Residual stress

[izyk]

Hi
I don't know how to apply a residual stress to a membrane. I used a ISTRESS command but it didn't affect on membrane deflection.
Here is a script i've used:

FINISH
/CLEAR

Lm=300
Wm=300
Tm=5

b=30

/PREP7

ET,1,SHELL181
R,1,Tm

MP,EX,1,130e+9*1e-6
MP,DENS,1,2330*1e-18
MP,PRXY,1,0.278

RECTNG,0,Lm,0,Wm

LESIZE,ALL,,,b,-5

MSHAPE,0,2D
MSHKEY,1
AMESH,ALL

NSEL,S,LOC,X,0
NSEL,A,LOC,X,Lm
NSEL,A,LOC,Y,0
NSEL,A,LOC,Y,Wm

D,ALL,UX,0
D,ALL,UY,0
D,ALL,UZ,0
D,ALL,ROTX,0
D,ALL,ROTY,0
D,ALL,ROTZ,0

ALLSEL,ALL

SFA,1,1,pres,300000*1E-6

ISTRESS,1000,1000,1000, , ,

FINISH

/SOLU
ANTYPE,STATIC
SOLVE
FINISH

 

[jiligeo]

Hi, I think you have to use Inistate command instead of istress for new elements (18+).

Regards
Jalil

 

[izyk]

There is no INISTATE command in Ansys v10.

 

[jiligeo]

Hi, it is right at v. 10. I am using v. 11 and in this vers. “The ISTRESS command is being replaced by INISTATE.”
I have checked the v. 10 manual. In manual v. 10 is written, Istress is available only in solution phase. (but you have used that in /PREP7). Try to use the Istress in solution phase.

Hope that help you.

 

[izyk]

Ok, now it works.
The first problem was this what jiligeo have noticed. The second thing is that the initial stress is applied to a material. So i had to simulate a membrane with a substrate.
Another question.
Does anybody know what values od stress should i use to simulate a membrane made of a material deposited on substrate? It means that stress appears due to difference between thermal dillatation coefficients. For example i would like to introduce 60MPa of residal stress. Should I use X and Y values only? What about XY and others?

 

[izyk]

Probably I've found the solution. To describe the residual stress due to difference between thermal dilatation coefficients in layers, one use Sx and Sy because the membrane is stretched / squeezed only in XY plane.
Simulation (using solid elements) of silicon membrane 300x300x5um with oxide substrate 600x600x20um gives following results:

applied pressure (kPa), applied residual stress Sx and Sy (MPa), maximal deflection (nm)

0kPa, 0MPa, 0nm
0kPa, 10MPa, 7.2nm
300kPa, 0MPa, 224nm
300kPa, 10MPa, 231nm

It seems that these results are correct, but now i can't understand why simulation (using shell elements) of membrane perfectly clamped (without substrate) gives different results:

0kPa, 0MPa, 0nm
0kPa, 10MPa, e-10nm - membrane is wrinkled
300kPa, 0MPa, 209nm
300kPa, 10MPa, 209nm - deformation doesn't change with applied stress, stress adds to the stress resulting from applied pressure on whole membrane

Is it normal? If one consider the equation of perfectly membrane (Timoshenko theory):

D*h^3*$$w + S*h*$w = P

where: D - rigidity, h - membrane thickness, S - residual stress, $ - Laplace operator, P - pressure

the deflection should change in case of applied residual stress if applied pressure is not zero. If P=0 the membrane should remain flat irrespective of applied residual stress.

Regards

 

[izyk]

Found a solution. A nonlinear simulation must be used.