How to get moment and shear from Solid stresses output

[monopoly]

Hi all,

I model my concrete structure with solid elements in STAAD. How can i use stresses output results (corner stresses & centre stresses of element) to get bending moment, shear and Axial forces. From there I can design reinforcement.

Any references and examples will be very appreciated.

 

[oneintheeye]

Interested in this one as i've never got an answer either other than using complex maths. I tend to leave the mesh element in the top which allows you to get moments out. Shears i've never been able to nail down. normally i will do a quick conservative hand check on a small segment of slab or convert my bending moment into an equivelent udl and work out shear locally to that.

 

[EdR]

Plot the stresses (normal and shear) across the surface you are interested in and then integrate the plot to get the total forces (axial and shear) on the section. Then do the same thing for the moments (force * distance from the bending axis)

Ed.R.

 

[Denial]

Some software packages will perform EdR's integration for you, for exactly the purpose you require. I am a user of Strand7, and it has this capability. Maybe STAAD has it, hidden away somewhere?

However you should always bear in mind that by using the single values that come from the integrations you are "throwing away" a lot of information, perhaps the very information whose absence in simpler approaches caused you to resort to solid elements in the first place.

 

[monopoly]

Hi EdR,

could you please provide more detail ? if you have any simple examples, it would be great

Thank you guys

 

[EdR]

monopoly:

Not sure I understand what you want....The forces acting on an area are simply the stress*area...If you plot the stresses normal (for the axial) and parallel (for the shear) to the section you are interested in you can then use numerical integration (via Simpsons rule, trapezoidal rule, or other rules) to determine the total forces...

If your concern is that you do not have the exact stresses at a particular node to make the plot just take the stresses from all adjacant locations (probably integration points) and perform a simple average of the values (while this may be off a bit when adjacent elements are not the same size it will be close enough)

As for the bending moments they are simply a combination of axial and bending stress....After you have the total stresses plotted normal to the surface you should be able to locate the neutral axis, remove the effects of the axial stress (not strictly necessary) and determine the bending stresses only....The integration of the bending stresses across the section is then the value of bending moment (sigbending = M y/I = sigi * yi)....

If I didn't understand what you wanted let me know and I'lll try again...

Ed.R.

 

[TheStructuralMule]

In a lot of FE programs that I have used, I find that I can get all the information that I need to determine moments, internal forces including shear as well as support/ connection information and edge forces/stresses by asking the program to output the FE element results in the Von Mises stresses format.

B. Chepren

 

[rb1957]

i would have thought that von Mises by combining direct stress and shear stress would have confused the situation. i'd use the direct stresses at each node and integrate as EdR posts.

 

[EdR]

Mule:

I think both rb1957 and I are interested in how you get direct stresses and forces (in specific directions) from Von Mises stress information. Please elaborate.....

Ed.R.

 

[Bobfromoh]

To All,

Attached (hopefully) is a paper I put together for evaluating the membrane and bending stresses from solid or axisymetric FEA elements. This is my opinion as to how to determine the needed stresses from the results of an FEA analysis.

It may not answer all your questions but it might provide some insight? The results of my analysis do match exactly with the published documents but the difference could be due to the approximation method used.

I took the liberty of using absolute values to more easily compare my results against the results from the source document. Review and comment if you want.

 

[EdR]

BOBFROMOH:

Basically what you are doing is correct but from a casual scan it looks like you have assumed that the neutral axis for bending is at the center of the section....This is not always true and the method should be modified to account for the neutral axis not in the middle....

Ed.R.

 

[Bobfromoh]

Ed.R

OK So show me how to do that. What should the equation look like?

 

[monopoly]

Thank you you guys for input. I'm going to do as EdR said and Bobfromoh's ref.
More disscusion please

 

[oneintheeye]

the fea software i use lets me leave my mesh in after making the element 3D. I then get moments, etc/ from this. Is there anything wrong with this approach that people may consider? Basically i'll have a 3d element with a mesh on top. The 3d element will spread the load more effectively and the moment can then be outputted. This gives less onerous results than a plate element. Any comments on approach?

 

[rb1957]

to answer bobfromoh, the FEA gives you stress at a point. allocate area to the point, say 1/2 the adjacent elements, maybe areas of endload elements; so that now you've got a bunch of forces at points. 1st moment of these gives you the NA, and from this you get the moment. the nett endload on the section is the simple sum of the forces.

i think EdR's point was that you knew the section you were summing over, and imbedded this into your equations, nothing wrong with that.

 

[rb1957]

one thing i forgot to mention is that the FE stresses need to be normal to the section. take your example of pipes with a 45deg joint. to get the force and moment normal to the joint, the FE stresses, which are axial in the tubes, need to be converted to be out-of-plane and in-plane to the section of interest. this is "just" a bit of vector math