Tie constraints are a powerful and effective tool for connecting different regions in Abaqus FEA model, ensuring they perform as a single, bonded structure during the simulation. They work by allowing the surfaces to move together as a single entity irrespective of their mesh and material differences.
These types of constraints are often used to
- Model welded and bonded joints in an assembly.
- Joining dissimilar meshes in assembly, for example in mesh refinement cases.
- Joining dissimilar material types in an assembly.
- Establishing connections between dissimilar part types like shells and solids or shells and beams or beams and solids.
- Attaching parts that share a common physical boundary in an assembly to prevent relative motion.
How Are Tie Constraints Defined?
Tie constraints are defined between two surfaces belonging to the same part or multiple parts. So, the first step in defining the constraint is to select the two surfaces forming the interface. The first interacting surface is defined to be the primary surface, and the other interacting surface is defined as the secondary surface. These surfaces can be element based, node based or analytical.
The rotational and translational degrees of freedom are the same for both sides of the interface which makes the connected nodes behave like they are glued together.
Tie Constraint Discretization Methods
The discretization process refers to how the tie constraints are numerically enforced between primary and secondary surfaces during the simulation by the software. In Abaqus, the calculation for the constraints is performed automatically using Lagrange multipliers or penalty method or augmented Lagrange method. There are two methods to enforce the tie constraints: Node to surface and surface to surface. Let’s briefly discuss about them in this section.
Node To Surface
This is the default method for defining the tie constraints. Each of the secondary nodes is projected onto the primary surface based on the initial configuration. The nearest distance from the primary surface is calculated for each of the secondary nodes. Constraint is applied to ensure that the secondary node follows the motion of that nearest primary surface node through the simulation.
Surface To Surface
This is a more robust method, where instead of only projecting individual secondary nodes onto the primary surface, the secondary surface as a whole is constrained to the primary surface. This approach generates an averaged constraint between the two surfaces. The entire secondary surface is integrated to compute the constraint, and the average behavior of the secondary surface is matched with the primary surface. Stress noise at the connection interfaces can be avoided by using this formulation because of the averaging method used here.
Below is the table summarizing the differences and applications of the two discretization techniques.
Things To Lookout For
Adjust Secondary Surface Initial Position Option
The initial positions of the secondary nodes may sometimes be misaligned with the primary surface. If it is not corrected, it can cause improper deformation, excessive constraints, stress concentrations, or inaccurate results. To prevent this, Abaqus includes options to adjust the positions of the secondary nodes, ensuring proper application of the tie constraint. This will be a strain free adjustment.
If this option is not selected, the secondary nodes remain in place, potentially leading to initial gaps or overclosures between the primary and secondary surfaces. This can be useful if maintaining a pre-existing gap or offset is needed, or if the user prefers for the secondary nodes to interact without any position adjustments.
Adjust Position Tolerance
Using computed default position tolerance ensures that the interface nodes are tied only where the primary and secondary surfaces are close in the initial state. But if we want a particular set of nodes within a specified distance from the primary surface to be tied, position tolerance has to be used. This desired tolerance has to be manually entered for ‘specify distance’ option. This option is very helpful when the default tolerance is either too large or too small for a particular application.
Final Thoughts
Hopefully this article has provided insights into tie constraints and their modeling approach. Of course, care must be taken to avoid improper use of tie constraints in a FEA model which could lead to error in the simulation results.
If you have questions regarding tie constraints in your model or FEA in general, get in touch with us today!
