VOLUMETRIC OBJECT - SOLID - NOT GETTING EXPECTED RESULTS

[Anonymous]

Hi,

I´m new to Autodesk Robot Software. I was trying to model a simple cantiliver steel plate (300x300x25 mm3) subjected only to self-weight to test model results, but I´m not getting stress values consistent to the expected theoretical values.

I have modeled the plate as a solid volumetric object and did what I believe is a balanced mesh, for the current geometry.

I have checked smoothing and no smoothing stress values and the diference is minimum.

To model the cantiliver, I have fixed all nodes in one of the faces.

I was expecting the following value for the bending stress at the top fiber (0.069 MPa), but I´m getting around double values (0.12 MPa) : 

Reactions are correct.

Can someone help me checking my model and see what I am doing wrong?

The file is in attachement.

Best Regards

Tiago Nobre

[Pawel.Pulak · Accepted solution]

Values are not coherent with expected ones because the reference ones were obtained using standard Euler-Bernoulli beam theory while your test model is not a beam element but a solid and moreover its geometry, support conditions and loads are far away from the assumptions of Euler-Bernoulli beam theory:
1/ cantilever with 0.025x0.3m section and 0.3m length - it's not a slender beam
2/ no constraints to keep the cross section perpendicular to the bending line and preventing deplanation
3/ load (selfweight) applied to the volume - so distributed both along the length and section of the cantilever
4/ supports defined fixing all 3 components of translation so preventing displacement in X and Z direction resulting from stresses in Y direction (Hooke's law in 3D)

I have modified your file copying the solid 2 times and modifying its loads and support conditions to get closer to the beam model.
See the screen capture below:
a/the solid on the right side is your original one - selfweight load results in the moment of 0.026 kNm at the supports - can be checked in the table of reactions of your original file
b/ the solid in the centre is modified in such way that the full rigid diaphragm is defined at the end of the cantilever and the moment of 0.026 kNm is applied there - this way the cross section is perpendicular to the bending line, no deplanation and the load is not distributed in all volume but pure bending is obtained.
c/ the solid on the left side is additionally modified in such way that both the supports and the diaphragm at the end of the cantilever are defined in such way that they do not block movement in X and Z directions

As it can be seen in your original model the maximum stress is 0.12 MPa, in the central model it is 0.085 MPa so it is closer to the reference value and in the model on the left side it is 0.069 MPa so it is coherent with the reference value.

I have attached such file.

Please note that solid elements in Robot have no rotation degrees of freedom.

---------------------------------------------
If this post answers your question please click the "Accept as Solution" button. It will help everyone to find answer more quickly!

Best regards,

[Anonymous]

Hi,

Thank You for your help.

I realized short time after I posted the message, that  the theory from my analitical calculations and my model didn't match. 

In fact, what I'm trying to achieve is to create a padeye/lifting lug type model (the shown cantiliver was just a basic example to pratice Robot capabilities, before I move to a more accurate model of the padeye). So, although, your explanation did help a lot, I don't think the beam theory will be the best way to model the padeye. According with the literature, curved beam or plate theory are more appropriate to analiticaly estimate the stresses. 

For a padeye type model (steel cantiliver plate - 127x163x25 - see picture), what do you think is the best option in ROBOT to model this element - Solid or plate? Loads will be along the 3 main axis and I will model the padeye with the connecting beam for better boundary conditions.  

 

I will also represent the external loads on the padeye as bearing loads aplied on the hole. Do you have any suggestions on how to model this with ROBOT?

Best regards

Tiago Nobre