Learning Forum

[s310413]

Hi everyone, I'm new on Ansys. I'm trying to simulate a cylinder (radius=6mm, E=200GPa nu=0.3) on flat Hertzian contact under 185N normal load. According to Hertz theory I should get a contact pressure of around 330 MPa but I don't manage to get it on Ansys. I attach some details of the analysis, please can someone help me to find the mistake or anyone has suggestions? Thanks a lot

[Ashish Khemka]

Hi,

Please search YouTube for a video titled 'Hertz Contact Simulation using Ansys Workbench 2019 R3' and you will get relevant instructions.

Regards,

Ashish Khemka

[s310413]

Hi,

thanks for your response. I tried following that video suggestions but I still get 1000 MPa. In the video a normal displacement is applied while I have to apply a normal load so maybe the problem is in defining the load condition. Any other ideas? Thanks

[Ashish Khemka]

Hi,

Can you check the following post as well for suggestions? Modeling Hertzian Contact Stress in Line contact by two cylinders (ansys.com)

In addition, have you cross checked your hand calculations with any of the online calculators?

Regards,

Ashish Khemka

[peteroznewman]

Hi Gabriele, this is an online calculator I like to use.

https://amesweb.info/HertzianContact/HertzianContact.aspx

I put your data in but you did not specify the Line Contact length. If I use 10 mm it calculates a maximum Hertizan contact pressure as 328.4 MPa. If I use 1 mm it calculates a pressure of 1038.5 MPa.

It looks like you have created a 2D analysis. Did you choose Plane Stress or Plane Strain?  Plane strain is calculated based on a unit depth, so if you are working in mm, then the Plane Strain contact pressure is expected to be the 1038.5 MPa result.

[s310413]

Hi peteroznewman, I think you guess the problem. Actually I was trying to replicate a paper in which the author uses a 2D simulation and selecting plain strain. So I chose plain strain getting 1038 MPa as you said. So do you have any suggestion to get 328 MPa in a 2D simulation or the only way is a 3D simulation? Thanks

[peteroznewman]

If the physical problem has a 10 mm depth with a 185N normal force, and you build a Plane Strain model that has a 1 mm depth, the force in that 2D model should be in N/mm or a value of 18.5 N/mm and then you will get 328 MPa of contact pressure.

[s310413]

That was the mistake. Thank you!