Using the Gear command bar

The Gear command bar options are used to define how one part moves in relation to another. It supports rotational-rotational, rotational-linear, and linear-linear type movements. For more information, see About the Gear relationship.

The following image shows the Gear relationships using the horizontal toolbar form of the user interface. The features displayed for the vertical docking window interface form are similar. You can change the version that is displayed using the Command User Interface options on the Helpers tab in the QY CAD Options dialog box. For more information, see Helpers tab (QY CAD Options dialog box).

The Gear command bar:

has the same features as the Assemble command bar:

when a Gear relationship type is selected. For more information, see Assemble command bar.

The command bars have the following features:

Command Bar Icon

The icon displayed is determined by how the command was accessed. The Gear icon is displayed if the Gear command is selected from the ribbon (Home tab→Assemble group→Gear) when defining or modifying a relationship for parts that are already in the assembly workspace. The Assemble icon is displayed after dragging a new part into the assembly workspace and a Gear relationship type is selected.

Occurrence Properties

Opens the Occurrence Properties dialog box. For more information, see the Occurrence Properties command. This option is only available after you select a part.

Construction Display

This option is only displayed when a part is selected. When visible, this option opens the Construction Display dialog box that is used to show or hide the selected reference elements for the selected part. The selected reference element can then be used to form the relationship. The reference items include:

show/hide coordinate systems
show/hide reference planes
show/hide sketches
show/hide references axes
show/hide construction surfaces
show/hide construction curves
use designed or simplified part

Relationship List

On the Gear command bar, the identifier for the next relationship to be formed is displayed. This value is for reference only and cannot be changed. On the Assemble command bar, the identifier for the next relationship to be formed is also displayed but any previously defined relationships are displayed in the list and can be selected. This allows previously defined relationships to be modified directly from the Assemble command bar.

Relationship Type

On the Gear command bar, this option is locked and cannot be changed. On the Assemble command bar, the type of relation to be formed can be selected from the list. Changing the relationship type from Gear to some other relationship type also changes the options that appear on the command bar. For more information, see Show list of assembly relationships.

Command Bar Options

Opens the Assemble command bar Options dialog box.

Placement Part

Use this option to select the placement part. This button is active when adding a relationship to a part that already exists in the assembly, or when placing a subassembly into the assembly. This button is inactive when placing a new part in an assembly.

Placement Part—Element

Use this option to select the placement part element based on the relationship type being defined. For a rotational element, select a circular edge or axis. For a linear movement, select an axis of movement or a linear edge.

Target Part

Use this option to select the target part.

Target Part—Element

OK

Applies the assembly relationship using the input you defined.

Relationship Type

Use this option to specify the type of gear relationship being formed. For more information, see Using the Gear command:

Rotation-Rotation: Specifies that both components will revolve.
Rotation-Linear: Specifies that one component will revolve and the other component will move linearly.
Linear-Linear: Specifies that both components will move linearly.

Gear Value Type

This option only becomes active if the gear relationship type is set to Rotation-Rotation. It is then used to identify how the rotational movement of the first element is to be applied to the rotational movement of the second element. Two options are available:

Ratio: Use this option to define how the number of rotations on the first part affects the number of rotations of the second part.
Teeth: Use this option to define the rotation movements of both part based on the number of teeth on each part.

Value Fields (2)

These fields are used to define the amount of movement in the two parts based on the type of relationship being defined. The value entered into the first field is for the first part and the value entered into the second field is for the second part. The values are based on the type of relationship being formed.

Rotation-Rotation: Specifies the movements of both parts based on the selected gear value type: Ratio or Teeth. The Ratio option is used to enter how the number of full or partial rotations of the first part effect the entered number of full or partial rotations of the second part. For the Teeth option, simply enter the number of gear teeth on the first and second parts in the appropriate fields.
Rotation-Linear: Specifies the movements of both parts based on how the entered number of full or partial rotations of the first part affect the entered amount of linear motion on the second part.
Linear-Linear: Specifies the movements of both parts based on how the entered amount of linear motion of the first part affects the entered amount of linear motion on the second part.

Flip

This option only becomes available after you select the target part element. It is used to ensure that the direction of movement of the second part correctly corresponds to the movement of the first part. If not initially correct, select this option to reverse the direction of the second part. This relationship is relational. It may not necessarily correspond with the eventual direction of movement.

About the Gear relationship

Position two parts by matching their coordinate systems