How to apply nodal equivalent vertically distributed load for shell element

[hustzjy312]

Dear all,

I am working on a cylindrical panel subjected to a uniformly vertically distributed load. How can I get the nodal equivalent load in FEAP for shell elements? In this case, I think the surface loading and pressure loading option in FEAP do not work. Does FEAP has particular function to deal with this type of loading?

Thanks.

Yang

[Prof. R.L. Taylor]

First, which shell are you useing?  Small displacement or finite displacement?  If small displacement which one - there are two in the shell directory (shl3ds and shl3di).

You are probably correct that the shell will not compute the loads for uniform values.  However, it should be possible to modify the code to do what you want -- uniform load is a special case since it depends on what projection you are going to make the load uniform, this is the main reason we do not provide it as a default.

Probably the simplest way to add it is to 'overlay elements' -- each element has an identifier number that matches it to the material set.  The default is the material number, however, you can have the same element associated to two or more materials using

MATE ma  (where 'ma' is some material number you wish to overlay)
   SHELl  ...
      data for shell



MATE 2
   USER  1    ma  (where 'ma' is the same as the shell element material number)


Then each element that has the 'set number = ma' will call both the shell element and the 'user 1' element (i.e.,. elmt01).

You can code the elmt01 to compute your loads using the 4-node shape functions of the the shell element.

[hustzjy312]

Dear Prof. Taylor,

Thanks very much for your kindly reply. In order to make my problem more clear, a illustrative picture of my cylindrical panel is attached to this reply. I want to apply uniformly distributed load in z direction.

Currently, I am using a finite deformation shell element (shl3df). I noticed that it is a 4-node bilinear element. Could you please provide me a reference book on computing nodal equivalent load for shell element?

In addition, I also want to use a 3-d large-deformation solid element to model the cylindrical panel subjected to uniformly distributed load in z direction. For the large-deformation solid element, does FEAP have the option to apply uniformly distributed load?

Regards,

Yang

[Prof. R.L. Taylor]

I believer the load should be just:

int_A q_z * e_z * n * dA where q_z is load intensity, e_z the unit vector (0,0,1), n the normal to the shell and dA the area.  In isoparametric coordinates n*dA is just dx/dxi  x dx/deta where xi and eta are the parent coordinates and x is the coordinates in cartesian form x = x_A N_A(xi,eta)  the N_A are bilinear.   The loading can be "dead" where x is just the reference coordinates at time 0 or it can be current where x = X + u -- in the later case there will be a tangent also.

Look in any FEA book where normal loading is computed (e.g., see Zienkiewicz, Taylor and Zhu).

[hustzjy312]

Hi Prof. Taylor,

Thanks for your previous help.

By the way, could you please provide me a related benchmark problem so that I can verify whether my code works correctly or not?

Yang