Brittle Material Bending Fracture in Static Structural

  • 62 Views
  • Last Post 6 hours ago
jackhero posted this 1 weeks ago

I am trying to simulate the brittle fracture of concrete under three-point bending. The concrete beam is 40mm x 40mm x 160mm with span length of 120 mm. The beam is not reinforced with any other material and is supposed to have a brittle fracture after some loading (experimental value around 5Mpa).

I would like to ask that how can I model the brittle fracture in static structural? I have defined the ultimate tensile and ultimate compressive load values in engineering data for the material. The simulation load is passing after the defined load values. I request if someone please guide me where I am doing wrong? I have used the PLC crack command to see the crack but I am not getting any thing there. I am only interested in getting the max load on which failure occurs and the crack on the material. The safety factor Mohr-Coulomb material model is optional.

I made the model in both 3D and 2D. Instead of drawing the physical rollers for the supports and loading, I have split the faces for the loading support at the top and bottom face for the two supports.For the 2D model it is quicker to solve but would be helpful if some expert may comment on whether the designed 2d model is correct or not.

Order By: Standard | Newest | Votes
peteroznewman posted this 1 weeks ago

 Jack,

The 2D model is incorrect for a 3 point bending model because your displacement has selected the entire top edge and not a vertex at the center.  You can create a vertex at the center in DesignModeler by splitting the edge.

The 3D model has created a narrow face to push on at the center. It would be better to put a remote point on that face and push down on the remote point, which will distribute the force to the face.

The 3D model also is holding two faces on the bottom with 0,0,0 displacement. That does not represent a 3-point bending test that is typically on rollers. Please review this discussion and come back with any questions.

The material you call concrete has no failure mechanism in it to generate cracks, but you can evaluate the Maximum Principal Stress and compare it with the Ultimate Tensile Strength to decide if a failure has occurred.  The Compressive Ultimate Strength value in the Material is only used by the Stress Tool to plot Factor of Safety.

Regards,

Peter

 

SandeepMedikonda posted this 1 weeks ago

Jack see, if these 2 videos of DrDalyo help:

Regards,
Sandeep
Best Practices to post on the Student Community

jackhero posted this 5 days ago

1. I would like to confirm that the failure criteria maybe defined as the UTS value only (ultimate tensile strength) in Engineering Data? In static structural, for linear elastic modeling, once this UTS value is reached the simulation would stop or give results that the applied load exceeded material ultimate strength. Is there any option to do something like this? Although the applied boundary conditions, as you have suggested, were not correct I have seen the simulation going pass the defined ultimate values. Maybe this is due to the incorrect boundary conditions but I would like to confirm about the failure criteria could be or could not be taken by ANSYS with the defined material values? I searched for this question in the community and came across to one of your post here, and it seems like we have to manually guess that the material failure has occurred.


2. I have seen some videos in which they have used Solid65 material to model the non-linear behavior along with the cracks (using PLC crack command). However, as you have mentioned that the default Ansys concrete material does not have the failure mechanism to generate cracks. Currently I am modeling the brittle failure only, in future if I were to model the non-linear behavior with cracks, is it like I can only select the Solid65 material instead of the default concrete material for crack observation? Or I have missed something when defining the default concrete material properties to include the crack as well?

3. For the 2D model, I split the top face while designing the beam in the Design Modeler.



I also split the bottom face for two supports.



But I did not get the split part when I had the final sketch. If you have time could you please take a look at where did I do wrong? It would be helpful if you may provide steps for creating the vertex at the center in DM by edge splitting? I have done face split for 3D models but for 2D I can not exactly figure out.

4. In 2D model, if I were to add displacement for the two bottom supports at the two extreme ends isn't it like no need to split the bottom face of the beam as I have done in the image shown above?

5. Are there any tutorials or guide available of 2D model designing for the ansys design modeler? And for creating symmetry, axisymmetry models.

6. For the two bottom supports, you mentioned in the discussion to use Z=0 for the roller bars, with all other displacements and rotations are free.

In one of your 2D designed model for fracture toughness by three point bending, the bottom supports were X=0, Y=0, for one end of the displacement while as Y=0 for the other end of the displacement.

 



Although the first model is 3D but the displacements applied or suggested to apply are same on both of the bottom supports. However in the 2D model the displacement applied on the bottom are different on both ends. Could you please suggest which one would be better to use?

7. In addition, with in that 2D fracture toughness model, the force applied on the top seems to be on the entire edge instead of the vertex as you have suggested in your reply above. If this was done deliberately, it would be helpful if you may explain the reason for it.



peteroznewman posted this 3 days ago

1. Engineering data holds the Ultimate Tensile Strength, but it has no effect on the solver. The solution will not stop when this value is reached. The only time this value is used is when you put the Stress Tool into the Results and plot the Factor of Safety. Then the UTS is divided by the Stress to compute the Factor of Safety.  If the material model is a linear elastic material, the solution can take the stress result way past the UTS. It is only in Post Processing, that you can make a plot like the Factor of Safety to show if the material is over or under the failure value of UTS.  I don't usually plot Factor of Safety. I prefer to just plot the stress (Max Principal for brittle materials, von Mises for ductile materials), and I set the value on the legend that separates orange from red at the value of UTS then any material colored red has failed. For ductile materials, instead of using a linear elastic material, I add a plasticity material model. That allows the material to stretch at values of stress above yield. Then instead of comparing stress to UTS, I look at Total Strain and compare that to Elongation. In this case, I set the threshold on the legend between orange and red to the value of Elongation and any material colored red has failed.

2. Solid65 is an element type not a material.  Solid65 elements are designed to work with the Concrete material.  When you use concrete and solid65 elements together, the material has failure mechanisms built in and the ability to simulate cracking and crushing.  The problem with the concrete/solid65 combination is the results are extremely sensitive to the mesh used in the solution. You have to use very small elements and very slow loadings and a slightly different mesh can give a very different result. 

Some people are more interested in the gradual failure of a concrete beam and a plasticity model is more useful than the cracking model used with Concrete/Solid65 approach.  A plasticity model has been developed called Microplane that is very robust and gives accurate results across a wide range of meshes. You can read the Microplane example in the Technology Guide in 19.1.  Here is a discussion on that topic.

3. You can put a plane at the center and use Slice, then put the two pieces in a Multibody part using Form New Part in DM.

4. You don't need any overhang, you can just apply the supports on the corner vertices.

5. Look on YouTube for tutorials on 2D design modeler.

6. In a 2D model without using symmetry about the center, you need one support to have X=0, Y=0 and the other support to have just Y=0.   If you have symmetry at the center, then the one support only needs Y = 0 because the symmetry prevents motion in X.

7. You can apply a force to the entire top surface of a beam. That is called a distributed load. That is not how a 3-point bending test is done, but it is a valid load.  Applying a displacement to the entire top surface is not a valid load.  A typical 3-point bending test is to apply a displacement load to a point or small area at the center.

Regards,
Peter

  • Liked by
  • jacks3215
jackhero posted this yesterday

3. You can put a plane at the center and use Slice, then put the two pieces in a Multibody part using Form New Part in DM.

 

I can not exactly follow this it would be helpful if you may show the steps graphically (screenshots). 

I created a new plane at  the center.

Right click on new plane > insert > slice

Then I get these options and for some of these I can not select the target body or the face for slice.

 

 

 

peteroznewman posted this yesterday

The XY axis of a plane does the slicing.

If you copy the YZ plane to the center, then that will be correctly oriented to do the slicing.

You can change the Base Plane to YZ or you can rotate the plane you have at the center.

  • Liked by
  • jacks3215
  • jackhero
jackhero posted this 16 hours ago

I followed the instructions and ended up with this.

 

However, while applying load on the top surface I can't find the vertex using the vertex selector. I turned on to show all the vertex and the point I created is not shown in there. Have I missed something in the DM or I am applying the loads in incorrect way in Mechanical?

peteroznewman posted this 15 hours ago

In one of your earlier screen shots I saw a Solid that was suppressed and a Surface Body that was not.

In your recent screen shots, I see the Solid has been sliced into two, but the Surface Body has not.  Delete the Solid Body and try the Slice on the Surface Body.

jackhero posted this 6 hours ago

I re-modified the design to slice the Surface Body. After Slice I selected both parts and formed a new single part. This is the final design I get in the DM.

I am not sure if I have followed your instructions correctly but I am ending up with this in the Mechanical. I had to separately assign Material Properties to both of the Surface Bodies under Part 2. Is it normal to have like this or I again have missed something in the DM?

 

peteroznewman posted this 6 hours ago

Yes, each body needs a material assignment. That is one of the benefits of Slice.  Instead of slice, you could have used Concept, Split Edge, and created a vertex at the 50% point on the edge.

  • Liked by
  • jackhero
Close