Static Structural Concrete Bending

  • Last Post 2 weeks ago
jacks3215 posted this 4 weeks ago

I am trying to carry-out a simulation for measuring concrete toughness (crack intensity) of a notched beam under three-point bending.

I followed a reference paper which has experimental results to verify the ANSYS simulation. According to that reference, a beam of 350x76x38mm, having a notch to depth ratio of 0.4, (notch height 30.4mm) was subjected to loading under displacement control rate of 0.06mm/min in three-point bending. The output values with different respective Young’s modulus values are shown in the attached image.

I have made the model and I have some queries, need some help on the following;

(1). How can I model crack propagation in ANSYS workbench?

(2). The model (A) is I am able to solve but I can not get the correct resultant values according to or near to those mentioned in the reference. Must be something I am missing, I feel that the applied load is maybe different than that of the experimental work. But how could I calculate how much displacement shall I apply in the model, as the displacement rate is mentioned in the experimental work?

(3). The model (B) I tried to design three-point having a span length of 304 mm. But somehow I feel that the design is not correct. Something is wrong with the bottom points which I have designed in the model (B) because of which I can not get the model to reach the solution. 

I would like to request for help and guidance on the said problem.

Attachments are as follows,

Experimental Setup




The model file is attached here at this link,

ANSYS Model File

Thank you

Order By: Standard | Newest | Votes
peteroznewman posted this 4 weeks ago

Please email me a copy of the reference paper. I don't know what FA/C is in the graph.

If you would say you were using ANSYS 19.0, I wouldn't waste my time opening 18.2 then finding that I can't restore your archive.

(1) The element SOLID65 in combination with the concrete material model can simulate crack formation.  Here is one post.  Here is another one.

 (2) The displacement rate is low, so just use a Static Structural model with a center support that has a displacement equal to the last displacement value in the paper. Request 100 Minimum Substeps to get 100 results along the way to the last point. You will plot the Force Reaction for the displacement support.

System A has the wrong supports and a mesh that is way too coarse. No surprise that you can't get anywhere near the correct resultant values mentioned in the reference.  Read the links I provided above.

However, the biggest reason why your results are a long way from the results in the paper is because their material is concrete and your material is Structural Steel. 

(3) System B has the proper supports for a 3 point bending test but contact is more difficult to solve. I mention in the links above how to replace contact with remote displacements. If you do that, the model should solve. Implement that and use a concrete material and reply with any new questions.

The figure you show has a rectangular notch, while your geometry has a sharp crack. Why are you not modeling what is in the experimental paper?

jacks3215 posted this 3 weeks ago

Thank you for your reply.

I have redesigned the model according to the links which you shared in your reply. The new model is attached here.

(1) I tried inputting the values for SOLID65 parameters from that reference paper, as per my understanding but the solution did not work. Then I modified the values from another work and the solution was able to work this time. I have marked my input values with ! in the solid65 command prompt. In the model, I am following the (FA/C = 4.0) results for getting corresponding Young's Modulus, Tensile stress, and compression stress. I tried changing the values of Uniaxial Cracking Stress and Uniaxial Crushing Stress to 1.8Mpa and 3.5Mpa respectively. I thought maybe these values are for the uniaxial tensile strength test and compression strength test. Kindly correct me if I am wrong for these steps.

(2) As for general discussion, I would like to ask that in three-point bending we could have either (i) two bottom fixed support and one top loading or displacement support or (ii) one top fixed support while the bottom two are loading or displacement support. Would the result be different for both of the mentioned cases (i) and (ii)?

(3) Within your model, I have seen you had the connection/contact tab in the mechanical, while as in my design I did not get this. I am not sure if you did modify something there or I have missed some steps while designing it.

(4) I randomly put a displacement of 30mm to check for the solution, I can not figure out the last displacement point from the reference paper as it is not mentioned there. 

(5) Basically, I am trying to simulate the experimental work to check whether the model could estimate exact or nearer value to that mentioned in the result. Later, I would like to design my own model to numerically estimate the values for fracture toughness. I do not have the necessary equipment to test the fracture toughness at my working place so I thought to estimate numerically and then use the estimated value for my research work. In your opinion, do you think this approach would be correct to get the fracture toughness value by simulation?



peteroznewman posted this 3 weeks ago

Hi Jack,

(1) I'm no expert in concrete material properties, but I have helped a few students get their model working.

(2) A three-point bending test may be done where the center contact has lateral constraints, and each end on the bottom of the beam is on roller supports. I don't think the bottom supports are typically fixed supports. How would you prevent lateral motion as the beam bends? The way I have modeled this in ANSYS is with a Remote Displacement scoped to a narrow area or just a split line on the bottom of the beam at each end. It seems simpler to move the center down rather than the two ends up, but your model is valid.

(3) You can right click on the Model item and Insert Connections, then you can right click on Connections and Insert contact or joint or spring etc.

(4) A displacement of 30 mm is too big, start with 0.3 mm and increase if you need to. Set the Analysis Settings to Number of Steps as 1 but Initial and Minimum Substeps to 100. Set the Restart Controls so you can restart if no cracking has occurred after 0.3 mm and you can add another step and a new displacement. That way you get some results. You can insert a Force Reaction in the Solution branch to show how the force for each increment of displacement.

(5) I don't know, but I don't think your models are going to be useful to estimate fracture toughness.


Your mesh is far too coarse.

I don't think you want to mix Fracture with SOLID65 Concrete Cracking. I think they are separate technologies.

Here is the result at 0.28 s.

Here is the results at 0.34 s after some cracks have formed.

Change the displacement to 0.34*0.3 = 0.102 mm you will have the solver complete Step 1, then the Cracking APDL will plot.

Attached Files

  • Liked by
  • jacks3215
jacks3215 posted this 3 weeks ago

Thank you for your detailed model.

One question I would like to ask how can I measure crack stress intensity factor (KIC or also known as SIF) in ANSYS within this simulation? In some references, I have seen for 2D simulation KCALC was used while as for 3D a direct approach in workbench is used, by inserting pre-meshed crack in the geometry.

peteroznewman posted this 2 weeks ago

Here is a 2D version of your model except with supports at the corners and a Pre-meshed crack with a Fracture Mechanics evaluation.

Attached Files

  • Liked by
  • jacks3215