Discussion Forum

Hi

if I understand youre model you have a thin membrane (lets say th=1e-3m thick, and R=1m radius, in default steel or any other material) represented in 2D axisymmetric structural physics mode.

You fix the centre (first how ? all length of axis or just in the middle in Z=0 and leaving the symmetry condition constrain in R ?) and then you apply a pressure (force over edge area =Frad/(2*pi*R*th) (where
let us say Frad=[100N], R and th are 3 constants you have defined and are using to construct your geometry
on the edge), pulling the membrane radially, right ?

You mesh (how ?, I sugest to double click the "EQUAL" sign in the lower border, beside the SNAP, when it's
off, click on the "zoom-in default" button, in this way you get unequal scales and you can study the membrane thickness, then you select left and right boundaries (along Z) and apply a manual meshing step of lets say 20 points and you mesh them and you can apply a quad mesh on the total surface), furthermore, as you have a symmetry around the neutral axis of your membrane, I would have cut the block in two by a horizontal line passing by 0,0 in draw mode (assuming your membrane is going from -th/2 to th/2 in Z) in this way you have a symmetric meshing too with a little luck

If you solve this you will see the von mises stress, but turn on the "deformed shape" in the Plot parameters, and you will see the membrane becomes thinner in the middle and expands somewhat radially, depending on the stretching force.

By the way, you can play with the material "poisson" criteria to change the thinning to stretching ratio. What happens if you fix the total length of the membrane on axis ? you will then force the membrane thickness to the original value, this is NOT physical and your stress and deformation distribution will be stricly speaking wrong ! (le diable se cache dans les détails, I believe one says in French)

So far for the first part.
Now several options are there, my preferred is to take the "solver manager" (once solved) and click "Store Solution", then select "Stored Solution" to start from there for next step, then adapt the constants (i.e. set Frad to 0 and add the constant, why not gravity, G = 1[lbf/lb] (the only way I have found in COMSOL to dump the acceleration constant in m/s^2 as a constant), the to select the material(s) and add a constant gravitational field by adding "subdomains" Load Fz = -G*(pi*R^2)*Length (note one could use "th" in stead of "Length" as its already defined in the constants. But I like to use integration constants for dimensional values, as these adapt to the model when I change the model size for any reason, therefore I often add "Options - Integration coupling variables - Boundary variables" "Length" and use "1" as integrant for the selected edges (or Area for surfaces), if you select several items it's the total integration Length (area, volume) you get out.

Now you have defined a load, you have already stored the previous deformations and stress in the "stored
solution" and you just go back to the Solver Manager and press Solve (by using the STORED SOLUTION
selections).

Now you have the sum of both.
Before you start again do not forget to redefine from where you start in the Solver manager or do a "File - Reset Model" but this will also suppress your meshing and that might not always be a good idea if you have spent a lot of time building it.

Another way is to use the Parametric solver and use the Param variable going from 0 to 2 and have a pressure load build up during Param = 0 to 1 and use *min(1,Param) in your pressure load case, and then add the gravity from 1 to 2 with a *(Param-1)*(Param>1) for the gravity load multiplier.

Another way is to save the mesh as a geomtry and then restart the model from scratch (but by adding the
sress too), or with the ALE.

I hope this gives you some ideas "how to",
now one more thing check carefully the results as they do not all add up lineraly ...

If you fix both ends its difficult to "stretch" the membrane. you can add a sliding or rolling condition by just bloking the Z displacement of one of the right edges of your membrane, but I would shoose the central point created by a central line on the "neutral axis" as then you allow the membran to change its Z shape with the minimum of distorsions due to extrnal boundary conditions.

What I have talked about above is structral analysis, exactly what you refer to with your absorption coefficient is not clear for me, so I might well have missed a point hereabove, nevertheles the example should be OK and it should give you some ideas I believe

Good luck
Ivar