Node connectivity at an interface

[naqib_mashrur4YFQQ]

I was wondering how bonded contact actually works, and how node connectivity is actually maintained ... at minute 50:17 to 52:53, they show that node connectivity can be maintained by sketching a line and then creating a split at the interface. But is this the best practice to ensure node connectivity in Inventor Nastran? To me it seems a little cumbersome for a more complicated model with many such interfaces. To me it seems like the intended workflow would be to use the Auto Bonded Contact feature in the GUI. Is my assumption correct?

[John_Holtz · Accepted solution]

Hi @naqib_mashrur4YFQQ 

That video is not showing bonded contact, at least not at the times 50:17 to 52.53. The video is discussing a different technique of connecting pieces together by matching the mesh. In Inventor Nastran, that method is referred to as Continuous Meshing. In other words, the elements use the same node numbers, so the elements are connected together. All transmission of loads goes through the nodes in one way or another. (The chapters for the video do not list contact, so I think the contact that you are referring to, bonded, separation, sliding, and so on, are not discussed in the video.)

In general, continuous meshing is not reliable for solid models. 

• IF the edges are the same length and location, and IF the mesh size is the same on both bodies, then it is likely that the same number of nodes and elements will be generated along the edge even though the mesh is technically random.
• IF by chance the nodes on the two parts are within the tolerance, they will be merged together. (The tolerance is under "Mesh > Mesh Settings > Setting > Tolerance".)
• If the mesh size is different, then it is unlikely that the random mesh will generate nodes within the tolerance distance of each other. In this case, the parts are not connected together. (Perhaps the nodes at the corners will be merged since those points are at the same location.)
• I noticed the software in the video (version 2016?) does not have the label that the current software has for Continuous Meshing: "(for solids only merges nodes on perimeter)". What this implies is that all the nodes on the interior face are not merged together. At best, the mesh matching would create a fillet weld around the perimeter.

The contacts that you are asking about (bonded, separation, sliding, and so on) and created by the three command "Contacts > Auto", "Contacts > Manual", and "Contacts > Solver", use a different approach that works with an unmatched mesh; the nodes do not need to be at the same location. The solver generates contact elements from the nodes on the secondary surface to the element faces on the primary surface. (If you could see these elements, it would look something like spokes going from the nodes to the corners of the faces.) The load on one part is transferred from the secondary node to the corner nodes on the primary faces through the contact. (So again, the load is transferred through the nodes. 🙂)

You can also think of the contact elements as springs. In the case of bonded contact, they transmit forces in all three directions, tension and compression. For separation contact, the springs only transmit a force in the normal direction, in compression, and only if the secondary node is touching the primary element face. The stiffness of the contact springs is calculated by the solver based on the material properties and mesh size. The user can control the relative contact stiffness by changing the default stiffness from 1.0 to a different value. This is necessary in some cases when a weak material is in contact with a stiff material. (Generally, the stiffness needs to be much smaller: 0.1 or 0.01.) Just for completeness, the contact stiffness needs to be 0.2 for an explicit dynamics analysis.

The advantages of contact are:

• you do not need to split the surfaces to try to get the Continuous Meshing to match.
• the choice of bonded, sliding, separation, and so on.
• One of the results is the contact force which is desired in many cases. (Technically, the internal forces calculated by the solver could be used for the continuous mesh to get the same load transmission, but Inventor does not display that result.)

The disadvantages of contact are:

• It is more of an approximation than what a matched mesh provides.
• In some situations, you need to be aware of how the Maximum Activation Distance affects how many contact elements are created, meaning too many elements or too few.
• Since the contact area is between a node and entire elements, the contact footprint is spread out beyond the contact area by up to one element. If the footprint needed to be more precise, the primary surface would need to be split to limit the footprint.

Here are some references:

1. Section 6) Contact in the PDF document attached to my forum post Suggested Reading - Tips and Tricks.
2. Understanding maximum activation distance and contact type in a Simulation
3. Difference between Maximum Activation Distance and Penetration Surface Offset in Nastran contact def...

John

[lauri_barnhart]

Hello, @naqib_mashrur4YFQQ,

Did the information provided by @John_Holtz help you and answer your question?

If yes, please click on the "Accept Solution" button on the post(s) that solved your problem. This will assist other community users in finding and benefiting from this information.

If not, please do not hesitate to give an update in this thread so all community members receive an update on the progression of your question, and can suggest next steps that may be helpful for you to achieve what you're looking for.

All the best,

Lauri | Community Manager

[naqib_mashrur4YFQQ]

John's solution did solve my problem. Thank you for reminding me to hit accept solution.