FEA corelation

[ananthaces]

Hello, I am analysing a sandwich panel as a plate and trying to corelate the displacment and stress with theoretical solution. I ran the analysis and the displacments conforms well with the theoretical solution but not the stresses. I don't understand why it works this way. i am comparing the vonmises stress. Any suggestions? Thanks.

 

[feadude]

if you are using linear tet elements this could happen. Linear tets give correct answers (sometimes)for displacement but not for stresses.To get the correct answer for stresses one should use parabolic tet elements.

 

[ananthaces]

I am using 2-d quad elements..

 

[jxc]

Try using principle stresses or shear stress results in your correalation. I have found these to be more reliable source.

Good Luck...

 

[ananthaces]

hmm..so does it mean that principal stress shld be equal to the normal stress? Thanks

 

[ananthaces]

i juss refined the mesh and the deflection still is the same but the shear stress is increasing by a great amount.Why is that? the refinement is not to a great deal. Would it really affect the stresses so much? Thanks

 

[SWComposites]

1) You are probably modelling a singularity condition, in which case the stresses will continue to increase without convergence as the mesh is refined.
2) FEA is an approximate, numerical solution to a continuum mechanics problem; it will not give exact answers except for simple cases like statically determinate problems with boundary conditons and loadings that do not produce numerical singularities.
3) Please describe in detail your model and theoretical analysis.

 

[ananthaces]

I am analysing a 2*0.5 inch honeycomb panel for 2 cases. One is simply supported beam and the second is simply supported plate.I ran both the cases and i want to compare these results with theory:
1.) deflection
2.) Facing stress
3.)Core shear stress
What I observed was the deflection matches exactly with the theory.But the problem is with stresses. I checked the ply1 vonmises stress for the facing stress. but the error is 14%..could i compare the facing stress with the principal stress? it does compare well though.
Now with the core shear stress as i refine the mesh the shear stress is goin on increasing.
I am using Pcomp to analyse the sandwich panel.
So, swcomposites..how do i rectify the singularity condition..cause my boundary condition seems to be allright? Thanks for your suggestions..

 

[SWComposites]

1) What are the 2 inch and 0.5 inch dimensions? width? length? thickness? What are the core and facesheet thicknesses and materials? What loads are being applied? (you only describe the boundary condition).
2) What theoretical solutions are you comparing to? How do you know that they are correct?
3) Where are you comparing stresses? in the center? at an edge? at a corner? You have to compare streses from the modl at the same location as the hand solution. Start be comparing at the center of the plate.
4) I doubt the hand solultion predicts von mises stresses, so forget using them. Also, forget using principal stresses as they can be confusing and misleading for comparisons. Compare x and y direction stresses in the plate.
5) For which loading case do you get the "error"?
6) Simply supported plates loaded out-of-plane will typically have a stress singularity in the corners. Thisis due to the fact that the corners tend to deflect upwards under a downward pressure load.
7) Turn off ALL contour plot averaging. Make comparisons only using un-averaged element stresses (not nodal stresses). Nodal stresses are typically not accurate since they are extrapolated from the element streses calculated at integration points. Contour plot averaging of nodal stresses is even worse and often produces results that look good but are rubbish.

 

[ananthaces]

sorry for nt being specific..the width is 0.5 m and the span is 2m. The face material and the core are both aluminum.In the case of a beam a centre load of 1500 N is applied and in the case of plate a pressure load of 0.139 lbs/in^2 is applied. Please note that both the cases are in different unit systems. The theoretical solution is from Hexweb website. They have some solved problems there.So from FEA i am comparing the maximum values with the theory.
I am not getting any error. The analysis runs without any problem.I checked the normal stresses in the plies i.e the facing sheets but it ds nt ocmpare well wth theory whereas principal stress does.
How do i turn off the contour plot avergaing? Thanks for your patience.would u like to take a look at the problem?

 

[SWComposites]

To turn off contour averaging in FEMAP you go to the Contour Options dialog, select element results, select NoAveraging. In other s/w there probebly is something similar.

The Hexcel beam example is analyzed using a beam formula; you are modeling it as a plate, therefore you will not get the same results.

The Hexcel plate example is analyzed using an old Mil-Handbook-23 approximate plate soluton using (I think) a truncated series solultion. It does not surprise me that you are getting different results in your FEM. The maximum stresses in the facesheet should be at the center of the plate, so compare your FEM results at that location (do not just look at the maximum values anywhere on the plate).

 

[airmail]

Ananthaces:

Have you checked that your constrainted points do not take load? Look at your "constraint forces", because it seems that part of the load of your model is being withstood by these point, which is wrong.

Good luck!