Laminated glass

[kribri]

Hi,
I hope someone can help me with this.

I'm analysing Monolithic glass vs Laminated glass.
I'm looking at a window of the size 800x1600mm.
The monolithic is 8mm thick.
The laminate consists of glass faces and is glued together with PVB. The laminate is 4+0.76+4mm.
Isotropic Glass material properties are: E=70GPa, v=0.23
Isotropic PVB material properties are: E=3.78MPA, v=0.49

When modelling this with shell elements (composite layup) in Abaqus the results does not make sense. (I ran a test where the monolithic window was stiffer than the laminate with double the thickness)

For the shell model elements I understand that the elements use first order shear deformation theory for transverse shear deformation. This assumes that plane sections remain plane, but can rotate relative to the shell surface. The shear stiffness is adjusted to compensate for the fact that the real deformation violates this assumption, but the adjustment is approximate. It is claimed to work for normal lay-ups, including sandwich lay-ups, but I have clearly gone far beyond the limits of validity of the procedure used - there is simply far too much shear deformation concentrated into the thin adhesive layer.

Any suggestions on how this can be modelled? Either as solid or as shell?

kind regards
Krish

 

[rstupplebeen]

Krish,

My guess is that the huge disparity between the moduli of the glass and the PVB is causing issues with the laminate. Are you sure that the modulus of PVB is appropriate for this application (thin under high shear)?

How large is the window you are simulating considering symmetry planes? You may be able to use continuum shells or solids depending on your model size and desired solve time.

I hope this helps.

Rob Stupplebeen

 

[kribri]

Hi Rob, thank you for responding.

The modulus of the PVB is an debatable value. Research presents values from 0.5MPa to 0.95GPa(!!!). I chose a value based on a Shear Modulus equation which depends on temperature (G=1.1GPa) and used Hooke's law(-> E=3.78MPa).

The window size I've been looking at is 800x1600mm.
My desired solve time could be quite long (several hours is okay).

The analysis I have performed so far shows a significant difference in stiffness (factor of 2) based on how fine the mesh is.
For the PVB layer, any suggestions of number of elements through thickness and maximum aspect ratio?

Krish

 

[rstupplebeen]

Since you have no idea what the modulus is for the PVB you will have to tune the model with this parameter once you get closer to a realistic solution. I would start at the stiffer end and work from there because the solutions should converge better and it really is a guess where to start.

Use quarter symmetry and possibly a much smaller panel for initial simulations.

3 elements through the thickness for bending is the general rule of thumb. With your situation with widely differing stiffnesses you will need to prove if this is appropriate (it probably isn't). For aspect ratios I usually strive for 1:4 or less but to start I would go with 1:10. You will have a fair amount of mesh sensitivity studies ahead of you to dial this in.

So start stiff and coarse and work from there.

What is the loading and constraints on the model? I hope this helps.

Rob Stupplebeen

 

[kribri]

The constraints are simply supported with pull in.
And the loading is 2.5kN/m2 (uniform pressure)

Conventional shell elements(S4R in abaqus) and solid elements (C3D8R) will not provide a reliable result. Should this be modelled with continuum shell elements?

Krish