# What is the difference between bonded contact region and fixed joint

• 3K Views
• Last Post 4 weeks ago
• Topic Is Solved
TimFethke posted this 11 July 2018

Hi,

I need to connect different parts for a project, and I noticed that there are 2 options. One is using the bonded contact region and one is using the fixed joint. Both can be used for surfaces so I am wondering what the exact difference is. I've done a test by connecting two parts and then calculating some modes (as I need to do modal analysis) and compared the connection methods to see if the result would be the same, but it is not.

I did find this through Ansys help:

Bonded: This is the default configuration and applies to all contact regions (surfaces, solids, lines, faces, edges). If contact regions are bonded, then no sliding or separation between faces or edges is allowed. Think of the region as glued. This type of contact allows for a linear solution since the contact length/area will not change during the application of the load. If contact is determined on the mathematical model, any gaps will be closed and any initial penetration will be ignored. [Not supported for Rigid Dynamics. Fixed joint can be used instead.]

The last line indicates that both can be used for similar purpose but that bonded contact region is not supported for Rigid Dynamics.

Can someone explain to me what the exact difference is?

peteroznewman posted this 11 July 2018

Hi Tim,

For solid bodies that share a face and need to be "glued" together, there are ways to achieve that connection that is neither bonded contact nor fixed joint. You can use "Shared Topology" and have the elements on each side of the coincident faces share nodes. The benefit of this is a smaller model. You can get the same effect with Node Merge if each face has mesh controls to force the nodes to line up. Shared topology does this automatically.

Imagine two tubes that are placed end-to-end and the annular faces need to be connected. Bonded contact puts elements between individual nodes over the whole face and creates a very localized connection. Say the other end of one tube is a fixed support and the far end of the other tube has a lateral load so the tube is a cantilevered beam and some bending occurs. In the annular ring, the force is transmitted locally all around the face. Depending on the contact formulation, you can get some penetration of nodes into the target surface. That doesn't happen with the shared topology method.

A fixed joint creates a point at the centroid of the faces, and builds a spider of elements out to all the nodes on each face.  All the forces and moments go through that one point.  That is one of the benefits of using a joint, you can easily extract those quantities from your model. But there is no local node-to-node forces transferred around the annular face. The force has to go down the spider, though the point and back out on another spider to get to the other side.

There is a danger when creating joints in Mechanical. Never use duplicate on a joint in the Outline to make another joint to use elsewhere in the model because the point that was created for the first joint is used in the new joint, rather that being updated to the location of the new faces. That means the invisible spiders that are created can go from one of the new faces, all the way over to a point on the other side of your model through a point, and then all the way back. You can imagine that a small tension on the tubes of the new joint will have a result that includes a HUGE moment, and a small force, when it should have a zero moment. This can cause the solver to have convergence difficulties. This kind of mistake cannot happen with bonded contact.

When there is a significant gap between the faces that need to be "glued together", the fixed joint will always work by simply choosing the two faces, but bonded contact may not create any contact elements and the bodies will not be glued. The corrective action is to type in a Pinball radius to make sure that the contact elements are created. You should always insert the Contact Tool and Generate Initial Contact Status before you start the Solver. You don't need to to that for Fixed Joints.

Regards,
Peter

TimFethke posted this 11 July 2018

Wow thanks Peter! This explanation is really elaborate. Did you find this from documentation or from experience with these connection methods? Escpecialy the explanation about the invisible spiders creating false moments sounds like an anecdote .

Tim

• Liked by
peteroznewman posted this 11 July 2018

Painful experience Tim; I still get burned occasionally : )

I once used a joint to represent a long lead screw between two faces that were far apart. Got burned on that because of huge moments. The right way to have a simplified connection like that is a Spring element (could also use a Link180 element).  A spring has two coordinate systems, one on each end, so there are no moments!

Regards,
Peter

• Liked by
jj77 posted this 4 weeks ago

As this is fluid related, move your post to the fluid dynamics section , as more people can help you there.