Reply To: To shell or not to shell, that is the question.

[Kaushal Vadnere]

 

 

Hi

Shell elements generally do not have stress component in thickness direction. That means you cannot get stress distribution through the shell thickness so, top and bottom faces of the shell will have same stresses.
But they do transfer force in out of plane direction as bending stress component exist. The reason you might be getting zero contact pressure on shell elements is because the default contact behaviour is ‘Asymmetric’ and using this behaviour, results are only reported on the contact side (I am assuming you have selected the solid body as contact and shell body as target). You can check in the Initial Information in Contact tool that only contact side is active for assymetric contacts. If my assumption is right, try changing the contact behaviour to ‘Symmetric’ and solve again to check if you get contact pressures on shell body as well. Also, I believe you have scoped multiple contacting pairs in single contact object, this is not recommended. Plase create different Contacts for every individual contact pair and make sure that you have set Shell Thickness Effect to Yes and select appropriate Contact Shell Face in the details of contact.
To learn more about contact formulations and behaviours, please refer to this article in Ansys Help Document: 9.6.3.2. Definition Settings
If you cannot open the above link, refer this: How to access the ANSYS Online Help
Refer to these free Ansys Innovation Course on Contacts: Contact Mechanics | Ansys Innovation Courses, Fundamental Topics in Contact | Ansys Innovation Courses
You can refer to Lesson 2 of this free Ansys Innovation Course to learn more about shell modeling: Geometry Representation | Ansys Innovation Courses
Hope this helps.