Ghost objects show up when a missing object—referenced by another Pro/ENGINEER part, assembly or drawing—is not available within the Workspace when you do a save or an import against the part, assembly or drawing. These virtual files contain metadata but no physical file and can never be checked into Commonspace. A check-in conflict caused by a ghost object can never be overwritten.

How do I know if I have one?

A ghost object displays with a special icon in Workspace (Fig. 1). Ghost objects cause a check-in error for the object to which it is related. Since you cannot overwrite this check-in conflict, you must replace a ghost object with a real object, resolve the references, or remove the reference before you can check in successfully.

Figure 1

How do I clean it up?

While you can sometimes delete the ghost object from the Workspace, this is not recommended because the ghost tends to reappear at each subsequent check-out and Pro/ENGINEER save. True elimination of ghost objects can require several steps. Here’s a logical process of investigation and resolution to make your ghost hunt as easy as possible.

1. Try to update the ghost object(s) in the Workspace.

• Highlight the ghost object(s) and select Objects, Update Ghost Objects.
• If an object with the same name exists in Commonspace, an Update dialog box appears (Fig. 2).

Figure 2

• To update and check the objects out to your Workspace, select Update to replace the ghost object with the actual file from Commonspace. (If you want to investigate the object in Commonspace, select Do Not Update or Cancel.)
• If you select Update and an error dialog appears (Fig. 3), select OK.

Figure 3

• Locate the corresponding objects in Commonspace and check them out to the Workspace.

2. If (1) doesn’t work, try to find out what file or files the ghost object relates to.

• Highlight the ghost object in the Workspace and select Reports, Relationship, Report.
• If this does not bring results, select Report, Where Used.
• If either report displays information, note the file name and relationship type.
• In Pro/ENGINEER, open the file listed in the report window to determine whether the file and relationship are still required.
• Several circumstances can cause a ghost object to appear in the Workspace—an Interchange group that has been deleted or renamed, a dependency to a Pro/ENGINEER layout, an assembly suppressed component, or a feature that was created in an assembly with a reference to another object. It can therefore take some detective work to track down and resolve the faulty files.

For example, It may be necessary to find the missing file in the case of an import of new data. References to a suppressed component in an assembly may, if no longer needed, be deleted. Interchange group references may need to be re-created or removed. If the ghost object is related to a layout, it could be un-declared from the related part or assembly if no longer needed. If the layout reference is still needed, the missing object must be found or re-created.

3. If (2) doesn’t work, check in any drawings in the Workspace marked as Modified one by one.

• If the ghost object is related to a drawing, a check-in error will appear.
• Interrogate the error message window to discover the name of the object at fault.
• Because of an issue with Pro/ENGINEER (TPI 114763, www.ptc.com/cs/tpi/114763.htm), the ghost object may only be cleaned up using hidden configuration file options. If you exhaust all other options, the TPI walks through the process of starting Pro/ENGINEER linked to the Workspace that contains the ghost object(s), adding the hidden configuration file options ‘cleanup_drawing_dependencies’ and ‘cleanup_layout_dependencies’ with a value of ‘yes’ to the current session through the Utilities, Options menu drop-downs.
• Open the damaged drawing file. If the ghost is related to the issue defined in TPI 114763, a dialog box usually appears with a message about cleaning up dependencies. Accept the clean-up option and Save the drawing.
• View the Workspace and select the Refresh icon.
• Select the drawing file and pick the check-in icon or select Object, Check In. If the ghost object was successfully cleaned up and references removed from the drawing, the drawing will not error on check-in. If there is still an error, verify the error message to make sure it is not the same ghost object issue still haunting the process.

If you follow all of these paths to disappearance and the ghost object just won’t go away, visit the PTC Technical Support area at www.ptc.com.

Karen Dougherty is a senior design technician in MCAD & MCAD PDM Support at Honeywell. She can be reached by e-mail at karen.dougherty@honeywell.com.