How to create Elemental vector-stress (using PRG codes) from GPForce output (global CSy)

[Oliver82]

I'm modelling two surfaces with one coincident node, which represent the rivet modelling. In order to calculate the bearing stress ,I get GPF output at local coordinate system from those coincident nodes. The stress is calculate in excel: Bearing stress = GPF/ (property element.
My question is: is there any way using PRG codes to performed this bearing stress creating a elemental vector of bearing stress and read it at material direction?

 

[APav]

Hello,

A few points:
1) In some cases what you have in mind might not work: keep in mind the fact that for body loads like gravity, GPForces come with an OLOAD resultant which isn't detailed, therefore you can't deduce "what comes from one side or the other", you would need an internal OLOAD calculator for that. IF your loads are not body loads OK

2) In essence you're looking for a "sensor", i.e. something to give you the force screw {F,M} at a point. GPForces is the most complicated way to do this and they should be used with care. FEMAP handles them extremely well through freebodies, but then accessing this through PRG codes seems complicated (I don't use PRG myself, but my first answer to your post is "No, can't be done"). I would recommend a different sensor:
- either a null length RBE2: instead of 2 coincident nodes merged, add a 0 length RBE2 between them and ask for MPCForces at one node. This has several advantages: output is easily and directly useable (6 values), and there is no possile error du to body loads.
- or a very rigid CBUSH, which is more or less equivalent. Though bush elements you can also pilot the various dof stiffenesses.

3) Just in case: if you're modelling 2 surfaces with shell elements, then your 3rd rotation dof only exists through the PARAM K6ROT. In other words the torsion in your rivet will be aritrarily calculated from the value of this parameter, because you're using only 2 nodes. If this is indeed your situation a solution is to use local RBE3 interpolation elements to reach out to neighbour nodes and force the 6th dof of your rivet node.

4) As for automating your process, MPCForce or CBUSH Force output are easily accessible. I don't know which "element property" you want to retrieve, no idea if they are accessible through PRG. And as for orienting in material direction, you would need to transform the nodal vector output to that coordinate system, should be feasable in PRG.

But the answer I often give: all this would be MUCH simpler through API programming...

All the best,

A.Pavageau