Simply supported thin rectangular plate boundary condition

[Anonymous]

Hi everyone, 

I have done various combination in boundary condition however there is a "give and take" in error percentage. It is a simply supported for all edges. But I constraint Tx, Ty,Rx and Ry at one edge, Tz on other two edges and Ty, Tz and Ry at another edge. This gives me a good error percentage except for first mode. 

For my other tried, I constraint the Tx, Ty, Tz and Rx at one edge, Ty and Tz at another edge, Tx, Tz and Ry at another edge and lastly Tx, Tz for the last edge. This gives me a reasonable error percentage except for the 5th mode. 

Any idea what constraint boundary is the most suitable? 

My theoretical freq for each modes are: 

Mode                  Freq (Hz)

1                         1092.513

2                         2100.986

3                         3361.578

4                         3781.775

5                         4370.051

Thanks for the kind help.

[AstroJohnPE · Accepted solution]

Hi,

Technically, you need to look at what assumptions were made by the "theory" when the equations were derived. It's possible that "simply supported" to one author has a different meaning than to another. But in general, simply supported means that the edge (node) cannot move "up-and-down" but is free to move "left-and-right" and rotate. You can translate these descriptions to XYZ based on the orientation of your model (which I believe we do not know) to restrain the translation in only one direction.

Since you are modeling a thin plate, it would be best to use plate elements and create a mesh that will look like a piece of graph paper. (That is, the mesh has area but no thickness).

If you are using a solid and creating a brick mesh (the thickness of the "plate" is represented by the mesh), then you need to devise a way to put the constraints on the neutral axis. In other words, the constraints cannot be around the perimeter on the "top face" or on the "bottom" face. I can almost guarantee 100% that they theory is based on the plate being restrained at the neutral axis (at the midplane of the thickness). You either need to split the 4 faces of the solid in CAD, or create an assembly of two "plates", each half the thickness of the real plate. That would put a layer of nodes at the neutral axis.

[Anonymous]

Kirchoff plate theory/classical plate theory. Assumptions are midplane remains neutral axis after bending, rotary inertia neglected.

But now i would like to try assembly of two plates in the simulation mechanical. The CAD were drawn in inventor. I divided the thickness into 1/2 which is 25mm. L = 600mm and B = 400mm. I constraint Tz on the surface of the midplane. However how can i bring in the 2nd part CAD model of the rectangular plate? I right clicked "parts" and clicked new part. However I cant seem to export the 2nd part of the plate into the simulation. Sorry and thanks for your advices.

[Anonymous]

Kirchoff plate theory/classical plate theory. Assumptions are midplane remains neutral axis after bending, rotary inertia neglected.

But now i would like to try assembly of two plates in the simulation mechanical. The CAD were drawn in inventor. I divided the thickness into 1/2 which is 25mm. L = 600mm and B = 400mm. I constraint Tz on the surface of the midplane. However how can i bring in the 2nd part CAD model of the rectangular plate? I right clicked "parts" and clicked new part. However I cant seem to export the 2nd part of the plate into the simulation. Sorry and thanks for your advices.

[AstroJohnPE · Accepted solution]

Hi,

You need to create an assembly in Inventor that consists of two parts. Each part is half of the real plate thickness. You can even use the same Inventor part and place it in the assembly two times. Then you will use the "Mate" or "Constraint" command in Inventor (I don't remember what it's called off the top of my head) to mate the midplane surface, the end face, and the side face so that the two half plates line-up to make one plate.

Then you will send the assembly to Simulation Mechanical, have two parts in Sim Mechanical properly aligned, etc.

If I understood your previous description, it sounded like you send one half-plate from Inventor to Sim Mechanical; this created part #1. Then you created a new (empty) part #2 in Sim Mechanical, and were expecting to merge another Inventor part for the second half of the thickness. Although this could be done (you use the "File > Merge" command in Sim Mechanical), there is no effective way to move the parts in Sim Mechanical in order to get them to line-up. Aligning parts is best done in Inventor assemblies.