SIMULATION PROBLEM 1

[StefBene]

I kindly ask for information about a simulation in ABAQUS with the explicit dynamic approach. I am simulating the bending behavior up to failure of a composite steel concrete beam. The model includes material non-linearities. The goal is to model an experimental test and confirm the collapse load, the test was performed in load control. The evaluation of the output is based on the response vertical displacement - load, the problem is how to know what is the maximum load that the model support. I noticed that in the simulation I reach the plateau of the displacement load curve in correspondence with the maximum load that I assign, doing so it is as if I fix the collapse load.
Other info: In the analysis the kinetic energy is lower than the internal one, therefore it does not center with the inertial effect. I don't use mass scaling and I simulate the experimental test in less time than the experimental test time.

Thank you for an answer.

 

[FEA way]

Do you use the CDP material model for concrete ? Is damage defined in this analysis ? There are some special output variables dedicated to each material damage model that can be used to determine failure.

 

[StefBene]

Thanks, the concrete is modeled with CDP considering the damage law, the steel through an elasto-plastic relationship (it is always far from the failure tension of the steel), the connecting elements between the steel beam and the concrete slab are springs nonlinear to which an experimental law has been assigned.

 

[Meysam Khodaei]

The simulation must be displacement control and you should verify RF of the moving support v.s it's displacement. Define moving support as a rigid body and use it's Referece Point's outputs.
Regards,
M. Khodaei

 

[StefBene]

Thanks Meysam Khodaei,
Ok, i try to do the test in displacement control. But I don't understand some things. If the beam were loaded with only one load concentrated in the centerline then ok, I increase the displacement in the centerline and as a force to draw the graph I take the constraint reaction multiplied by two. The problem is that the test I have to simulate is performed with six concentrated loads, so how do I increase the displacements of the various points to simulate the test? and what force do I take for the graph.

Thank you very much

 

[Meysam Khodaei]

You can define displacement constraints in different points independently.
Or you can define constraints in five points to follow U1 displacement from the sixth point and then define displacement for the sixth one.

 

[StefBene]

Thank you very much for your reply, I did the test in displacement control as suggested. A strange thing happens, the curve relating to the simulation in displacement control in addition to showing a lower ultimate load differs much earlier from the simulation in load control. can you justify me which curve to refer for the ultimate condition, and why?
I attach the graph.
Thank you so much

 

[bkal]

Can you show contour plots of principle stresses or damage parameters for both runs? Can you also show a view of the model indicating boundary conditions and applied loads. It could be that the way you load the model affects stress field close to the load application or prescribed boundary conditions.

 

[Meysam Khodaei]

I think displacement control is true because 1. Real experiments are displacement control 2. In load control, When the specimen fails because the force is bigger than static force, it accelerates and the simulation gets dynamic, not quasi-static.

 

[StefBene]

ok thanks