Frame deflection problem - beam models

[Anonymous]

I'm have a little issue with a frame i'm analysing.

I've set up the frame, overall dim 12.5m by 4.3m. Consisting of 2 UNP 400 beams with smaller size crossemembers.

At the moment i'm only subjecting the frame to gravity and I get deflections that are just way too large. The frame is supported in Tx, Ty, T,z at all four corners.

The overall mass of the frame is about 6900 kg, so assuming 1 beam, supported at both ends with half the weight of the frame acting in the centre I'd expect a displacement of 32 mm. I'm getting 490 mm according to the simulation..

What am I missing?

Material is S355, beams are all selected from European library.

[Anonymous]

Added ACH of the model. 

Hope now more properties are transfered.

The simulation is run in Autodesk Mechanical 2016

[AstroJohnPE · Accepted solution]

Hi Pete,

This appears to be the same issue reported by Carlo Fazzini (mec) in the thread "Pre-define​d beam sections orientatio​n is wrong". Based on my limited test, the 3D visualization is wrong for shapes from the Australia, Canada, DIN, Europe, and Japan databases. The clue that the visualization is wrong is by noting the moments of inertia for axis 2 and 3 (I2 and I3) and comparing the strong axis based on the numbers with the strong axis of the visualization. I think that it is not a coincidence that the strong axis for all of the other databases is the opposite from the AISC database, but the visualization is not opposite.

I only tested one I-beam shape from each database, as indicated in the attached images. Look at "FEA Editor.png", then "Results.png", and finally "Results with visualization.png" to see the error. (FYI: The model is from the 2017 beta.) There are many, many shapes in each database, and I only tested one section from one shape. The other shapes may be okay or wrong.

In summary, set the orientations based on the numbers for the moments of inertia. Only display the 3D visualization if it agrees with the input.

Notes:

1) To display the beam orientation axes in the FEA Editor, use "View > Visibility > Object Visibility > Element Axis *".

2) To display the beam orientation axes in the Results environment, use "Results Options > View > Element Orientation > Element Axis *".

3) To show or hide the 3D visualization in the Results environment, right-click on the part (in the browser) and choose "3-D Visualization".

[Anonymous]

Ok quite a dangerous error in those databases then. Guess I should have checked more carefully but one assumes things to be correct 😄

I did check the area's but failed to look at the intertia's.

Manually put all profiles in and get "correct" displacements now.

Any chance of a "fix" for those databases?

If one where to make a design report with those profiles visualized in the wrong orientation people might start to wonder..