numerical singularity issue in ABAQUS

[martino81]

Hello everyone,

I have been trying to model in ABAQUS (I am new to the software) a simple supported reinforced concrete beam. I have used solid elements for the concrete beam and wire elements for longitudinal rebars and stirrups.

The simulation keeps failing for 'numerical singularity' issues. I have checked my boundary conditions and constraints and everything looks fine. Both supports have U1=U2=U3=0 and all the reinforcement is constraint to the beam with an 'Embedded region' type constraint. The problem appears to occur on the node located on every longitudinal rebar (24 rebars along the perimeter of the section) at midspan. The red dot in the picture below shows the node where the singularity occurs, i.e. on the rebar at midspan. There are other 23 failures occuring at midspan and corresponding to the remaining rebars.

Do you have any suggestion on what the issue might be?

I appreciate your help.

Thank you very much.

Regards,

Martino

 

[corus]

It could be that your beams aren't tied to the 3D elements or more likely that the beams are able to rotate whilst being tied translationally.

 

[martino81]

This is exactly what is happening as the error occurs on DOF 6 which I believe is twist (rotation around the beam axis). I thought the embedded region constraint would have prevented that though.

Any suggestion how to solve this? I am only trying to repeat this exercise

https://www.youtube.com/watch?v=XzJC8Nqf8vo#t=15.465033.

I have exactly done what the guy in the video does.

However, I wonder if there is a more efficient way to model reinforced concrete with appropriate elements which I know they are available in ANSYS for instance. With these elements there shouldn't be the need to model the steel reinforcement.

Thank you for your replies.

 

[corus]

In the video he says that he either uses 3D beams or wires. Without checking, perhaps the wire doesn't have DOF 6 and so removes this problem. Similarly the problem wouldn't occur if you used 3D solids for the beams as these have only translational DOF.

 

[martino81]

Thanks Corus. I had already solved the problem. I used truss elements which have only 3DOF. Beams shouldn't be used therefore I guess the video is a bit misleading although he seems to make it work. He uses wire as part and beam as section (in the second part of the video). He should use truss elements as rebars do not take shear and bending but only axial loads. In addition modelling reinforcement in 3D solid is computationally hard and should be avoided.

 

[Dave442]

There is a chapter in the Analysis User's Guide that describes different methods of defining reinforcement. It's not something I've had to do in the past but the different methods seem well defined. Might help you out if you haven't already read through it:

Abaqus Analysis User's Guide 2.2.3 Defining Reinforcement

 

[martino81]

Thank you everyone for your help!