Occurrence Properties dialog box

Specifies the values of system occurrence properties and custom occurrence properties in an assembly.

Translate/Rotate About

Specifies the coordinate system that the origin for an occurrence is based upon. For grounded occurrences or occurrences that have no positioning relationships, you can move or rotate a part by specifying a linear or angular offset value in the x, y, or z axis using the Offset From Assembly Origin columns in the list.

If no user-defined coordinate system exists in the assembly, the only option available is Model Space. If user-defined coordinate systems exist, you can select a coordinate system from the list. You can then type a value in the coordinate columns to move or rotate an occurrence relative to the active coordinate system.

Add Custom Occurrence Properties

Adds the custom occurrence properties defined in the file C:\Program Files\UDS\QY CAD 2022\Preferences\CustomOccurrenceProperty.xml to the assembly. These properties can be either local, global, or global+overrides. You can type or select values for these properties, depending on how they were defined. For more information, see Custom occurrence properties in assembly.

Delete Custom Occurrence Properties

Opens the Delete Custom Occurrence Properties dialog box for you to select the check boxes corresponding to the custom occurrence property columns that you want to remove from the table.

Cut

Cuts the current selection and pastes it to the Clipboard.

Copy

Copies the current selection to the Clipboard.

Paste

Inserts the Clipboard contents at the specified insertion point.

Restore

Restores the table to the previous saved configuration. A dialog box is displayed to confirm that you want to discard the changes you have made. The Restore option is not available for changes made to the position of an occurrence.

Print

Displays the Print dialog box so you can print the occurrence properties table to a printer you specify.

Synchronize All

Updates the item number, quantity, and custom occurrence property information with information from Teamcenter. A .CSV file is generated in the Log Files folder that contains details of any issues that occur during synchronization.

System Occurrence Property Columns

The following columns for system occurrence properties are available in the Occurrence Properties dialog box. You can use the Columns command on the shortcut menu to control the column display and order.

Placement Name

Specifies a name for the occurrence. You can use the Rename command on the shortcut menu to rename the assembly occurrence. You can also rename an occurrence by double-clicking an occurrence in the Placement Name column. When you rename an occurrence, the new name is displayed in the Occurrence Properties dialog box and PathFinder. The actual document name on your computer is not changed.

Note:

The Rename command is unavailable when the Document Name Formula is defined as anything other than Filename.

Item Number

The Item Number column is displayed only when the Maintain item numbers check box is selected on the Item Numbers page (QY CAD Options dialog box). The item numbers that appear in the assembly Occurrence Properties dialog box are based upon the item numbering schema selected in the QY CAD Options dialog box. For example, if the Top level only option is selected, then item numbers are not created for subassemblies.

In the Occurrence Properties dialog box, you can select a cell to edit the item number. The item numbers in edited cells are underlined.

If you enter a number that is already used by a different part or subassembly, the text color in the cell turns red and a popup message notifies you that this is a conflict. You can change the item number using the Next Available Number command on the shortcut menu of that cell.

If you change the item numbering schema in the QY CAD Options dialog box, then you can update all item numbers in the Occurrence Properties dialog box using the Reset Item Numbers command on the shortcut menu in this column.

Filename

Displays the name of the file as found on disk.

User-Defined Quantity

Specifies whether a user-defined quantity is specified for a part. When you set the Yes option, you can define a quantity for a part so that it is counted a particular number of times. See Quantity, below, to see how this can be useful.

For non-graphic parts that you have defined custom non-graphic part properties, such as Liters; or As Required, these custom properties are automatically displayed in the cell, and the cell is read-only. For more information, see the help topic, Non-graphic Parts in Assemblies.

Quantity

If User-Defined Quantity column is set to Yes, this is where you enter the number of occurrences. This can be useful if you have parts, such as fasteners, which occur numerous times in an assembly, but you placed only once. For example, if you place one bolt in an assembly, but want the bolt to be counted eight times, you set a user-defined quantity of eight for the bolt. Using this approach can reduce design time and file size.

The quantity value you specify for the part is counted in the Parts List Properties dialog box when you create a drawing of the assembly and place a parts list. The quantity is determined by collecting the unique parts within the assembly and calculating the quantity values assigned to the part. You should use this option if you want a part to be counted a certain number of times in the part list.

You can also set this value to zero, which can be useful for parts in the assembly that are used for reference purposes. They will still be included in a parts list or assembly report, but the quantity value will be zero.

To specify a user-defined quantity of zero for a part, first set the User-Defined Quantity option to Yes. You can then set the Quantity column value to zero.

Note:

Valid values for a user-defined quantity are zero, and any positive whole number greater than one. If you set the Quantity=1, which is the default value, the User-Defined Quantity option will be set back to No when you click OK.

Offset From Assembly Origin Columns

Specifies a relative location for the selected occurrence. You can define a linear or angular offset value in the x, y, or z axis for grounded occurrences or occurrences that have no positioning relationships.

In some design scenarios, it can be useful to edit these values gradually to incrementally move or rotate an occurrence into position. For example, when you are trying to determine the proper position for an occurrence in a cramped location.

In these situations, you can type a value, and then click the Apply button on the dialog box to relocate the occurrence, without dismissing the dialog box. When you determine the final location, you can click the OK button to dismiss the dialog box. You can also use the Enter key to update the positional location of an occurrence without dismissing the dialog box.

These boxes are read-only for occurrences that are positioned using assembly relationships or linked to an assembly sketch.

X

Sets the linear offset value in the x direction.

Y

Sets the linear offset value in the y direction.

Z

Sets the linear offset value in the z direction.

X degrees

Sets the rotational offset value in the x axis.

Y degrees

Sets the rotational offset value in the y axis.

Z degrees

Sets the rotational offset value in the z axis.

Selectable

Controls whether the occurrence can be selected in the graphics window. When you set the Selectable column to No for an occurrence, you can still select it in PathFinder.

Higher Level

Specifies that the occurrence is displayed when the current assembly is used in a higher-level assembly. When set to No, the occurrence is not displayed in higher-level assemblies and is not included in a parts list when the higher-level assembly is placed in a draft document.

A component is set to a construction component by setting the occurrence property column Higher Level to No. However, in the Teamcenter-managed environment, a component is considered a construction when both the Higher Level and Physical Properties occurrence property values are set to No.

For a construction component, the occurrence is only loaded and shown when the assembly that the component resides in is opened. If a higher-level assembly is opened, the assembly component is not loaded nor displayed in Assembly PathFinder in those occurrences.

By not showing the construction components in lower assemblies, this functionality reduces the loading of components when in-place activating and working in the context of a higher-level assembly.

If an assembly containing a construction component is in-place activated, the component occurrence displays as an unloaded component in PathFinder that must be explicitly loaded if the component is needed.

Draft Reference

Specifies that the occurrence is displayed as a reference part in a drawing view. Reference parts in drawing views are displayed using a different style.

Reports / Parts List

Specifies that the occurrence is included in reports generated for the assembly, such as bills of material and parts lists.

Drawing Views

Specifies that the occurrence will be displayed in drawing views created of the assembly in the Draft environment.

Physical Properties

Specifies that the occurrence is included in physical property calculations of the assembly.

Interference Analysis

Specifies that the occurrence is included in interference analysis calculations of the assembly.

Linked To

Displays the name of the assembly to which the part is linked.

Custom Occurrence Property Columns

The following default columns for custom occurrence properties are delivered with QY CAD in the CustomOccurrenceProperty.xml file.

Note:

Your administrator may have removed or renamed these columns or added other custom occurrence property columns. For more information, see Custom occurrence properties in assembly.

Custom occurrence property name	Edit behavior	Definition
BOM ID	Local	Unlike item numbers, which are the same for the same part wherever it occurs, a BOM ID can be different each time the same part or component is placed.
Reference ID	Global	Reference ID or location designator for a component.
Maintenance	Global+Overrides	Maintenance schedule with predefined options: Daily, Weekly, Bi-Weekly, Monthly, Quarterly, or Yearly.
Notes	Global+Overrides	Component placement or assembly instructions.

Shortcut menu commands

Cut

Cuts the current selection and pastes it to the Clipboard.

Copy

Copies the current selection to the Clipboard.

Paste

Inserts the Clipboard contents at the specified insertion point.

Columns...

Displays the Format Columns dialog box so you can set the column display and order options.

By default, all available columns are selected for display in the Occurrence Properties dialog box. You can hide columns, change the column width, and change the column data alignment in the Format Columns dialog box.

You can save these changes for reuse by typing a name in the Saved columns setting box and then clicking the Save button. This writes the settings to a text file, OccurrencePropertyColumns.xml in the QY CAD Preferences folder.

Font...

Displays the Font dialog box so you can select the font, font style, and font size you want.

Find... (or Find and Replace)

Displays the Replace dialog box for you to find and replace text based on whether a cell is read-only or writeable.

Freeze Columns

Keeps columns visible while scrolling horizontally. The command locks in place the selected column and all columns to the left of it. You can resize a column even if it is locked.

Example:

To understand how this works, try locking the first three columns so they stay in place as you scroll to the last column.

1. Right-click the third column and select Freeze Columns. The system locks in place the first three columns.

2. Scroll horizontally to the last column. The first three columns remain in view as you scroll across the document list.

3. To unlock all columns, right-click any column and select Unfreeze Columns.

Unfreeze Columns

Unlocks the columns frozen with the Freeze Columns command. The command unlocks all columns.

Sort

Provides options for sorting the list in Ascending or Descending order.

Expand All

Expands the table to show all parts and subassemblies in the currently selected assembly. If you select this command on the top-level assembly, then the full structure of all of the lower-level assemblies and parts is shown.

Rename

Renames the selection. The selection is renamed within the Occurrence Properties dialog box and PathFinder, but the actual document name on your hard drive is not changed. This command is not available when the Document Name Formula is defined as anything other than Filename.

Reset Default Name

Restores the occurrence name to its default value effectively removing the overridden placement name.

Next Available Number

Renumbers an item in the assembly with the next available item number. Right-click a cell in the Item Number column in the parts list or assembly report to get the next available number.

Note:

This command is available only when the Maintain item numbers check box is selected on the Item Numbers page (QY CAD Options dialog box).

Reset Item Numbers

Regenerates all item numbers based on the settings on the Item Numbers page (QY CAD Options dialog box).

Note:

When you reset item numbers, any edits you have made are reset, too.

Note:

This command is available only when the Maintain item numbers check box is selected on the Item Numbers page in the QY CAD Options dialog box.

Add Override

Enables you to change the value of a property in a lower-level assembly within the context of the active assembly. First select the Add Override command, and then change the value in the cell.

Note:

Overridden values display a tooltip indicating where the override was applied. The cell color also changes according to where in the assembly structure the value was applied.

Cell color	Edit Behavior	Indicates
White	Global or Global+Overrides	If you want to change the value of all occurrences of the property in the active document, simply type a value in the cell. This pushes the change down to the part level and in every assembly the part was used in (unless the other assemblies have an override for that part). If you only want to change the value at the current level, then use the Add Override command.
Light Yellow	Local	Acts like an item number. You can change the value and it applies to lower-level occurrences. Values cannot be overridden. The changes are stored in the active document.
Dark Yellow	Global+Overrides	An override was applied in a lower-level assembly with the Add Override command.
Light Blue	Global+Overrides	An override was applied in the active assembly with the Add Override command.
Gray	Value is read-only from a read-only assembly.	You can override the value in the active assembly.

Remove Override

Removes the override value from the selected property and uses the value defined in the subassembly. You can only remove an override at the same level in the assembly structure where the override was applied originally using the Add Override command.

Example:

If you are editing an upper-level assembly, you cannot use the Remove Override command to change an override done at a lower level in the assembly structure.

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