MPC's 1

[airmail]

Hello all!

Well, my question is very easy for people who visit this forum (I am new in FEA).

Which is the difference between the types of MPC's (RBE2, RBE3, Explicit...) that I can model in PATRAN? I've been searching information and I've found the next:

"RBE2 is a rigid element that references a group of nodes to an independent node and RBE3 is a rigid element that references a dependent node to a group of independent nodes" Can somebody explain me this (an example, please) ?

THANK YOU ALL IN ADVANCE.

 

[fkmeyers]

All rigid elements (RBEi) are essentially MPC equations. The purpose of RBEi elements in Nastran is to make things easier. RBE2 is a general rigid element that connects one master node (independent) to many slave nodes (dependent). RBE2 is a rigid element and would be used to force a rigid connection. RBE3 is an interpolation element. This is used mainly to distribute loads from one point (slave node or dependent or reference node) to many other points (master nodes or independent or averaging nodes). It can also be used to distribute mass at a point to many points. Example would be to model the mass distribution from an airbag onto a steering wheel for a normal modes analysis. RBE3 elements are a bit tricker to setup. They have other uses as well. I would check out either the NEiNastran website or MSC.Nastran website knowledge base for more information.

 

[gwolf]

RBE* elements are intrinsically evil. I can't count the number of cock-ups which I have seen as a result of their use, I include myself. Use extreme caution.

The main one is using RBE2's indavertently in a loop which becomes infinitely stiff. The bicyle wheel of RBE2's is also a common one to feed load into a hole which then becomes infinitely stiff and won't ovalise. The user then switches to RBE3's and a whole new set of problems emerge.

Read up well on these creatures and try lots of small test models where you know what the answer should be.

 

[SWComposites]

I agree with gwolf - there are many ways to screw-up a model with rigid elements, and often the problems are not obvious. You should obtain the NASTRAN manuals and read everything in them about the various rigid elements, then look thru the Example Problems manual for sample usage (I can't remember if there are any example problems which include rigid elements, but it won't take long to check). Then take gwolf's advice and run a bunch of very small test models so that you are sure you fully understand how they work. There are lots of subtle effects that are hard to explain in words and its best just to try them out for yourself. ALWAYS look at the forces generated by the rigid elements (and MPC's and SPC's) in a model and be sure that you understand and agree with the results (if you don't understand the internal forces generated by the rigid elements than either there is something wrong with the model or you haven't run enough test cases to fully understand the effects of the elements).

 

[johnhors]

I recently reviewed an FE model of a pin that was held at two bearing positions and had an offset lug at one end through which loading had been applied. The loading at the lug had been applied via an RBE2 element and spring gap elements had been used to connect the pin to RBE2 elements at the bearing positions which were fixed to earth.

In over 25 years of FE analysis this was probably the worst example I have ever seen of inappropriate use of rigid body elements! As neither the lug or pin was free to ovalise and results were pure rubbish.

Since this was nothing more than 3 point loading the correct approach would have been to apply the lug load as a variable pressure distribution over the lug bore using the Gencoz empirical formulation. Similarly the same pressure formulation should have been used to apply loading at the bearing positions to a achieve a fully load balanced model. Minimal supports could have then been used to earth the model. And not a single rigid body element in sight!

 

[gwolf]

As a slight aside, when I model shafts in holes these days I frequently model the shaft, hole, and contact using a coarse ABAQUS mesh. Extravagant perhaps but it takes very little time to set up in PATRAN and the increase in run time is paid back by the simplicity of post-processing.