Seeing the result after simulation

  • Last Post 4 weeks ago
Shivani posted this 17 January 2018


I am trying to simulate a model which is a sandstone cube with a bolt fixed in one of it's face.I have applied all the boundary conditions and the model has been simulated.I would like to see the damage caused to the bolt and the cube separately due to applied pulling force on the bolt but I am not able to see that after the simulation.

Some perspective would be very helpful.

Order By: Standard | Newest | Votes
peteroznewman posted this 18 January 2018

Hi Shivani,

There are many different types of simulation models that have different purposes.

When I perform a simulation, it is usually to predict the load at which failure would occur, and compare that with the expected service load to calculate a factor of safety. With that goal, I don't need to simulate the behavior of the system beyond the point of failure.

A Static Structural model will calculate the stress in the sandstone and the bolt for a specific load. The result is the maximum stress in each part. You need to compare the maximum stress with the strength of the material.  If the stress < strength, then no failure or damage is predicted to occur in a physical test.  If the stress > strength, then failure or damage is predicted to occur in a physical test, but you won't see that in the simulation, that happens only when you compare with the strength.

There are other models that are built to simulate the damage caused when the stress > strength of the material. Explicit Dynamics is one software module in the toolbox that can simulate the damage to a material. The material has to include a failure model so that the elements that exceed the failure criterion are removed during the simulation.  Here are three videos of rebar being pulled out of concrete. There are two concrete material models with different failure criteria and a steel with no failure criteria.  I hope they help you understand how different types of simulation can be used.

  • Liked by
  • Shivani
Shivani posted this 18 January 2018

I have begun learning explicit simulation,thank you for your insight.

Shivani posted this 18 January 2018

I tried to simulate my model with basic settings(all of them default) and setting my boundary conditions.The running of simulation gives an error (A general failure occurred during the solution process.).How should it be overcome?

And also I am simulating the model with the purpose of seeing the effect of applied force on the nut and the cube.And would like to keep changing the boundary conditions for the experiment.Should I be going forward with static structural or simulate in explicit analysis?


peteroznewman posted this 18 January 2018

To predict the load on the bolt when damage would occur to either the sandstone or the nut and bolt, use Static Structural. If you know the sandstone is stronger than the nut and bolt, you can turn on plasticity in the material model of the steel and see the damage to the nut only if the sandstone does not fail first.

To see the damage to the sandstone, you need Explicit Dynamics or the Ekill ACT extension for Static Structural, but ACT is not available in the Student license.

I recommend you first learn Static Structural. You will have to learn to define frictional contact.  You will also need to know the strength of the sandstone. Do you know that?


  • Liked by
  • Shivani
Shivani posted this 19 January 2018

Yes, I have the strength of the sandstone.Although I'm not very well versed with all the details in frictional contact.I have set rough contact as the type of contact.

From my simulation I first need to see the damage done to the sandstone and nut due to applied load.This I need to do for various values of stresses.And I would also like to see the safe loading conditions,so that no damage is caused to either.What do you recommend?

peteroznewman posted this 5 weeks ago

Start with a Static Structural model of the nut on the face of the sandstone. I expect you will apply a load to the shaft of the bolt (you don't need the bolt head) and calculate the stress in the steel and sandstone. Then compare those values of maximum stress with the strength of sandstone and steel. You can then predict the load at which damage would begin.

You can attach an ANSYS Project Archive (.wbpz file) to your post above, if it is < 120 MB. You can Clear Generated Data on the mesh to reduce the file size.


  • Liked by
  • Shivani
Shivani posted this 4 weeks ago

I am attaching the simulated model in the post.

The results are really weird .

Attached Files

peteroznewman posted this 4 weeks ago

I find that the cube and Resing Grout are assigned a material of Structural Steel.

You should always insert a Contact Tool whenever you use Contact in your model. The contact tool shows the contacts are far open.

That is because there is no hole in the cube or the resin grout and why the nut is being pulled out to an enormous distance.

There are also two extra bodies in the simulation that don't belong. They should be suppressed. I imagine those are the bodies you meant to Boolean Subtract from the cube and resin grout to create the holes, but that is not what you have. Your archive doesn't include C:\Users\my\Documents\pullouttest6.iges so I can't fix that for you.

Fix the above problems and try again. But this time, open the Geometry in DesignModeler and it will be saved in the Archive.

Tip: You can have one pressure BC and pick 4 faces, since pressure always acts normal to the surface.

  • Liked by
  • Shivani