Line Elements

[Anonymous]

Hi,

So I want to model a beam in Nastran in Cad with simple supports. I have tried modelling this as a line element, by first sketching a line, apply a line element idealisation, and then adding my loads and constraints. It comes up with huge stresses which can no way be correct. Can anyone do a quick video maybe of how to model this? 

I can always just create a simple extrusion, and do it that way, but would like to be able to mimic the capabilities of Strand7.

Thanks,

Henderson

[shigeaki.k]

Hello @Anonymous,

are you able to attach the model?

And here are some thoughts that I have. Others may also add to it.

It looks like you are using distibuted load. Are the input values correct.

What is the cross-sectional shape of the beam? It is non-symmetrical, is the orientation correct?

I also noticed that you have 3 constrints. If you are modelling a continous part, is the constraint in the middle of the part necessary? Are the boundary conditions applied correct?

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Hi,

It is a distributed load. I have checked all values and they should be all correct.

[shigeaki.k]

Hello @Anonymous,

was the correct model attached? You have a load applied in he z-direction, and you seems to have contraints stopping motion in that direction, as well in-adequate constraints, hence the analysis will not run.

Could you please check your constraints again?

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Sorry, this is the one. I basically want it to be modelled as a simply supported beam. I am getting 4000 MPa which doesnt seem correct

[John_Holtz]

Hi @Anonymous

Your stresses are wrong because your displacements are wrong.

Your displacements are wrong because of one or all of these reasons:

1. Your model is not sufficiently restrained, so you are getting infinite rigid body motion. It is free to rotate about the Y axis, so you should change one of the constraints to include Ry. It is also free to rotate about the Z axis, so you either need to add an Rz constraint to one of the constraints, or change the constraint at the bend from Tz to TxTz.
2. I suspect the orientation of the I beam is wrong. Right-click on "Elements" and choose "Display Cross Section". If the orientation is wrong, you can change it by editing the Idealization for the beams, check "Associated Geometry" and choose the sketch segments, and then change the Rotation Angle.

With both of those changes made, the von Mises stress goes to 695 MPa (100835 psi). This is still high but probably correct given the loads and constraints applied to the model.