads !
!------------------------------------------!
SFA,15,,PRES,(100000),,
*DO,i,0,3
DL,37+i,15,ALL,0,0
*ENDDO
*DO,i,0,3
DA,4+3*i,ALL,,
*ENDDO
FINISH

/SOL
!NLGEOM,ON
SOLVE
FINISH

 

[meshparts]

You must first mesh the areas and then the volumes!

FINI
/CLEAR  
/TITLE,  
/PREP7
!______________________________________________________________
       !!!!Parametres
*SET,e,0.003
*SET,em,0.000015        
*SET,p,350000      
*SET,a,0.052         
*SET,l,0.003     
*SET,b,0.005     
!______________________________________________________________
           !------------------------------------------!
           !            MATERIAU 1=PP    Pa           !
           !------------------------------------------!
!MATERIAU 1=316LN Pa
UIMP,1,EX, , ,193E9,
UIMP,1,DENS, , ,8000,   
UIMP,1,NUXY, , ,0.272,
ET,1,solid95

!MATERIAU 2=Film PP
UIMP,2,EX, , ,100E9,
UIMP,2,DENS, , ,8000,   
UIMP,2,NUXY, , ,0.49,  
ET,2,SHELL93
R,2,em, , , , , , !epaisseur membrane
           !------------------------------------------!
           !                Geometry                  !
           !------------------------------------------!

RECTNG,a/2-e/2,a/2+e/2,0,a,
RECTNG,0,a,a/2-e/2,a/2+e/2,
AADD,1,2
VOFFST,3,b,,

! changed:
RECTNG,0,a/2-e/2,0,a/2-e/2
RECTNG,a/2+e/2,a,a/2+e/2,a
RECTNG,0,a/2-e/2,a/2+e/2,a
RECTNG,a/2+e/2,a,0,a/2-e/2
nummrg,kp

MSHAPE,0,2D
MSHKEY,0
asel,s,loc,z,0
AATT,2,2,2,0,
esize,e
AMESH,all
alls

ESIZE,e,0,
MSHAPE,1,3D
MSHKEY,0
VSWEEP,1
! :changed

 

[pepette]

mihaiupb, thank you so much for your help.

And now if I want to model the global displacement of the strongback, I must to use the CP's?

 

[meshparts]

No CP's are necessary. Lok at the mesh with node numberings on. All Nodes on the interface of shells to solid are common to shells and solid elements.

Regards,
Alex

 

[pepette]

The reults with your method are very good !
Thank you for your help Alex !

Cheers