When two or more bodies are brought from CAD into the FEA software, the FEA program is able to interpret that there’s multiple bodies but makes no presumption about what the relationship of these bodies are as far as relative motion is concerned.

Are the bodies completely joined to one another (such as with a full penetration weld), are they able to slide relative to one another, or maybe they are restricted from sliding – but readily able to pull apart? Defining these relationships, how the parts may move (or not be able to move) relative to one another, is what the various contact types allow us to define.

*Inventor Nastran contact generation options via ribbon*

Contact generation options

Automatic
- Contact pairings automatically identified, and conditions assigned.
- Default contact condition is bonded.
- Contacts can be modified.
- Works well for simple assemblies with mostly welded connections.
Manual
- Assigning contacts manually enables greater control over the contacting surface pairs.
- User must manually choose faces (or edges).
- Allows multiple faces to be chosen together as Primary or Secondary entities.
- Works well for complex assemblies.
Solver
- Contacts generated at runtime wherever surfaces are within the set distance.
- Doesn’t allow user to view or modify the generated sets.

Contact types

There are several contact types available to represent how your model interacts in the physical world. You should aim to apply what is needed to represent actual conditions as best as possible (similar to constraining a model).

There will be some variability, depending on the specific finite element analysis package you are utilizing, but you should generally expect to find contact types that will fit your structural analysis. Below, note what Inventor Nastran includes and when you might utilize each type:

Separation
- This type of contact is a surface-to-surface contact. Both relative sliding and opening are allowed.
- The example in the figure below shows three blocks. The bottom block is pushed up and a separation contact is used between the touching surfaces.
  
  Separation contact
Bonded
- This type of contact is used to bond surfaces together. Surface to edge contact is also permitted. Once bonded, the surfaces move together as though they are welded.
- The translational degrees of freedom are linked together.
- It can be useful in cases where touching surfaces on different parts have dissimilar meshes and do not undergo relative displacement. In other words, the surfaces are treated to be bonded together.
- The bonded contact response between the beams is shown in the figure below. It moves together as shown in the image.
  
  Bonded contact
Sliding/No separation
- With this type of contact, the element will act similarly to a welded contact element in tension and compression but will slide in-plane.
- This is useful for pinned connections.
- Friction is ignored for this contact type, so contact data should not include friction settings.
- Slide contact can be used in linear and nonlinear solutions.
  
  Sliding contact
Separation/No sliding
- With this type of contact, the element will act similarly to a general contact element in tension and compression but will not permit sliding in-plane.
- Essentially, this applies infinite friction between the surfaces.
- Can only be applied in Nonlinear Analysis. If the analysis type is not nonlinear, the contact type will default to welded.
  
  Separation / No sliding

Offset bonded
- The offset weld setting is intended for welded connections with significant separation between contact surfaces.
- Links together Translational AND Rotational degrees of freedom.
- Useful for shell-to-shell and shell-to-solid welded connections.
  
  Offset bonded
Shrink fit/Sliding
- This contact type has initial interference between the contacting parts and sliding is permitted.
Shrink fit/No sliding
- This contact type is like a Separation/No Sliding contact but with initial interference between the contacting parts. Use this type when the intensity of fit and friction are great enough to prevent relative motion (sliding) between the contacting parts.
- Both types of Shrink Fit contact are for nonlinear analysis. Interference can be specified automatically (CAD-based) or manually, by entering the penetration surface offset value.
- Realistic interference is recommended, to prevent excessive penetrations that can cause the solver to fail to converge, or converge with large penetrations.
- Shrink Fit contacts should have at least two subcases defined, and the first subcase should have no defined loads. Loads can be defined for other subcases. This setup allows Nastran to solve for interference until an equilibrium is achieved with minimal contact penetrations.

Contact settings

The settings for manual and automatic contact sets can be modified. The dialog box allows users to change the participating entities, contact type, stiffness, friction, and more.

Primary entity
- Field allows you to select the primary surface(s).
- Only surface selections are allowed.
- Blue colored faces indicate that they are primary entities.
Secondary entity
- Field allows you to select secondary surface(s).
- Edges can also be selected.
- Pink colored faces indicate that they are secondary entities.
Penetration type
- Only applicable for manual contacts.
- Unsymmetric – only checks for penetration from secondary nodes into primary.
- Symmetric – checks for penetration both ways between primary and secondary nodes.
Stiffness factor
- Controls stiffness scaling of the contact.
- Higher the value – the less the penetration.
- Default of 1.0 usually works well.
Coefficient of friction
- Coefficient of static friction. Only applies to separation contacts.
Penetration surface offset
- Defines numerical thickness offset value for instances such as shell to shell or solid to shell contact.
Max activation distance
- Specifies the distance that contact elements should be activated.
- Helps to limit the number of contact elements and decreases solution solve time.
- When checked and no value is specified, the default solver distance will be used. This can be too large.
- When unchecked, the auto function will be used (solver).

Amount of contact

Solution times

Contact allows analysts to more precisely model the interactions between parts. However, keep in mind that adding contact to a model will increase solution time. We will examine two reasons for this.

Defining contact (which must be done when there is an assembly), even if bonded contact is used, will add to solution time. This is because elements are built to create the relationship between the part mating surfaces.

The two models shown both have a 2"x2"x1" base with a 1" cube on top. In the upper image, the geometry was constructed as a single body, so no contact was required. In the bottom image, the model was made as an assembly, so bonded contact was set. Compare the differences in element count and solution CPU time.

*As a single body, this model has 31,000 nodes, 20,994 elements, and the model analysis total CPU time is 8.9 seconds.*

As a two-part assembly using bonded contact, the model started with 32,532 nodes and 21,524 elements. The program adds 1,027 contact segments for a total of 22,551 elements. CPU time increased 27% to 11.3 seconds.

Another reason that an analysis can take more time with contact is due to the iterative nature of some types of contact. The program may need to go through many iterations to determine whether the parts are attempting to come closer together, pull apart, or slide. Then, either allow that motion or prevent it based on the setting of the contact parameters.

The two models shown both have the same geometry and assemblies that utilized contact. In the upper image, the contact was set to bonded. In the lower image, the contact was set to separation, so the solution uses more time iterating to determine if and how there is movement and then arrive at a statically stable solution. Compare the differences in element count and solution CPU time. For a rather similar element count, the separation contact model requires a good deal more solution time.

*As a two-part assembly using bonded contact, the model started with 32,532 nodes and 21,524 elements. The program adds 1,027 contact segments for a total of 22,551 elements. CPU time is 11.3 seconds.*

As a two-part assembly using separation (and symmetric) contact, the model started with 32,532 nodes and 21,524 elements. The program adds 4,165 contact segments for a total of 25,689 elements. CPU time increases to 50.1 seconds.

Applying contacts in an analysis will lengthen the solution time by some amount. This is not reason to not utilize contact, but rather, information to know to allow ahead of time for longer solution times and for consideration of where and when to utilize contact.

Reducing amount of contact

Given the illustration of these simple block examples, it is possible to see how the effects can be even more extreme with a large assembly of many parts. If a goal is to try and keep solution time to a minimum, there are a few different techniques – you might be able to utilize one or more.

Review the geometry and consider how the model should behave under loading. If there are interfaces of bodies that will experience no relative motion in the physical world, consider using bonded contact there and only utilizing a more computationally expensive type of contact (like separation) in the regions where it will impact the outcome of the results.
In more extreme cases, when you have an assembly that is all (or mostly) the same material and will all (or mostly) be bonded, then when you have adjacent parts that meets those two conditions, it is possible to union or Boolean those bodies into a single component to eliminate the need to define contact between them. You could, as a hypothetical case, convert a 20-part assembly to one joined body plus the three or four parts it needs some sort of separation or sliding contact with. Take advantage of symmetry as well to reduce the element count by half or more.

Thinking through the model before diving into the analysis, such that contact is utilized only when and where required, can help save significant solution time.

Use element types and meshing in FEA - Quiz