August 8, 2018 at 10:20 pmjonsysSubscriber
I am interested to know how generating Initial Contact from Contact Tool, helps to further decide which contact parameters should be changed to have a better model.
I know that someone probably gets this kind of experience with time (therefore it is not easy to explain it in a post), but I would like to know let's say some rules of thumb. Or which output parameter from Initial Contact affects which parameter at Details of Contact (like Trim, Formulation, Detection Method etc)
August 8, 2018 at 11:00 pmSandeep MedikondaAnsys Employee
First, one of the advantages of having a worksheet view is you can easily modify your selection of contact regions in the Worksheet :
- Add or remove pre-selected groups of contact regions (All Contacts, Nonlinear Contacts, or Linear Contacts), use the drop-down menu and the corresponding buttons.
- Add any number of contact regions, you can also drag-drop or copy-paste any number of contact regions from the Connections folder into the Contact Tool in the Tree View. Also, one or more contact regions can be deleted from the Contact Tool worksheet by selecting them in the table and pressing the Delete key.
- Change the Contact Side of all contact regions, choose the option in the drop-down menu (Both, Contact, or Target from the drop-down menu and click the Apply button).
- Change an individual Contact Side, click in the particular cell and choose Both, Contact, or Target from the drop-down menu.
Next, and more importantly it gives you a better idea if the contact is open/closed or near-open. That means that it gives you an opportunity of adjusting pinball radius so that the contact doesn't miss during the solution. So look out for the yellow colored contacts. Now lets say you are observing a penetration in your model it gives you a chance to change the contact detection method (integration point/nodal) or use adjust to touch etc or even change the contact stiffness (again these can be changed from the worksheet itself).
Hope that helps a little.
August 9, 2018 at 12:38 ampeteroznewmanSubscriber
I want to see a contact is closed, since I always go into CAD and move parts around to put them into initial contact, like a tangent condition, before the solution begins. Though the geometry is tangent, after meshing, there can be a tiny gap.
If Frictional, Frictionless or Rough contact, is not closed, then I use Adjust to Touch to close the contact. I use this frequently.
If Bonded contact is not closed then I make the Pinball Radius larger. I use this rarely.
August 10, 2018 at 1:49 pmjonsysSubscriber
Sandeep and Peter,
thank you for your replies, I always find them very helpful.
So while working with Contact, our aim will be to change contact properties in order keep the Geometric Penetration and Gap close to 0?
I can see as well that Contact 'Formulation' (under Advanced) has a considerable effect on Geometric Gap, Normal and Tangential Stiffness. What should be kept in mind when choosing Formulation?
August 10, 2018 at 3:26 pmSandeep MedikondaAnsys Employee
Ideally yes, because there is no penetration in a physical sense. Although it becomes very difficult to do this in like a snap-fit type of analysis using highly deformable bodies.
With regards to your question on different formulations, this differs widely based on numerous factors from geometries to the type of analysis you are doing to the kind of materials you are using. Hopefully, the following resources will give you some more insight into this:
- Resource 1: Blog posts by John Doyle (@jjdoyle); 1 & 2.
- Resource 2: This section from the manual.
- Resource 3: Best practices for specifying Contacts.
Note that the contact stiffness is like a spring acting in between the 2 bodies and depending on how strictly it is enforced, it is expected for it to change significantly
August 10, 2018 at 5:36 pmpeteroznewmanSubscriber
One situation where I do not use Adjust to Touch is when there is a deliberate, designed-in interference fit.
At room temperature, a shaft may be 0.1 mm larger in diameter than a hole. I want that penetration to exist unchanged at the start of the solution, then the contact algorithm will stretch the hole and compress the shaft until there is no significant penetration at the end of the solution.
In a practical sense, the part with the hole may have been heated to a high enough temperature where the cold shaft has clearance and can be slipped into the hole. As the parts come back to room temperature, the interference returns. Now you can include the thermal changes in an ANSYS model, or you can just run the simulation at room temperature and let the contact algorithm resolve the interference.
December 11, 2019 at 5:14 pmJerinSubscriber
Can you share these resources again. I am not able to get theses blogs again by clicking on the resource link.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- How to calculate the residual stress on a coating by Vickers indentation?
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.