Default Contact Stiffness Behavior for Bonded Contact

Categories:

p7 It recently came to my attention that the default contact stiffness factor for bonded contact can change based on other contact regions in a model. This applies both to Mechanical as well as Mechanical APDL. If all contacts are bonded, the default contact stiffness factor is 10.0. This means that in our bonded region, the stiffness tending to hold the two sides of contact together is 10 times the underlying stiffness of the underlying solid or shell elements.

However, if there is at least one other contact region that has a type set to anything other than bonded, then the default contact stiffness for ALL contact pairs becomes 1.0. This is the default behavior as documented in the ANSYS Mechanical APDL Help, in section 3.9 of the Contact Technology Guide in the notes for Table 3.1:

“FKN = 10 for bonded. For all other, FKN = 1.0, but if bonded and other contact behavior exists, FKN = 1 for all.”

So, why should we care about this? It’s possible that if you are relying on bonded contact to simulate a connection between one part and another, the resulting stress in those parts could be different in a run with all bonded contact vs. a run with all bonded and one or more contact pairs set to a type other than bonded. The default contact stiffness is now less than it would be if all the contact regions were set to bonded.

This can occur even if the non-bonded contact is in a region of the model that is in no way connected to the bonded region of interest. Simply the presence of any non-bonded contact region results in the contact stiffness factor for all contact pairs to have a default value of 1.0 rather than the 10.0 value you might expect.

Here is an example, consisting of a simple static structural model. In this model, we have an inner column with a disk on top. There are also two blocks supporting a ring. The inner column and disk are completely separate from the blocks and ring, sharing no load path or other interaction. Initially all contact pairs are set to bonded for the contact type. All default settings are used for contact.
p1

Loading consists of a uniform temperature differential as well as a bearing load on the disk at the top. Both blocks as well as the column have their bases constrained in all degrees of freedom.
p2

After solving, this is the calculated maximum principal stress distribution in the ring. The max value is 41,382.
p3

Next, to demonstrate the behavior described above, we changed the contact type for the connection between the column and the disk from bonded to rough, all else remaining the same.
p4

After solving, we check the stresses in the ring again. The max stress in the ring has dropped from 41,283 to 15,277 as you can see in the figure below. Again, the only change that was made was in a part of the model that was in no way connected to the ring for which we are checking stresses. The change in stress is due solely to a change in contact type setting in a different part of the model. The reason the stress has decreased is that the stiffness of the bonded connection is less by a factor of 10, so the bonded region is a softer connection than it was in the original run.

p5

So, what do we as analysts need to do in light of this information? A good practice would be to manually specify the contact stiffness factor for all contact pairs. This behavior only crops up when the default values for contact stiffness factor are utilized. We can define these stiffness factors easily in ANSYS Mechanical in the details view for each contact region. Further, we need to always remember that ANSYS as well as other analytical tools are just that – tools. It’s up to us to ensure that the results of interest we are getting are not sensitive to factors we can adjust, such as mesh density, contact stiffness, weak spring stiffness, stabilization factors, etc.

Categories

Get Your Ansys Products & Support from the Engineers who Contribute to this Blog.

Technical Expertise to Enable your Additive Manufacturing Success.

PADT’s Pulse Newsletter

Keep up to date on what is going on at PADT by subscribing to our newsletter.


By submitting this form, you are consenting to receive marketing emails from: . You can revoke your consent to receive emails at any time by using the SafeUnsubscribe® link, found at the bottom of every email. Emails are serviced by Constant Contact

Share this post:

Upcoming Events

03/28/2024

SAF Blue Carpet Event

03/28/2024

2024 Arizona Space Summit

04/03/2024

Low Frequency Updates in Ansys 2024 R1 - Webinar

04/03/2024

Venture Madness Conference Reception + Expo

04/03/2024

Stratasys F3300: Game Changing Throughput - Webinar

04/08/2024

39th Space Symposium

04/09/2024

39th Space Symposium

04/10/2024

Discovery Updates in Ansys 2024 R1 - Webinar

04/10/2024

39th Space Symposium

04/11/2024

39th Space Symposium

04/22/2024

Experience Stratasys Truck Tour: Houston, TX

04/24/2024

Structures Updates in Ansys 2024 R1 (2)

04/24/2024

Experience Stratasys Truck Tour: Houston, TX

05/07/2024

Experience Stratasys Truck Tour: Albuquerque, NM

05/08/2024

Fluent Materials Processing Updates in Ansys 2024 R1 - Webinar

05/09/2024

Experience Stratasys Truck Tour: Los Alamos, NM

05/14/2024

Simulation World 2024

05/15/2024

Simulation World 2024

05/16/2024

Simulation World 2024

05/22/2024

Optics Updates in Ansys 2024 R1 - Webinar

06/12/2024

Connect Updates in Ansys 2024 R1 - Webinar

06/26/2024

Structures Updates in Ansys 2024 R1 (3) - Webinar

06/27/2024

E-Mobility and Clean Energy Summit

07/10/2024

Fluids Updates in Ansys 2024 R1 - Webinar

08/05/2024

2024 CEO Leadership Retreat

10/23/2024

PADT30 | Nerdtoberfest 2024

Search in PADT site

Contact Us

Most of our customers receive their support over the phone or via email. Customers who are close by can also set up a face-to-face appointment with one of our engineers.

For most locations, simply contact us: