Why is the measured tyre stiffness behaving contrary to what we expect from theory?

Hello all,

My thesis is based on the modelling a light agricultural tyre in ANSYS Mechanical. In my simulations I am subjecting the inside of the tyre to either a 2Bar or 0.8Bar as well as am applying a remote displacement to a road surface which is moved towards the tyre to cause tyre deformation. 

I am trying to understand what the smulation is doing but cannot understand where I am going wrong. Below I have attached my results, the solid lines represent the exisitng data that I am trying to match, and the dotted lines represent some of the simulations I have run. At this point in time I have only simulated a 2Bar, 0 camber as well as a 0.8Bar, 0camber case. 

I have two issues:

  1. As the stiffness of the tyre is determined by the slope of the line’s in the figure below, I tried adjusting the Young's Modulus to relax the stiffness of the tyre however found that with a decrease in the Young's Modulus the stiffness increases which is the opposite effect that is expected
  2. The model fairly estimates the tyres behavour for 20mm for the 2Bar case and around 30mm for the 0.8Bar case, however there after for both simulations the data points exponentially increase. 

As you can see in the figure, when removing the belt of the tyre and making it the same material as the tyre tread, the stiffness of the tyre increases which indects that something is happening in the physics that is causing the opposite expected behaviour.

Can anyone make sence of these behaviours?

The following are the connections. The frictional contact has a friction coefficient of 0.64 which is the frictional coefficient between rubber (tyre tread) and stainless steel (road).

The origin of the model sits at [x, y, z] = [0, 0, 0]mm and is at the center of the tyre:

To ensure that the tyre rim is treated as static the displacement [x, y, z] = [0, 0, 0]mm as follows is applied to the faces of the sidewalls which come in contact with the rim:

The internal pressure as said before is applied to the internal surface of the tyre. The image below is a section of the tyre, just so you can see on which surfaces the pressure is applied to.

And a remote displacement is applied to the road surface along the tyre-road interface:

As I have the vertial force-displacement curve of the experimentally tested tyre I can input the vertical displacement value and thoguh using a force reaction probe and a deformation probe I can collect the vertical force and displacement that my model experiences.

The force reaction probe:

where the "Coordinate System" is as follows:

The defomration probe then sits at the same point as the force reaction probe:

Please let me know if there is any other information that you might need.

Thank you in advance

Best Answer


  • Getting a model to match experimental data is a difficult task and is not limited to looking at the model. You also have to look at the experimental setup. For example, if the frame that is holding the tire loading mechanism and road surface is flexible, the instrument that measures displacement is measuring the combined displacement of the tire and the frame. Since you don't have the frame in your model, the model reports less deformation at the same force as the experimental data. In this case, you could add the frame to your model. This is unlikely to explain a 10 mm error, so it is more likely that your model is too stiff.

    Models can be too stiff if they do not have several elements through the thickness. Elements can exhibit volumetric locking, where they become too stiff. Look up Hourglass mode. There are keyopts that can be used on elements to prevent hourglass mode from developing. Poor element shapes can contribute to elements becoming too stiff.

    Material properties could be inaccurate. Do you have hyperelastic data for the actual rubber the tire is made from? Hyperelastic material models are highly nonlinear. You could have a material model that matches the rubber very well as low strains and becomes too stiff at high strains.

  • Hello @peteroznewman,

    Thank you for this. The 10mm error is not what I am primarily concerened about, it is that drastic increase in stiffness which you clarified for me.

    Regarding the Hourglass mode, is there a paper or a ANSYS manual you could refer me to as I cannot seem to find information assisting in describing the method that would help resolve the phenomenon. I did find this article which illustrated what happenes when the Hourglass mode is active in oes simulation: https://www.quora.com/What-is-the-hourglass-effect-in-finite-element-analysis-How-does-the-reduced-integration-resulting-in-the-hourglass-effect-work-How-can-we-counter-the-hourglass-effect

    I do want to point out that from what Ive seen, my model does not exhibit this sort of behaviour (as shown in the image).

    The material properties that I have have been based off of work done on previous tyres which are similar to mine and are linear properties and not hyperelastic/nonlinear. Thus I do not have the exact material peoperties of the rubber of my model. I have attached a more clear graph, the results of which have taken your recommendations regarding the force reaction probe into consideration, which illustrates the existing data I have (solid lines) as well as my simulated results for both the 0.8Bar and 2Bar cases. As you can see, the results better appraximate the vertical force at lower deformations and then show a exponentially increasing stiffness after a certain point for each of the respective cases. Is there no way to reduce the integration so that there are less volumetric constraints or to increase the order of the shape functions to reduce volumetric locking? As I read that the excessive non-realistic stiffness which I am getting in my results are due to interpolation errors which volumetric locking causes.

Sign In or Register to comment.