I've used beam elements (point to surface) in FEM Mode for export to Ansys.

They seem to work well enough, but you get high stresses at the interface.

-Dan

Dan thanks again for responding,

Did you ever use point to surface beam in ProM?  Ill try that later anyways...

Thanks

Tobalcane
"If you avoid failure, you also avoid success."

I have used beams and springs to simulate fasteners. I would second the fact that you get unrealisticly high stress locally for the situation you are recreating; but if for load transfer only ,that is the ticket.

Mechlad,
Thanks again for responding.  How did you use beams as fasteners?  I don't work with beams that much.  Can you give me a quick method to use when I want to used them as fasteners.

Tobalcane
"If you avoid failure, you also avoid success."

Basically I used the "wagon wheel aproach". A node in the middle of youe hole, with beams connected from it to the hole's edge, do this on both holes, connect the two beams "wheels" with another beam. There are a couple other details to this,(releases) which im sure you will figure out. This method is not without fault though, which im sure you will figure out.
A great book on FEA is "Building better products with Finite element analysis" by Adams and Askenazi. it covers the subject.

I use beams with rigid connections to attach the beam end node to circular edge of the plate.

Principal - http://www.OnlineFEASolver.com
General FEA Consulting Services

Doesn't connecting a rigid rod to a non rigid plate give you a singularity? Yes I believe it does, and such a connection if it does is an example of a point load or constraint and is illegal within the principle of virtual work, which is the basis of the finite element method. Unless of course the connection really isn't directly between a rigid rod and the non rigid plate (say if there was a soft interface between them). You can choose to use it of course, despite that, but be prepared for "GIGO".

good shootin prost, but what is your suggested method?

Using the rigid connection to connect the end of a beam to the circular edge of a bolt hole does NOT give any singularity. You have to pick the entire circular edge of the bolt hole, i.e full circumfrance. It locks all 6 dof of the beam with the circular edge, so no rigid body mode is present.

Principal - http://www.OnlineFEASolver.com
General FEA Consulting Services

It wasn't a shot, it was a question of using what look to me to be incompatible elements. Before I personally would use beams with 2D quads or plate elements, the first question I'd ask myself what is the goal of my analysis? and next, if I need stresses near the hole, then I'd ask the software vendor is what sort of manipulations are being used to make beams and quads compatible at the interface between those elements? A lot of this is proprietary of course, but it would take only a test case or two to verify that the elements are compatible or not at the interfaces.

As for my suggestion for using, try using StressCheck, by ESRD, easy to connect 3 plates with any number of fasteners. And no I don't work for ESRD. The right tool for the job, that's a good rule to follow, don't you think?

It seems odd to characterize the beams as 6 DOF, as a 3D brick element would be characterized. The two element types, the beam and the brick, have two different formulations, two different sets of governing equations. I can imagine there are a few tricks that can be used to make these two elements compatible, I was just curious  as to the tricks, and if anybody cared.

Pro/Mechanica's beam elements do have 6 DOF's.  This is due to the shape functions that are used to model both translations and rotations that occur throughout the length of the beam.  

Solid elements in mechanica only have 3 DOFs (translation only).  Rotations throughout the domain of the solid element are not modeled within ProMechanica.  Tranlations are the only displacements that are modeled throughout the domain of the element via interpolation using the polynomial elemental shape functions (i.e. order of 1 thru 9).

True the solid element in mechanica and the beam element have two different formulations throughout the domain of the elements themselves, however the element connectivity is handled at the common node.  A beam element cannot be connect to a solid mid way along the lenght of the beam element.  If it appears that this is occurring in your mechanica model it is because a new node has been added along the length of the beam, thus dividing the original beam element into two new beam elements.  Given that the displacements are calculated at the nodes, the difference in elemental shape functions is irrelevant.  The beam and solid elements will form their couple at the connecting nodes.

However, the connection between shells and solids in mechanica is totaly different.  At the interface between a shell and a solid element, a link element is created.  This link element ties the edge of the shell element (which has 6 dof's 3 trans and 3 rot) to the side face of the solid element.  In this case the link element is required to couple the displacement of the two different elements at along the entire length of their respective interface.  Link elements show up in mechanica as dotted pink lines.


The "waggon wheel" method is classic method that works fine.  One alternative is to model the head of the fastener as a shell with a diameter (or shape) of the fastner head, then connect the center of the shells using beam elements.  This, in essence, is what mechanica is doing in its "fastener feature".  Also, as mentioned above, simple beams from the center of one hole to another with rigid links between the ends of the beams and the edge of their respective hole works great too.

Any of these idealizations is going to produce a stress field result that will not represent the real world conditions, because...they are idealizations.  In addition, some could create singularities.  However, if the stress, strain, displacment values of interest are far enough away such that they are not affected by any singularity then the results from any of the above methods should be similar.

Good luck.

Steve