How to Troubleshoot ANSYS Contact Issues

How to Troubleshoot ANSYS Contact Issues

Please Share Us

点击此处查看 ✿水哥原创ANSYS视频教程清单 ✿


What is a contact in ANSYS?

Do you know what a contact is in ANSYS? It’s a way of defining how different bodies interact with each other in an assembly. Without proper contacts, components may overlap or pass through each other, which can cause significant problems. In this article, we will explore why contacts sometimes fail and what you can do to fix them.

What happens when a contact is not defined or is not working properly?

What happens when a contact fails to work properly? Well, without a defined contact, the components in an assembly won’t interact with each other as expected. Even if a contact is defined, it may not be functioning correctly, leading to further issues.

I have defined contacts but ANSYS is not seeing them. What now?

If you’ve defined contacts in ANSYS, but the software doesn’t seem to recognize them, don’t panic. The first step is to figure out which contact is causing problems. You can do this in several ways.

1. Use the contact tool.

To access it, simply right-click on connections, hover your mouse pointer on Insert, and then left-click on Contact Tool. This will add a contact tool item to the tree. From there, you can right-click on the contact tool and select “Generate initial contact results”. This will bring up a list of the contacts in the model with some information about them. The contact tool is especially helpful for assemblies with multiple contacts.

How to Troubleshoot ANSYS Contact Issues

ANSYS Contact Tool

One of the most helpful features of the contact tool is the color-coding. Red contacts are those that require immediate attention, while orange contacts are worth investigating. You can select multiple contacts and then right-click to “Go to selected items in tree”. This will help you identify and address any problematic contacts.

How to Troubleshoot ANSYS Contact Issues2

Contact Tool – Assembly with one contact

It’s worth noting that if you’ve defined MPC contacts in the model, they won’t appear under the contact tool. However, you can still troubleshoot them using other methods.

2.Check your results at actual size

It’s important to do this step, even though it may seem obvious. Sometimes, we may overlook it. Take a look at the image below. Even though our solution appeared to be complete, there is obvious interference between components. In some cases, there may be an incomplete solution, which can give you an idea of which components are not fitting properly.

How to Troubleshoot ANSYS Contact Issues3

Contact – Bodies interference

3.Pay attention to any error or warning messages

If certain parts are meant to only be constrained in a specific direction and the constraints are not detected, it may result in rigid body motion and solver pivot warnings. You might also receive an error message like the one below:

*** ERROR *** CP = 2.016 TIME= 10:26:54 There is at least 1 small equation solver pivot term (e.g., at the UX degree of freedom of node 219). Please check for an insufficiently constrained model.

This message is helpful. If you have a large assembly with multiple contacts, you can identify the component or contact with large deformations by its node number. To do this, you can create a named selection with the node number. Right-click on Model, hover over Insert, and select Named Selection. Then, select “worksheet” as the scoping method and choose the relevant drop-downs from the cells. In our case, we want to create a named selection for node 219, as shown below.

How to Troubleshoot ANSYS Contact Issues4

Named Selection

How to Troubleshoot ANSYS Contact Issues5

Mesh Node Selection

After entering the necessary inputs, click “Generate”. Then, click on the named selection you just created and ANSYS will highlight it for you, as shown below. You can see that the grey body is displacing indefinitely.

How to Troubleshoot ANSYS Contact Issues6

Named Selection Flag

Now that you have identified the problem contact(s), you can take steps to address the issue(s).

Steps to address contact issues

If you’re experiencing issues with contact, there are a few steps you can take to address them. Keep in mind that some of these steps may work better than others, and you may need to use a combination of them.

1). Look for gaps in the geometry: Sometimes, you might not have intended gaps in the areas where contact is happening. You can fix this by adjusting the geometry. If you’re using ANSYS Mechanical, you can also use the geometry interface setting to fix any gaps (check out point 8).

2). Double-check the contact type: Make sure that you’ve defined the right kind of contact. Maybe you meant to have frictional contact with an initial gap, but you accidentally defined it as bonded.

3). Check the pinball radius: The pinball radius determines the area where the contact search takes place. You can adjust the pinball radius in the advanced contact settings. If you want more information on how pinball radius works, check out the ANSYS help.

“In the Contact Behavior properties, you can set the Pinball region, which allows you to specify a contact search area commonly referred to as a pinball region. Setting a pinball region can be useful in cases where initially, bodies are far enough away from one another that, by default, the program will not detect that they are in contact. You could then increase the pinball region as needed. Consider an example of a surface body that was generated by offsetting a face of a solid body, possibly leaving a large gap, depending on the thickness. Another example is a large deflection problem where a considerable pinball region is required due to possible large amounts of over penetration. In general though, if you want two regions to be bonded together that may be far apart, you should specify a pinball region that is large enough to ensure that contact indeed occurs.”

4).Make sure your mesh is “reasonable”. Sometimes, if the elements are of poor quality or too coarse, it can result in odd contact behavior.

5).Check your contact detection algorithm. ANSYS allows you to select an algorithm for contact detection to help with solution convergence. The Nodal-Projected Normal From Contact method is the latest and possibly the most robust option. It can often help achieve convergence when other methods fail.

6).Apply the load more slowly. ANSYS may not be able to detect contact with an initial gap if the load is applied too quickly. You can ramp the load slowly by specifying sub-steps or using multiple time steps and applying a smaller load in the initial step.

7).Try applying the load as a displacement instead of force or pressure. A displacement-controlled model is usually more robust than a load-controlled model.

8).Consider using “Adjust to Touch” for the interface treatment. For non-linear contacts such as frictionless, rough, or frictional, you have the option to define the contact interface treatment as part of the Geometry Modification Setting. This ensures that initial contact occurs even if there are gaps present, as long as they are within the pinball region.

How to Troubleshoot ANSYS Contact Issues7

Adjust to Touch

Note that if you have concentric cylinders with a small initial gap, you may need to manually specify the gap with the Add Offset, No Ramping option. Gaps may still be present if the contact pair has regions of differing gaps, but this setting ensures that the smallest gap is closed to allow for initial contact.

Good Luck!



有时间麻烦帮忙点击下公众号文末的广告哦, 权当码字的辛苦费,感谢大家!

Please Share Us
© 版权声明
点赞0赞赏 分享
评论 抢沙发