I'm modeling simply supported and continuous reinforced concrete beams with flexural behavior. My goal is to get the full load-displacement response, including the post-peak behavior (after rupture of the rebars).
However, the analysis usually stops early with the error "too many attempts made for this increment".
I tried using automatic stabilization for the step and it usually helps, but the analysis still stops halfway through.
I noticed that the material properties I input have a lot of influence.
I'm using the Hognestad Parabola for the concrete with the Concrete Damaged Plasticity behavior and the elastic-plastic behavior for steel with the plasticity option. I'm taking the tension strength of the concrete as constant after the peak, because if I make it go back to near 0, the analysis stops very early. I'm considering linear strain hardening for steel and dropping the resistance to 0.1 MPa after that.
Let me know if you need more details.
Any help is appreciated.
Hi
This error can be on the grounds of many reasons, like assigning loads, boundary conditions, interaction, meshing and also details of increments, etc.
Please provide more information about your model like analysis type, interaction and so on ...
I think that you can enhance your meshing performance when you working according to convergence and divergence curve for a certain results that you need to found it.This may help to reduce your problems error
.These link may help you .
https://caeai.com/blog/how-do-i-know-if-my-mesh-good-enough
https://knowledge.autodesk.com/support/simulat…
Hi,
It is because the stiffness matrix results in negative definite. You may require to change the value of viscosity parameter in your CDP input. Please try 0.00001. Care should be taken into account when defining this parameter otherwise it will greatly affect the results of your model.
Thank you.
Sajjad:
I tried both force and displacement control. The beam is supported at both edges (roller and pin) and loaded at midspan. The rebars are embedded in the concrete. I'm using 0.01 initial increment size, 10^-8 minimum and 1 maximum with max 10000 increments. Nlgeo is off. Tried all automatic stabilization options, including none.
Asdam:
I tried that and it helped indeed, but I used 0.01 last time and it made much difference. I'll try this smaller value.
I also learned that the concrete may be failing due to lack of compression provided by the stirrups, since it's a 2D model and I'm modeling the stirrups as individual bars. Is there a way to model them as smeared reinforcement?
See a screenshot of my model below:
Hi
Thanks for providing detailed information. how did you assign the load (either displacement or load) at the center? this may cause this error? In order to be sure that the error is on the grounds of loading, you need to suppress it, then analysis, if you have no error , you need to change this condition. Other parameters you indicated seem to be good.
Hi
Initially I added a partition on the top edge and applied a boundary condition (displacement) at the partition point, like in the first picture. Afterwards I also tried distributing it over a small length on that edge, instead of applying it in a single point.
Thank you all, increasing the viscosity of the concrete to 0.0001 works. I was using 0 before and this was causing the convergence problem. The results don't seem to be affected by this value (I think it's low enough to not influence them).
First remove contact interaction. Then try to run your job. If same error popups then again apply your contact properties and no check for mesh. Use uniform mesh size and same element type. And also, make sure that properties that you are giving are correct.
You can try:
1. Increase IA (Step-Other-General solution control-edit step-specify-Time increment-more- change IA to the maximum value 30)
2. Refine the mesh in the contact regions to reduce the percentage of elements flipping in and out of contact.
3. Using mass scaling in Dynamic/Explicit to control the stable time increment.
- Badges
- Science topic