You can try partitioning the edges of your sheet from the center and apply DOF constraints to them.

If you simulate the parts that hold the sheet (as rigid bodies), you can also try applying a small displacement of the upper part so it presses on the sheet, until you get a reaction effort value that is consistent with the pressure usually applied to ensure tightness for this application.

Thanks Etienne

I partitioned the sheet as you said at first and tried different constrains to model clamp effect. Analysis completes in some cases but the results are not reasonable because the maximum sheet height is much less than the real one.

Could this problem arise from using shell element? I wrote a UMAT for viscoelastic behavior and used it for shell element. could rotations in shell element cause problem? In wrighting UMAT for shell elements except defining relations for stress increment and DDSDDE is there any other point  about rotations in shell elements that i missed?

Hi Mhdi,

Without knowing what you put in you UMAT subroutine I can't tell for sure, but maybe. What I know is that the documentation of the UMAT subroutine specifies you have to define transverse shear stiffness for beam and shell elements. Do you mean sheet thickness when you say sheet height? Or forming height?

As for shell elements, my guesses would be that they're either not well formulated (reduced integration for example) or maybe your mesh is not fine enough?

Hi Etienne

I mean forming height of the bubble.

At the previous hours i tested my code and the process. my material behavior is viscoelastic and material parameters are temperature and shear strain rate dependent. for strain rate dependent i used DSTRAN(3)/DTIME and strain rate in the real process is in the range 0.001-0.5 but when i printed this variable for material point i saw that strain rate in different material points of a single elements is not the same. As you know shell element has section points in the thickness direction. when i printed strain increment in the section point i saw that strain increments are different in section points of each shell element and the magnitude of strain rates in these section points are much bigger than the strain rate range that must be.

I think this is because of the pressure amplitude. do you have any idea about defining pressure amplitude in a way that shear strain rate in the material points becomes in the range 0.001-0.5?

Mhdi,

I know there is an option for defining amplitudes to make them solution dependent, specifying starting, minimal and maximal values. Then, when you affect this amplitude to a certain load (in this case, pressure), you can edit the .inp file and write a CREEP STRAIN RATE CONTROL command below the name of the load and associate it with the name of the amplitude (see documentation, or example with an old version fo ABAQUS here : http://imechanica.org/files/SPF%20Manual.pdf ). You can then specify your target strain rate. You also have to associate it with a set of elements in which you wish to obtain this strain rate. For clarity, define the elements set in the assembly module so you can just copy/paste its name in the options for the CREEP STRAIN RATE CONTROL.

However :

- I've never used that option with shell elements, I don't know if there are subtleties in this case;

-I've only used it in "ideal isothermal" cases where my creep law parameters are therefore considered constant, so I don't know how heavy the effect of thermal dependence can be on the computation times.

-I've also only used it for CREEP materials (ie materials in temperature ranges where elasticity is neglected), I don't know if this is suited for a VISCOELASTIC material. Maybe there is an equivalent option for this kind of material.

Anyways good luck

Also one thing : note that this strain rate control option will modify the pressure in order for the greatest amplitude of strain rate in your element set to be between 0.7-8 and 1.5 times the target value. The greater the element set, the more spread your actual strain rate values will be.

Thanks so much my friend for your valuable information.