Assemble command bar Options dialog box

The Options dialog box associated with the Assemble command bar is used specify which assembly workflows and part placement options to use when forming assembly relationships. It is opened by selecting the options button on the Assemble Command bar. The options on this dialog are also associated with the command bars for the other assembly relationships. See Understanding Assembly relationships for more information about different workflows, Assemble command for more command information, and Show list of assembly relationships for a list of the other assembly relationships that share the settings on this dialog box.

Use FlashFit as the Default Placement Method

When checked, the FlashFit assembly relationship becomes the default assembly relationship. By default, this option is checked.

When unchecked, the Mate assembly relationship is the default assembly relationship.

The FlashFit workflow reduces the steps required to position parts using Mate, Planar Align, and Axial Align relationships when compared to the traditional workflow. For more information about different workflows, see Understanding Assembly relationships. See About the FlashFit relationship and About the Mate relationship for more information about these assembly relationships.

Use Reduced Steps When Placing Parts

When checked, the number of steps required to position a part using relationships is reduced. This is called the Reduced Steps workflow. Only the target part face and placement part face have to be selected to form a relationship.

When unchecked, the target part and target face as well as the placement part and placement face all have to be selected. For more information about different workflows, see Understanding Assembly relationships.

To use a reference plane or coordinate system on the target part to position the placement part, they must be displayed first when this option is set. For more information, see the Construction Display Options on the Assembly page of the QY CAD Options dialog box.

Automatically Capture Fit When Placing Parts

When checked, the relationships used to position a part are automatically captured to reduce the number steps required to place the part again. This is effective when repetitively placing the same part such as fasteners or parts that are used several times in an assembly. The user must have write access to the placement part to preserve the relationship. To manually record the relationships of a part when this option is not set, highlight the placed part and select the Capture Fit command (Home tab→Assemble group→Capture Fit). For more information, see Capture Fit command.

Use Distance Between Faces as Default Offset

When checked, the current distance between faces is used as the default offset value when using the Edit Definition command. This can be useful when editing the position of a part, and the Offset type is changed from Floating to Fixed, or when adding a new relationship to an existing part. This option is not available when using the Use FlashFit as the Default Placement Method is checked. When this option is set, and the position of a part where a fixed offset value is available is edited, the actual parallel distance between the two parts is displayed in the Offset Value box. If this is the desired value, click the OK button to complete the placement process. If a different value desired, enter the value then click OK.

Place As Adjustable

When checked, this option is used to specify that the placed subassembly is considered an adjustable assembly. This allows relationships to be applied to a part in the subassembly rather than the subassembly itself. The relationship can only be placed to a part in the subassembly that is not fully constrained. For more information, see Adjustable assemblies. This option can only be set when a subassembly is being placed.

Disperse After Placement

When checked, the parts associated with a placed subassembly are individually added to the assembly rather than a subassembly. This option can only be checked when a subassembly is being placed.

This option is typically used when placing a subassembly that contains a component that is part of an alternate components group.

For more information about working with alternate components, see Define Alternate Components.

Match click points on the parts when creating first assembly relationship (pre-ST8 behavior)

This option determines the part placement behavior when creating assembly relationships.

When checked, the pre-ST8 relationship behavior is used. When applying the relationship, the placement part moves as much as practical to match the click point on the surface of the target part. As much as possible, the target part remains stationary. Due to this behavior, sometimes the placement part moves when it is not required. This often occurs in imported assemblies where the parts are mostly in place but do not have some relationships applied.

When unchecked, the placed part only moves the minimum amount to accomplish the relationship. Selecting this option can improve placement performance. This is the default setting.

This feature can also be set using Component Placement Options section of the Assembly page in the QY CAD Options dialog box. For more information, see Assembly page (QY CAD Options dialog box).

FlashFit

Locate the Following Element Types

Check the individual element types to be recognized when forming a FlashFit assembly relationships. This determines which types of relationships FlashFit recognizes and applies. For example, if all the element types except Planar faces are unchecked, the only relationships FlashFit applies are Planar Align and Mate relationships. With the Planar faces, Cylindrical faces, and Circular edges options checked, FlashFit can recognize and apply Planar Align, Mate, and Axial Align relationships.  For more information about the individual assembly relationships, see Show list of assembly relationships.

Dimensions

Show All Dimensions

When checked, relationship dimensions are displayed when a part is selected and the Edit Definition button is clicked. This action opens the Assemble command bar to allow the assembly relationships associated with the part to be edited.

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