Similar to fully defined sketches for parts, assemblies in SOLIDWORKS should be fully constrained wherever practical. A well-constrained assembly is more stable, easier to edit, and less prone to unexpected motion or mate errors. At the same time, some degrees of freedom must remain for mechanisms that need to move.

This tutorial explains:

• How SOLIDWORKS shows fixed, floating, and under-defined components
• How to unfix (float) a component
• How to find components that are not fully constrained
• When it is acceptable to leave motion in an assembly
• How to use Lock Rotation and configurations to handle both “fully constrained” and “flexible” states

This example uses the same gear assembly as in “How to mate gears in SolidWorks?”. The concepts apply to any assembly, not just gears.

Fixed, floating, and under-defined components in SOLIDWORKS

Each rigid component in a 3D assembly starts with six degrees of freedom (three translational and three rotational). Mates and/or a fixed status remove those freedoms until the component is fully constrained.

In the FeatureManager design tree, SOLIDWORKS uses small prefixes to show the state of each component:

• (f) – the component is fixed in all six degrees of freedom and cannot be moved by dragging it.
• (-) – the component is floating and under-defined; at least one degree of freedom is still open and it can move when dragged.
• No prefix – the component is floating but fully defined by mates (no remaining free degrees of freedom).

By default, the first component inserted into an assembly is fixed at the assembly origin and appears with an (f) icon.

Best practice: fix one component, mate everything else

For robust assemblies, a common guideline is:

• Fix one key component (for example, the base plate or housing).
• Mate all other components to that part and/or to stable references (assembly planes, axes, origins), rather than fixing multiple components.

Fixing multiple components arbitrarily can over-constrain the assembly, making it harder to edit and more likely to show mate conflicts during rebuilds, particularly in larger assemblies.

How to unfix (float) a component

If a component is fixed and you want to reposition or fully mate it, you need to convert it from Fixed to Float.

1. In the FeatureManager design tree, locate the component marked with (f) before its name.
2. Right-click the component.
3. Select Float.

The (f) icon disappears, and the component becomes floating. You can now drag it or add mates to constrain it.

In newer versions of SOLIDWORKS, the Fix/Float option can also be applied per configuration (This configuration, All configurations, or Specify configurations), which is useful when you want a part fixed in one configuration but floating in another.

Identifying under-defined components in an assembly

As with sketches, it is strongly recommended that assemblies be fully defined unless there is a deliberate need for motion. Under-defined components are one of the most frequent causes of unexpected movement, especially when you drag one part and others slide or spin relative to it.

There are two quick ways to identify under-defined components:

1. Check the FeatureManager symbols

• Expand the assembly tree and look for components or subassemblies that show (-) before the name. These items are not fully constrained.
• Fully constrained components (other than the fixed one) will not show a (-) icon and will not move relative to the rest of the assembly when dragged.

2. Drag-test the model in the graphics area

When you drag a component in the graphics area, SOLIDWORKS allows it to move within its remaining degrees of freedom.

• If the entire assembly moves rigidly as one unit, all internal relationships are fully constrained; you are just moving the whole assembly in space.
• If one component slides, spins, or shifts relative to the others as you drag, it is still under-defined and needs additional mates (unless that motion is intentional).

To better understand the remaining degrees of freedom, you can also:

• Right-click the component and choose Move with Triad to move it along specific axes and see where motion is still allowed.
• Right-click the component and use View Mates (context menu) to review exactly which references are constraining it.

When is it acceptable to leave the assembly under-defined?

In practice, there are two common exceptions where leaving some degrees of freedom open is both intentional and desirable.

1. Rotation that does not affect fit, form, or function

Some hardware and fittings only need their position fully constrained; their rotational orientation is irrelevant to function. Examples include:

• Bolts, screws, and dowel pins in clearance holes
• Hydraulic fittings where the body can swivel without affecting performance
• Cylindrical spacers or bushings

In these cases, it is acceptable for the component to remain under-defined by a single rotational degree of freedom. However, you may still want to lock the rotation (see next section) so that models and drawings look cleaner and assembly performance is more predictable, especially in large assemblies.

2. Mechanisms that require motion (e.g., gears)

For mechanisms such as gears, hinges, linkages, and hydraulic cylinders, motion is part of the design intent. To simulate motion correctly:

• At least one degree of freedom must remain open somewhere in the mechanism.
• The motion should be controlled using appropriate mates (e.g., Gear mates, Hinge mates, Limit angle mates, etc.), rather than by leaving random components completely under-defined.

In the gear example used for this tutorial, only the rotation of the gears should be unconstrained; all axes and positions should be fully defined.

Using “Lock Rotation” to constrain unwanted spin

When a component is constrained with a Concentric mate, it usually still has the freedom to spin around its axis. For many components, that rotation is not needed and just contributes to under-definition.

Instead of adding extra mates just to stop rotation, SOLIDWORKS provides a Lock Rotation option for concentric mates.

Lock rotation for a single concentric mate

1. In the FeatureManager design tree, expand the Mates folder.
2. Right-click the relevant Concentric mate and select Edit Feature.
3. Check Lock Rotation and click OK.

The mate icon changes to indicate locked rotation, and the component can no longer spin freely about that axis. Note that if the component is already fully defined by other mates, locking rotation may have no effect.

Lock rotation for all concentric mates in the assembly

When you have many fasteners or similar components, you can lock all applicable concentric mates at once:

1. In the FeatureManager, right-click the Mates folder.
2. Select Lock Concentric Rotation.

This command locks rotation on free concentric mates that still allow spin, which is particularly useful in larger assemblies with many fasteners.

Automatically locking rotation for Toolbox fasteners

For Toolbox hardware (bolts, nuts, etc.), you can enable automatic lock rotation when concentric mates are created:

1. Go to Tools > Options > System Options > Hole Wizard/Toolbox.
2. Under Toolbox Mates, enable Lock rotation of new concentric mates to Toolbox components.

With this option enabled, new Toolbox components you insert and mate concentrically will have their rotation locked automatically, reducing the number of under-defined degrees of freedom in your assembly.

Using configurations for “Fully constrained” vs “Flexible rotation”

Often, you need both:

• A fully constrained configuration for drawings, simulation, and general use where everything is locked down.
• A flexible configuration where specific motions (like gear rotation) are allowed for demonstration, checks, or motion studies.

Configurations are an efficient way to switch between these states without rebuilding mates from scratch.

Step 1 – Create two configurations

1. Go to the ConfigurationManager tab in the FeatureManager.
2. Rename the existing Default configuration to Fully Constrained.
3. Right-click Fully Constrained and choose Add Derived Configuration.
4. Name the new derived configuration Flexible rotation.

The derived configuration will initially inherit all mates and settings from Fully Constrained.

Step 2 – Fully constrain the mechanism (gears)

First, ensure that the mechanism can be fully defined. For gears, this typically means:

• Gear centers are fully constrained relative to the housing (e.g., concentric to shafts, shafts fixed or fully mated to the base).
• Teeth engagement is set up using a Gear mate or equivalent relationships so that gear motion is correctly coupled.
• Any redundant or conflicting mates have been removed.

This tutorial assumes you already have working gear mates from “How to mate gears in SolidWorks?”.

Step 3 – Configure mates using “Configure Feature”

Now you will choose which mates control rotation and configure them differently between Fully Constrained and Flexible rotation.

1. In the FeatureManager, expand the Mates folder.
2. Ctrl + click the mates that you want to configure (for example, the mates that lock rotation or fix the gear positions).
3. Right-click any of the selected mates and choose Configure Feature.
4. In the configuration table that appears:
   • Set mates to Unsuppressed in the Fully Constrained configuration.
   • Set those same mates to Suppressed in the Flexible rotation configuration.

By suppressing only the mates that control rotation, you allow gears (or other components) to rotate in the flexible configuration while keeping all other positional constraints intact.

Step 4 – Use each configuration appropriately

• Use the Fully Constrained configuration for:
  • Manufacturing drawings
  • Static FEA or interference checks
  • General day-to-day design work where motion is not needed
• Use the Flexible rotation configuration when:
  • Demonstrating motion to stakeholders
  • Running motion studies (basic or with add-ins)
  • Checking clearances at different positions via dragging or collision/physical dynamics.

Quick workflow checklist

• Fix only one reference component; mate everything else to it or to reference geometry.
• Unfix components by right-clicking and choosing Float before adding mates.
• Scan the FeatureManager for (-) icons and use drag tests to reveal remaining degrees of freedom.
• Use Lock Rotation on concentric mates where rotation is not required (especially on fasteners and fittings).
• Leave motion only where it is intentional and controlled by suitable mechanical or advanced mates.
• Create Fully Constrained and Flexible rotation configurations to switch between locked and movable states of your mechanism.

Following these practices will give you assemblies that are stable, predictable, and easier to maintain, while still allowing realistic motion where it matters.