Tie vs Shell-To-Solid Coupling In Abaqus – What Is The Difference? And Which Should You Use?

One of the biggest strengths of Abaqus is its large library of available element types, meaning that you can optimize analyses for both accuracy and efficiency. It is well known that, when we’re modeling very thin structures, such as the wall of a pressure vessel, it is beneficial to utilize shell elements rather than solids. We don’t have to worry about the number of solid elements through the thickness of the wall since we can select as many integration points as we want in the shell construction.


But what happens when we come across a section of the thin wall that needs relatively fine, through-the-thickness solid mesh to properly resolve the stresses and strains that are relevant to the analysis being performed? Is it possible for us to add a patch of 3D elements into our shell model? Well, the answer is yes. But not so fast… How do we join them together? Read on to find out!


Options To Join Shell Elements To Solid Elements


Firstly, we should note that there are two main options we have here to join the two regions together. They are ‘tie constraints’ and ‘shell-to-solid couplings’. But what is the difference?


Tie constraints


Tie constraints are reasonably universal in FEA codes, although they are often given other names - like ‘glue’. These are used to make translational and rotational bonds between nodes in a structural model (other degrees of freedom when different physics are being analyzed). Nodes are tied together where surfaces are very close to each other and, in the case of shell edges, that is typically only along a line in the center of the thickness being represented (regardless of shell thickness – important!). Where better to go than the Abaqus manual to find a good schematic?

Tie Abaqus

Shell-to-Solid Coupling


Shell-to-solid couplings, on the other hand, take account of the shell’s thickness, even when it is joined to the solid along its edge. Instead of simply tying local nodes together, Abaqus assembles constraints that couple the displacement and rotation of each shell node to the average displacement and rotation of the solid surface in the vicinity of the shell node. This is an important distinction, and we’ll see why in our example problem below.


The shell-to-solid coupling works by enforcing automatic creation of an internal set of distributing couplings between the shell edge and the opposing solid surface. In fact, each shell node has its own distributing coupling, with the solid nodes in the vicinity acting as the coupling nodes. This allows the distribution of forces and moments acting at the shell node to be translated to forces (no rotational degrees of freedom in the nodes of solid elements) on the related set of coupling surface nodes in a self-equilibrating manner.

Shell-to-Solid Coupling Abaqus

Which Interaction Should You Choose?


But which should we choose for the below analysis example? Let’s find out!


Here we have a simple model of a plate in tension. As you can see, there is a join between shell and solid elements halfway along the length of the 60x20x5mm steel plate, and we’ll be applying a tensile load of 100N at one end. Let’s see what happens…

Shell-to-Solid Coupling Abaqus

As you can see on the left in the image below, in the tied version, the continuity of stress is very poor. That is because the tie is doing exactly what it says on the tin – it is ‘tying’ the translation of the nodes that are closest together. Meanwhile, the nodes outside the reach of the tie in the 3D elements are free to move however they want. That leads to the artificial stress concentrations that you see in the nodes that lie in the middle of the thickness below.


On the right, the shell-to-solid-coupling generates very good stress and deflection continuity between the shell and solid elements, owing to its distributing nature. Of course, this is much more preferable where solid elements are patched into predominantly shell mesh.

Tie vs Shell-to-Solid Coupling Abaqus

Let’s review:

  • When you’re trying to maintain thickness continuity in a plate or thin-walled structure, then it is appropriate to use shell-to-solid couplings

  • When you’re attaching shells to solids for any other reason then ties are appropriate (although be careful with the lack of rotational degrees of freedom in the nodes of solid elements)

Final thoughts


Shell-to-solid couplings might be something that you’ve heard of before in Abaqus, but perhaps you weren’t exactly sure what they were or when it is appropriate to use them? Hopefully this short post has clued you in on their function and, just maybe, you’ll start to see where you might need them more often moving forward?


For more Abaqus help and general FEA reading, check out the rest of our blog posts. And if you’re interested in talking simulation with us, don’t hesitate to reach out to the team!

558 views

Recent Posts

See All