FEA of Steel rolled shape

[anilkvyas]

If I take a wide flange beam and apply a point load at the mid point of the simply supported beam, I can calculate bending moment and shear at the load location and design the beam. If I take the same beam and model it as Finite Elemente as top and bottom flanges as beams and the web as a shell element and apply the same point load at the same location, should I see the same bending moment and shear, if not how do I design the beam using FEM?

 

[jetmaker]

anilkvyas,

In short, the answer would be yes. The bending moment and shear are independant of the beam geometry. However, deflection and slopes would be different, as would be the stresses, as all of these are functions of geometry.

jetmaker

 

[Drej]

If shear force and bending moment are all you need to calculate, and the beam has a relatively simple cross section, why model the beam at all when a simple and cost-effective hand calculation will suffice? I'm also not clear why you would need to use beam elements for the flanges, when a single row of beam elements or an assemblage of shells or bricks would suffice for the entire beam? Depending on what you require for the analysis (in terms of results etc.), you would need to then consider how to model the beam.

-- drej --

 

[anilkvyas]

Drej/Jetmaker,

Thank you for quick response. Actually I am working on a very large bridge model which I created in STAAD Pro. The bridge has three trapezoidal steel boxes with two top flanges, two webs and a common bottom flange. The bridge is five spans 60m, 80m, 90m, 80m, and 60m. I ran this model using two dimentional analysis and have bending moments and shear for dead and live loads. Now I need to use wind load, seismic load etc. and I created a three D model using top flanges as beam elements and the webs and the bottom flange as shell elements. After running the model I got big difference in the deflection in 2D and 3D models. Why there is a difference in deflection I can not figure out. Also how do I use the stresses in the beam and shall elements to design against allowable stresses given in AASHTO?

Your response will be greatly appreciated.

Thank You

 

[jetmaker]

anilkvyas,

Unfortunately, I know very little about bridge design, and AASHTO, so the bridge description does not make much sense to me.

However, the question you ask is partly an FEA one, so I'll try and answer that one. The main difference will be in the way you idealized the structure. Check to make sure that your modelled Moment of Inertia and Area are close to those of your 2D beams. Any difference here will clearly be seen in your results. Secondly, proper selection of elements is key. For example, using rod elements in lieu of beams, or membrane plates or bending plates. Finally, you now have more nodes to constrain, and must be careful that the loading applied is representative of that applied to the 2D model.

Hope this helps.
jetmaker

 

[bvi]

I would think the way you modelled this, there would be much more deflection than reality. The reason is the beam and plate sections probably do not function in the model as a composite section, but as individual beams. This would greatly reduce the effective moment of intertia. You have to be very careful in mixing up elements like this. Before doing something like this in a large model, start with a simple beam model to make sure it works.

 

[RiBeneke]

I have not seen the AASHTO code, but I suggest that you cannot just check your calculated stresses against simple allowable stresses. The governing stress conditions in a bridge structure like this include things like out-of-plane buckling of the plate elements, crippling stresses at load transfer points, fatigue stresses at stress reversals, etc. Presumably the plate elements making up the bridge section will be stiffened, and the design of these stiffeners affects the safe stress levels.

 

[Dinosaur]

anikvyas,

This is essentially the great subject of modeling composite steel girder bridges, along with how you apply the live load. First off, you should get similar results if you computed the constituent moments of inertia properly. Some differences come from the following . . .
Do you have the composite slab in the correct position relative to the top flange? The additional eccentricity of the slab thickness and bolster change the stresses dramatically. Do you realize you will see some deflection due to "shear" deformation in the second model that you didn't get in the first model? This should be small, but will contribute to differences. When back checking the moments, did you add the moment in the flanges, the web, and the slab? If you only added the moments in the steel, you will have too little moment. In your second model, there will be a correction for the inclination (superelevation) of the box which may not have been captured in your hand calcs. Also as mentioned in a previous post, check your restrained nodes to make sure you have them in the right place and acting in the correct global direction.

If you check some of these things, I think you will get better agreement between your two models.

Good Luck - Dinosaur