top of page

Connector Elements In Abaqus - What Are They And How Should We Use Them?

Connector elements are one of my favorite element types in Abaqus. They are extremely versatile, and they can also save time in postprocessing if you set them up correctly during the model build. In this blog, we will go through how to make connector elements and the different connection types available.


Why Use Connector Elements?


There are countless modeling problems in FEA involving two or more parts connected together. Sometimes, the connection is simple and a simple tie constraint or RBE2 can do the job. But what if you’re trying to model a shock absorber with stopping mechanisms, or if you’re trying to model hundreds of slotted pins, where physically modeling the pin would be computationally expensive? Problems such as these and many more can be solved by using connector elements!


If you’re already familiar with multi-point constraints (MPCs), connector elements are very similar in that they both impose kinematic constraints on the model. However, unlike MPCs, connector elements do not eliminate degrees of freedom. Instead, kinematic constraints are enforced with Lagrange multipliers. This is less efficient, but in return, they are able to return a force and moment output as well as provide other functionalities, such as loading and damping – just to name a few.


Building Connectors In Abaqus CAE


First, we have to create the connector section. In the interaction module, create a connector section, then you can select the connection category and connection type. Finally, you can add connector behaviors. We’ll go through the connection behaviors and types later in this blog.

 
Connector Elements in Abaqus

Connector Elements in Abaqus
 

After making the connector section, we can now use the connector builder to make the connector element. First, select the two reference points you want to connect. The connector builder will create the reference point for you if you select a geometric point or a datum point instead. Additionally, you can also choose to connect to ground instead of selecting a second point. This option can be used to make grounded springs or dampers. After selecting the two points, you can select the connector section and the orientation of the connector.

 
Connector Elements in Abaqus
 

For my example, I let the connector builder create a coordinate system as an axis between the two points:

 
Connector Elements in Abaqus
 

We can always change the connector section and orientation in the connector section assignment manager.

 
Connector Elements in Abaqus
 

You can also assign the connector section to a pre-existing wire instead of using the connector builder, but I think using the connector builder is much more convenient.


The Connector Type Library


Abaqus offers many different connection types that can allow connector behavior or kinematically constrain different components of relative motion. These are summarized in the table below:


Connector Elements in Abaqus

Cells in green show a component of relative motion available for defining the connector behavior, connector motion, or connector loads.


Cells in red show a kinematically constrained component of relative motion.


Cells in white are neither available for defining connector behavior/motion/loads nor constrained kinematically.


In the sections below we’ll go into the connection type diagrams for each connection type and when to use each of them. This will be very high level; consult the Abaqus documentation for the full details on each connection type. You can also view the connection type diagrams in Abaqus CAE by clicking on the lightbulb symbol in the connector section creation page.


Accelerometer


This connection type is only available in Abaqus Explicit. This is used to measure relative position, velocity, and acceleration between two points.

Connector Elements in Abaqus

Align


This connection type constrains all rotations between two points.

Connector Elements in Abaqus

Axial


This connection type is used where the relative displacement is along the line separating the two nodes. This is useful for connections such as springs or dampers.

Connector Elements in Abaqus

Beam


This connection type kinematically constrains all components of relative motion. This is a versatile connection type – one application is for quick modeling of bolts. If you’re only looking to pull bolt forces without considering preload, a beam connector can do the trick!

Connector Elements in Abaqus

 

Bushing


This connection type has all components of relative motion available. It is a great way to approximate deformable connections where physical tests aren’t readily available, such as automobile control arms.

Connector Elements in Abaqus

Cardan


This connection provides a rotational connection between two nodes where the relative rotation is parameterized by Cardan angles (yaw-pitch-roll).

Connector Elements in Abaqus

Cartesian


This connection provides a connection between two nodes where the change in position is measured in three local connection directions. This works great for orthotropic connections.

Connector Elements in Abaqus

Constant Velocity


This connection type fixes the angle between two joints.

Connector Elements in Abaqus

CV Joint


This connection type is the same as the constant velocity connector, but it also constrains all translations. Like its name implies, its best application is to model CV joints on vehicles.

Connector Elements in Abaqus

Cylindrical


This connection type allows torsion and axial translations but constrains all other components of relative motion. This is a great way to model pins.

Connector Elements in Abaqus

Euler


This connection type provides a rotational connection between two nodes where the relative rotation is parameterized by Euler angles (precession-nutation-spin).

Connector Elements in Abaqus

Flexion-Torsion


This connection type models the bending and twisting of a cylindrical coupling between two shafts. Instead of representing three successive rotations, the flexion, torsion, and sweep angles are measured separately.

Connector Elements in Abaqus

Flow-Converter


This connection type converts the relative rotation about a user-specified axis between the two nodes of the connector into material flow degree of freedom at the second node of the connector element. Belt or cable material is considered to be wrapped around an axle or a drum, and material can be spooled either into or out of the connector element. It can be used in applications such as seat belts and cable drums in winch-like devices.

Connector Elements in Abaqus

Hinge


This connection type only allows rotation along its axis. It can be used in applications such as door hinges, axles, and drawbridges.

Connector Elements in Abaqus

Join


This connection type makes the position of two nodes the same. It can be used for modeling ball and socket joints.

Connector Elements in Abaqus

Link


This connection type maintains a constant distance between two nodes. It can be used for modeling coupling rods and taut lift slings/chains (assuming there’s no compression).

Connector Elements in Abaqus

Planar


This connection type provides a local two-dimensional system in a three-dimensional analysis – combining the revolute and slide-plane connection types. It be used for modeling sliding constraints.

Connector Elements in Abaqus

Projection Cartesian


This connection type is very similar to cartesian. However, instead of using a coordinate system that follows node a, projection cartesian uses a coordinate system that follows the systems at both nodes a and b.

Connector Elements in Abaqus

Projection Flexion-Torsion


This connection type is very similar to flexion-torsion. However, two component flexion angles are reported instead of one flexion angle and one sweep angle.

Connector Elements in Abaqus

Radial-Thrust


This connection type provides a connection between two nodes where the response differs in the radial and cylindrical axis directions. It be used in applications such as cylindrical bearings where the radial and thrust responses are different.

Connector Elements in Abaqus

Retractor


This connection type combines the join and flow-converter connection types. It can be used in applications such as seat belts and cable drums in winch-like devices.

Connector Elements in Abaqus

Revolute


This connection type provides a connection between two nodes where the rotations are constrained about two local directions and free about a shared axis. This provides the rotational part of the hinge and cylindrical connection types, but it doesn’t have much use on its own.

Connector Elements in Abaqus

Rotation


This connection type provides a rotational connection between two nodes where the relative rotation is parameterized by the rotation vector. If defining connector behavior, Cardan or Euler is typically preferred; however, Rotation works well in conjunction with prescribed connector motion.

Connector Elements in Abaqus

Rotation-Accelerometer


This connection type is only available in Abaqus Explicit. This is used to measure relative angular position, velocity, and acceleration between two points.

Connector Elements in Abaqus

Slide-Plane


This connection type keeps node b on a plane defined by the orientation of node a and the initial position of node b. This is a good way to model the feet of structures not fastened to the floor and where friction is low.

Connector Elements in Abaqus

Slipring


This connection type provides a connection between two nodes that models material flow and stretching between two points of a belt system. This is a great way to model seat belts, pulleys, and taut cable systems.

Connector Elements in Abaqus

Slot


This connection type only allows translation about one direction. This is great for any slotted connections.

Connector Elements in Abaqus

Translator


This connection type constraints two nodes in all directions and rotations except along the line connecting them. This connection type works well for modeling railed connections such as drawer slides.

Connector Elements in Abaqus

U Joint


This connection type constraints all translations and fixes rotation about one local direction. As its name implies, its best application is to model U joints on vehicles.

Connector Elements in Abaqus

Universal


This connection type fixes rotations about one local direction and frees the other two. This can be used whenever you need to constrain a single rotation.

Connector Elements in Abaqus

Weld


This connection type kinematically constrains all components of relative motion. It’s very similar to the beam connector. Use this when the two nodes have the same position – otherwise, use the beam connector.

Connector Elements in Abaqus

Connector Behaviors


You can assign connector behaviors to connection types that have available components of relative motion. The types of connector behaviors that can be assigned are listed below:


Elasticity: This behavior allows spring-like elastic behavior to be set for the available components of relative motion.


Damping: This behavior allows damping behavior to be set for the available components of relative motion.


Friction: This behavior allows frictional effects to be defined for the available components of relative motion. For example, if using a connector to model a pin in a slot, there can be some friction at the interface between the pin and the slot.


Plasticity: This behavior allows plastic behavior to be set for the available components of relative motion. This must be used in conjunction with the elasticity behavior option.


Damage: This behavior allows the force response in the connector to degrade if relative forces or motions in a connection exceed critical values. You can specify the criteria for damage initiation as well as a damage evolution law that specifies how the damage evolves. This should be used in conjunction with the elasticity behavior and possibly also the plasticity behavior if the damage initiation behavior is plastic motion based.


Stop: This behavior sets upper and lower limits for the positions in the directions of the components of relative motion. For example, shock absorbers in vehicles have a certain length where they bottom out, so the stop behavior can be used to set that bottom out value.


Lock: This behavior allows the connector to lock if any one of a list of criteria is met. You can set whether all or some components of relative motion become locked once the locking criterion is met. An example of this is the velocity-locking criteria in a seat belt. Other locking criteria that can be set include force, moment, and position.


Failure: This behavior allows the connector to break if a relative motion component, force, or moment becomes too large. All components of relative motion will be released upon meeting the failure criterion.


Reference Length: This can set the translational or angular position at which constitutive forces and moments are zero for the available components of relative motion. This should be used in conjunction with either the elasticity or friction behaviors when the reference position is different than the initial position in the model.


Integration: This behavior is only available in Abaqus Explicit. By default, connector constitutive behavior is integrated implicitly, which does not affect the stability or time incrementation of the analysis in any way. However, there may be a small improvement in computational performance by using explicit time integration for “soft” springs modeled with connectors.


Connector Actuation


In addition to the behaviors described above, you can apply forces and displacements to connector elements with available components of relative motion. Connector forces and moments can be applied from the loads menu, and connector displacements and velocities can be applied from the boundary conditions menu.

 
Connector Elements in Abaqus
Connector Elements in Abaqus
 

Outputting Connector Element Results


In Abaqus CAE, you can request connector element output in the step module. Change the domain to a set containing the connector elements or connector wires and then connector output variables will become available in the field/history output request box. Available output variables include forces, moments, displacements, and rotations. 

 
Connector Elements in Abaqus

Connector Elements in Abaqus
 

Note that for history outputs and *_LOCAL field outputs, the results will follow the intrinsic coordinate system of the connector. For field outputs not ending in _LOCAL, the results will follow the orientation of the first node of the connector. Neither of these will necessarily line up with the global coordinate system of the model.

 

Here’s one area where the connector element really shines. If you add *EL PRINT to your input deck, you can output connector element history outputs right to the .dat file. Imagine being able to copy all the bolt forces in your model into a table without even having to open the .odb!


Connector Elements in Abaqus

Putting It All Together


 
Connector Elements in Abaqus
 

Here we have a model of a small tensegrity table consisting of two wooden pieces connected with five pretensioned cables, giving an illusion that the table is floating. The four corner cables help stabilize the table while the main loading goes through the center cable. All the cables are modeled using axial connectors (available in CU1 only) with elastic properties and a reference length. The elastic properties are set such that if the connector ever goes below its reference length (AKA if the cables go into compression) they will no longer react axial force. The connector on the center cable combines the axial and Cardan connectors, but no behaviors are set on the rotational components of relative motion. A weld connector (constrained in all components of relative motion) is used to measure the loads transferred from the bottom of the table to the constrained floor. All the connector elements are attached to contact patches using RBE3s.

 
Connector Elements in Abaqus
Connector Elements in Abaqus
Connector Elements in Abaqus
 

I have loaded the table with downwards gravity in the -Y direction as well as a 30N load in the -Y direction distributed on the entire tabletop, a connector force of -30N on one of the corner cables, and 5N loads in the X and -Y directions on the corner of the table.

Connector Elements in Abaqus

I’d probably design the wood pieces differently if I were to build this table in real life. But more importantly for this example, how about what the connectors are doing? I don’t even have to check the .odb for that since I printed the connector output to the .dat file!

 
Connector Elements in Abaqus
Connector Elements in Abaqus

 

Connector Elements in Abaqus
Connector Elements in Abaqus

Some observations regarding these results:


  • Note that since the .dat file is printing a history output, the results follow the intrinsic coordinate system of the connector. This does not line up with the global coordinate system of the model.

  • Elements 2 and 5 are clearly in compression based on the connector displacements. Elements 3 and 4 are still in tension since they did not go under the reference length.

  • Force and moment output is available for all constrained components of motion, while displacement and rotation output is available for all available components of motion. Since element 1 is an axial + Cardan connector, we can see rotation outputs for it even though it does not react moments.

  • The connector force output on element 2 is reacting the applied connector force we applied in the loading.

  • Since element 5 is in compression, it has no stiffness and therefore cannot react any force.

  • The connector force output for element 6 is exactly what we’d expect based on the applied load (30 + 5 + 0.37 (weight of the wood pieces) in connector X, which corresponds to global Y; 5 in connector Z, which corresponds to global X).

Final Thoughts


Connector elements are some of the most versatile and powerful elements you can use when building models in Abaqus. Hopefully, this blog has given you everything you need to start utilizing connector elements in your own models!


Of course, mastering the use of connector elements takes practice and experience. Luckily, there’s nothing our engineering team loves doing more than building large FEA models with hundreds of connector elements! Reach out to us today!

Komentarze


bottom of page