realistic selfweight deflection?

davefo

please can anyone advise how to get the attached file to calculate realistic deflection.

According to analysis it sags 340mm due to selfweight alone which i find hard to believe.

Dave

VMH

Dave, I did a quick hand calculation using the dimension from your model and came up with 13.72" which was close to 340mm.  See attachment.

Victor

Keep in mind that since it's so slender, there will be stress stiffening effects here, like a catenary. So a linear calculation won't be accurate.

Instead:

Change the analysis type to Nonlinear Static 3D

Change the solver to CCX

Unsuppress the rotation constraints. Just one is enough.

Solve

Now it shows only 19 mm displacement.

VMH

The calculation I did was just checking the analysis results using the same assumptions used the model: linear static analysis. For actual displacement, nonlinear analysis as mentioned by Victor is what I do for this type problem.

Andrea

If you release the X displacement of one end node, in a nonlinear static analysis , you will obtain the same results of static analysis. It's typical "large deflection" problem and so is correct to perform nonlinear analysis. In ccx input deck is suitable adding NLGEOM= YES as a *STEP parameter

*STEP,NLGEOM=YES
*STATIC

For faster solution add DIRECT to *STATIC. Mecway does it in a faster way

davefo

Thanks for your responses

I'm not familiar enough with ccx yet. I'm trying to read up on it now.
can you advise why doesn't it work as non linear static analysis in mecway instead of ccx?

The reality of this beam is that it is a model of a single x flat brace in a roof and the fabricator has expressed concern that his analysis says it would deflect over 330mm. Obvioulsy i was surprised and couldn't believe this to be correct especially when the ends are held in place by bolt fixings to relatively stiff members so I couldn't see how this much deflect could possibly occur. This deflection would require approx 70mm elongation of the member. based on this elongation the resulting axial force in this plate would be over 2e6 N which is obviously wrong.

19mm deflection is more realistic, there will be some additional stiffness at the end connections so the real answer will be probably less.

VMH

Mecway currently doesn't support beam and shell elements for nonlinear static analysis with its internal solver, but you could use solid elements.  They are supported.

See attachments.  

For linear static analysis, the max. deflection at midspan found to be about 13.75" with the ends simply supported and about 2.72" with the ends fixed.

For nonlinear static analysis, the max. deflection at midspan found to be about 4.91" with the ends simply supported and about 0.66" with the ends fixed.

Andrea

I think that your model for simply supported beam is not correct. In fact end faces must be free to rotate. So Y displacement must be fixed only for bottom nodes and not for all nodes lie on the face. Try to fix Y displacement only for bottom nodes and deflection will be similar to the linear static solution

VMH

Thanks for the notes.