Composite section FAQ

Why am I getting unexpected response for composite section? (Impact of Support Conditions)

Extended Question: I have models 1 and 2 (please see the description below), but I am getting unexpected deflections for model 1. The deflection form model 1 is smaller than expected.

Model 1:

• Steel girder modeled by frames and concrete deck by shell elements.
• U1, U2 and U3 restraints assigned at both ends of the girder.

Model 2:

• Just one frame element with composite section created in the section designer.

Answer: The unexpected results for the model with shells over steel girders may be caused by the boundary condition, since you are providing longitudinal restraint at both ends of the girder. For this particular model, the longitudinal restraint is not located at the centroid of the cross-section and it results in a longitudinal force acting on an arm about the neutral axis of the composite section. This introduces additional moment which impacts the response. While this is kinematically correct behavior, it does not correspond to the other model (with section designer section) in which the composite beam is essentially supported at its centroid.

The axial force in the girder is the net effect of stresses acting on the girder. The applied moment is resisted by the entire composite section, with tension stresses below the neutral axis of the cross-section. Since most (if not all) of the girder is located below the neutral axis of the composite section, this results in axial force (tension) in the girder.

How can I model partially composite sections?

Extended Question: I have a 85% composite design with concrete over steel girder. If in the SAP2000 model I put 0.85 for the membrane stiffness modifiers in the shell element, will it simulate the 85% composite action?

Answer: The total stiffness of the composite section (let's consider concrete deck on a steel girder) comes from the following three sources:

1. Stiffness of the girder about its own center of gravity.
2. Stiffness of the deck about its own center of gravity.
3. Additional contribution of the deck and the girder about the center of gravity of the entire section.

Changing the deck membrane modifier to 0.85 would directly affect the 1st source of the stiffness and indirectly affect the 3rd source of the stiffness. However, the 85% composite action would allow some slip between deck and the girder and therefore only the 3rd source of the stiffness should be affected.

Therefore, in a detailed model with the deck and the girder explicitly modeled (which seems to be your case), your could reduce the 3rd source of the stiffness by connecting the girder and the deck with flexible links instead of rigid or fixed links. You would need to derive the stiffness of these links based on the discretization of your model and the 85% composite action.

Alternatively, if the composite section is modeled by a single frame element, the [stiffness modifiers] would need to be derived for the entire section.

Why I am getting jumps in my frame moment diagram? Why does the moment diagram follow saw-tooth pattern?

Extended Question: I modeled composite section using frame members for the girders and shells for the deck. However the frame moment diagram does not appear to be correct, since there are sudden jumps, resulting in a moment diagram which looks like a saw-tooth pattern.

Answer: Please note that the deck and the girders are connected to common joints to model a composite action. The jumps in the moment diagram at these connection points are caused by forces that are being applied by the deck to the girders at these connections. You can reduce these jumps if you refine the [test3:discretization] for the shell or frame elements to make these connection points distributed closely to each other.

Is there any difference in modeling composite sections in SAP2000 and ETABS?

• The modeling and analysis is similar between the two programs, however ETABS can perform a design for the composite section. This design capability is not included in SAP2000.

How can I obtain design forces for T-beam composite section modeled by frame and shells?

Extended question: I have a concrete floor modeled using finite element for slab and frame members for girders, beams and columns. The beam are girder members are offset to their physical locations. I found that the direct reading of member forces and moments cannot be directly used for the design of the composite T-beam section. How do I get the correct member forces for design?

Answer: It is important to remember that you are using finite element model with shells to model the deck and frames to model the supporting girders. If you need to obtain design forces for the design of T-Beam which corresponds to the girder and a tributary slab width, you would need to combine the corresponding forces from the frame and shell elements to obtain reasonable design forces for this composite T-Beam section.

Although there is no direct way to this in the current version (V14.0.0 as of 5/2009) of the program, you could try one of the following approaches:

• You could create a sequence of section cuts to obtain the design forces - see related [FAQ on sequence of section cuts] for additional details. This may require significant effort if done manually, but it would be a reasonable approach if it is automated using [Application Programming Interface (API)]. The [test3:discretization] should be refined as needed in order to adequately define the section cuts.

• You could also replace the rectangular beams in your structure with T-Beam section and modify the adjacent shell elements (using [test3:property modifiers]), such that they do not contribute the same stiffness and weight as the T-beams in the relevant directions. Then the T-Beam frame forces would directly correspond to the design forces for the composite section.

How can I model noncomposite action for girders modeled by frame elements and slab modeled by shell elements?

If the slab and the girder are connected to common joints then the [composite action] would be considered (please note that [joint offsets] and frame [insertion points] can be used to offset the slab from the girder). The composite action would be also considered the slab and the girder do not share any common joints, but full [body constraints] are used connect joints on the girder with corresponding joints on the slab.

To model noncomposite action (with the girder and the slab both contributing stiffness, but with slip allowed along the slab-girder interface), the girder and the slab should not share the same joints, but corresponding joints should be connected such that they share same deflection in gravity direction. For example, for a horizontal girder with a noncomposite slab, you could use equal Z constraint to model this condition.

To model a condition when the slab does not contribute any stiffness, you could use [test3:property modifiers] to reduce the flexural and axial stiffness of the slab in the direction parallel with the girders. I would recommend to use very small values for the property modifiers, say 1e-3, to avoid numerical problems that may occur when zero modifiers are used. Property modifiers for the direction perpendicular to the girders could be also modified to account for the stiffness of the forms.