(ABAQUS) Earlier Failure and Unrealistic Cracking of Reinforced High Strength Concrete Beam Under Bending Simulation

[Daniel_LEE]

Hi all,

I am simulating a RC beam under 4-point bending test and the results were terrible. I have attached the results below and I have three problems that I have no idea how to solve. I have been refining this model for the past few weeks. I could not resolve the problems and thus seeking help here. I would be really grateful if anyone could help me on this.

Model Description: I am building a reinforced high-strength concrete beam under 4-point bending test. The steel reinforcement includes ties, tensile bars with anchorage and minimum reinforcement bars at the compression zone of the beam. I have defined CDP damage parameter with relationship I have obtained by inserting concrete properties into an excel. I followed standard settings for interaction of the parts I have seen on YouTube. I used "embedded region" for constraining the steel bars and concrete beam. For the loading point and simple support simulation, I define them with steel material properties, used "general contact" as their contacts with the beam. I have then partition the support into half and applied boundary condition to the partition lines. For the loading, I have used "rigid body" constraints to tie the reference point to the loading plate and then applied point loads to the reference point.
The analysis took roughly 30 hours and has a total of 13811 increments. I am not sure if this is normal. The dimension of the beam is (3600x250x400) in mm.


The problems are as follows:
1) The load-deflection curve showed an earlier failure, approximately 100kN lower in ultimate strength, of the beam.

2 The bending stress distribution within the bending is not realistic. The results at the end of the analysis showed concentrated stress distribution around the loading point, where as the bottom of the beam where should experience the highest tensile stress only showed average stress values.

3) At the end of the analysis, the entire beam had cracks formed all over it. The result attached should indicate a beam that has been completely torn apart. which is not realistic and does not match with the experimental result. Even the compressive damage value is unrealistic.

I have tried to find the cause of these problems and specifically looked at the instant when failure of the beam started. Yet, I did not know how to interpret the results and thus had not idea how to proceed to resolve all these problems. I would be really grateful if someone could provide me with some advice on what to look into or share their experiences in modelling RC beam under bending.

 

[FEA way]

I have defined CDP damage parameter with relationship I have obtained by inserting concrete properties into an excel.

Maybe CDP model parameters are not accurate and require further calibration.

I used "embedded region" for constraining the steel bars and concrete beam.

This is correct but I would rather model the reinforecement using embedded beam elements.

What type of solid elements are you using ? Did you try refining the mesh ?

For the loading, I have used "rigid body" constraints to tie the reference point to the loading plate and then applied point loads to the reference point.

Accurately modeled supports are very important. Are they really just cuboid plates ? Also, it would be better for convergence (you've mentioned it was very slow) to use prescribed displacement instead of force.

 

[Daniel_LEE]

Maybe CDP model parameters are not accurate and require further calibration.

I have doubled checked the CDP parameters, and it seems to be fine. It is also verified by experiments so I guess that might not be the major problem here. But I would like to ask one thing regarding the DAMAGET in ABAQUS, if an element is completely red under this parameter, does that equivalent to a wide opening crack on the concrete beam in real life?

What type of solid elements are you using ? Did you try refining the mesh ?

I am using C3D8R for the solid element. I haven't tried refining the mesh because using mesh size of 40mm already took the software one literal day to run the analysis. I am afraid that using more refined mesh would take much longer.

Accurately modeled supports are very important. Are they really just cuboid plates ? Also, it would be better for convergence (you've mentioned it was very slow) to use prescribed displacement instead of force.

Yes, I am using cuboid plates to model the support and partitioned the plates into half. I then applied boundary conditions to the partition line.
Yes, I am also using displacement load in the analysis. I have actually tried to use both point load and displacement load. In my case, point load gives a much faster convergence rate than displacement load, roughly 2 times faster.

 

[FEA way]

But I would like to ask one thing regarding the DAMAGET in ABAQUS, if an element is completely red under this parameter, does that equivalent to a wide opening crack on the concrete beam in real life?

Check the paragraph Visualization of “Crack Directions” of the documentation chapter about CDP material model. DAMAGET is just a (tensile) damage variable:

The damage variables can take values from zero, representing the undamaged material, to one, which represents total loss of strength.

I am afraid that using more refined mesh would take much longer.

Sometimes it actually improves convergence rate if too coarse mesh causes convergence issues.

In my case, point load gives a much faster convergence rate than displacement load, roughly 2 times faster.

Usually, it's the opposite in nonlinear analyses, especially with contact. Maybe it's a matter of the magnitude of displacement or applied amplitude.

 

[Daniel_LEE]

Check the paragraph Visualization of “Crack Directions” of the documentation chapter about CDP material model. DAMAGET is just a (tensile) damage variable:

I have read that paragraph and I am a little bit confused with the description stated in the document with interpretation of my model. I am using another model to illustrate my confusion. The paragraph said the normal vector to crack plane is parallel to the direction of max principal plastic strain, which is pointing upwards in the picture. Then, that should imply a horizontal crack for the left notch in my model. However, from the "DAMAGET" parameter view, I the left notch has a vertical loss of concrete strength. From my understanding, this should imply a vertical crack which gives such as direction of strength loss.

Sometimes it actually improves convergence rate if too coarse mesh causes convergence issues.

I see, let me try that.

Usually, it's the opposite in nonlinear analyses, especially with contact. Maybe it's a matter of the magnitude of displacement or applied amplitude.

Yes, I am working with non-linear analysis. Point load gives faster analysis results but the ultimate load is 10 times less that the experimental result. Whereas displacement load show a lower displacement result, but more accurate result.

I think one of the reasons that make the analysis having a low convergence rate is because of the boundary conditions at the load. I am current using rigid body constraint to tie the reference points to the loading plate to simulate 4-point bending test. I notice that in real life experiment, the loaded beam is allowed to rotate and move sideway a bit when it deformed. Using rigid body constraint may not be able to capture that and may be an incorrect boundary condition. I have tried to use "coupling" constraint to relax degree of freedom in DOF3 and DOF4, yet the analysis is aborted immediately, I am still figuring the reason to that. May I know how do you usually simulate 4-point bending test?