Surface Pressure in FEA Model

[FrederickBrannan2187]

I have a model constructed of solid midside node tetrahedrons of a container that is pressurized.  When I apply surface pressure on the interior surfaces of the model as generated by the mesher and decode it to check the model before analyzing, the pressures are applied correctly.  If then, I maually alter the mesh, the pressures are mostly lost when I decode it.  Is there a way of retaining the applied pressures after editing a portion of the mesh.  Note that each time I regernated the solid mesh before decoding to check the model. 

The reason I need to resolve this, is that some 3D solid models I receive from customers have meshing problems that I have to manually repair to get a watertight surface mesh.  If it is a pressureized container, it will not correctly apply the pressures.

Let me know if there is a way to get around this problem.

Thank You,

Fred Brannan

330-867-8134

[S.LI]

I'm not sure if you can do that.

As you see, there are always warning messages when you try to edit your mesh from CAD model.

"edit" means that there is no relation between mesh points/lines and CAD features (edges,surfaces) any more.

Decoders have to build surfaces/elements according to its rules.

In another word, all loads/constraints on CAD edges, surfaces will be lost.

[John_Holtz]

Hi Fred,

I have a correction to S.Li's reply. Surface loads and constraints should not be dropped just because you convert a CAD solid part to a hand-built part. (Edge loads are lost because hand-built models do not have the property of "edge" for the lines composing the mesh.)

You did not mention what analysis type you are using, but I may have been able to reproduce the problem in linear static stress when the element type is set to Tetrahedron. Trying setting the element type to Brick. That appears to work correctly, and a 4-node brick element is essentially the same as a tetrahedron. (No doubt one of the developers will correct me on that last statement!)

[S.LI]

To clarify my points, what I wanted to say is there is "no guarantee" on the relations between CAD features and mesh lines/points once you edited the model by drawing/adding lines there manually.

To apply a surface load, it must finally go to element faces in FEA. These element faces are marked with the same surface number.

For a CAD model, a surface is a CAD feature, and own its surface number (surface color). After meshed, its number is automatically transferred to element faces.

For a hand-build model, a surface is re-constructed from element faces with the same surface number. The surface number of an element face is decided by all lines associated with it. In this case, lines are the basic ones and surfaces and element faces are derived from lines. It becomes much more complicated to decide which surface an element face belongs to now. 

for example, if one or several lines are added to a CAD surface, which original surface number is 1. Will all element faces on this CAD surface be always sharing the same surface number? The answer is "no guarantee". It really depends on the mesh type, how lines added, lines' surface number (lines' color) etc.

In another word, essentially, there are two surface numbers here, one is from CAD and another is for FEA. FEA surface number (element face color) is used finally by simulation. Usually, they are consistent, at least code tries making them consistent. To manually edit a CAD model could result in that FEA surface number might NOT consist with the original CAD surface number any more. In these cases, users might see unexpected loads/constraints.  

Maybe what I said here is away from the original question. Just want to explain the gap between a CAD-based model and a hand-build model could be much larger than what you can see. Sorry if this confuses you more :).