Shear Center FE vs. analytical. NO MATCH

[flyforever85]

I need to validate the shear center in a complex geometry so I'm using a "C" section, a channel. I spent something like 5 hours but I can'y understand what I do wrong.

According with the attachment, my values are: b=2.95, h=6.1 and t=0.1. Analytically the shear center is 1.0966 from the center line of the web (Ix = 7.382). I then created a model in ABAQUS, same geometry of course, and a load applied at 1.0966 from the center line on the web generates a very small rotation. After 11 iterations, I found the shear center to be at 0.92966 from the center line of the web (rotation is down to 1.5e-8). There is a different of 0.16 in, not negligible at all in my opinion. What I'm doing wrong?

In abaqus I create a reference point and then with MPC I connect the reference point to the section. The load is applied at the reference point, deflection is around 2e-3 so no large displacements and/or non-linear effects.

 

[FEA way]

Which type of elements do you use ? Did you try with coupling constraint instead of MPC ? There might be some differences due to the fact that analytical solution is just an approximation and requires several assumptions.

 

[Erik Panos Kostson]

Not sure exactly what your are doing - in FEA if the point tip-load is applied on the shear centre (SC), then we would not see any twist.

Below is an example of a c-section beam element with load on the centroid (right beam below), where twist is seen (as expected), and one that has the load applied on the SC via a RBE2 element (left beam below), and as expected there is no twist. The RBE2 equivalent in abaqus is coupling of kinematic type or *kinematic coupling. Or even easier like in Strand7 where a rigid link (RBE2) is used, a rigid element in abaqus called RB3D2 can be added in the same way as in the Strand7 model above (just between the end-node of the beam and another node on the SC). With this method, the same results are seen in abaqus as below, with of course no twist of the section.

I must say though it is much easier for me to visualise the twist, render stresses in 3D on the section, and also run both material and geom. nonlinear analysis (do not think it is possible in abaqus with a meshed section) of a user defined beam sections (beam general section of mesh type in abaqus) in Strand7 than in abaqus. There is a free demo version of Strand7 should you want to try that out.

 

[flyforever85]

Thank both of you for you answers. Although my model still has a very small rotation (we are talking about e-5 or lower), I think my problem was the length of the channel. I made it only twice and long as the section height. Also, I used 3D elements (C3D8R), probably I should have used shell elements?

 

[Erik Panos Kostson]

Ok, thought you talked about beam elements - the same thing applies for shell or plate elements - that is if force is at SC then no twist (see image below - left beam has force at SC, right has it at the centroid).

Sure, it depends what you want to do - so for a local model, looking say for local buckling of the section (say web buckling), one would use shells.

On the other hand if you have 100 or 1000 of members, (say doing a global model large stair case, according say to EC3 standard), one would of course then use beam elements, get forces/moments and check against allowable capacities defined by the code. So global large models use perhaps beams, local models (say looking for local buckling, or other funny stuff, e.g., like local plasticity/yield on a one off section or connection), use shells.