Solid Edge contains commands that allow you to change the structure of an existing assembly.
The Transfer command transfers parts and subassemblies from one assembly to another. You can transfer these parts and subassemblies to any level of the assembly that can be seen from the top level assembly that is open. You can also use the Create New Subassembly dialog box to create a new subassembly for the transferred files. To access the Create New Subassembly dialog box, on the Transfer to Assembly Level dialog box, click the New Subassembly button.
The Disperse command transfers the parts in a subassembly to the next highest subassembly and deletes the reference to the subassembly. The command disperses only the top-level occurrence of a subassembly. For example, if a subassembly exists as an occurrence within the assembly being dispersed, the subassembly remains unchanged, but is moved up to the next higher assembly level.
To change the order of the files within an assembly, you can drag and drop parts in the PathFinder.
You can use the Transfer command to transfer assembly files, parts containing inter-part relationships, tube parts, and pattern parts. It is important that you understand how Solid Edge handles these transfers so you can avoid possible problems.
When transferring parts, it is very important that you have write access to all of the part and assembly files involved in the transfer.
Solid Edge handles relationships during transfers just like it would if you deleted a part from one subassembly and added it to another. It attempts to re-establish each positioning relationship exactly like it was before the transfer, with reference to the same reference part. If the reference part remains in the assembly tree below its new location, the relationship should be successfully re-established. If the reference part is not below the transferred part's new location, it will not be converted into a non-positioning relationship and the relationship is removed. You will not receive warnings for affected relationships during transfers, so you should be very careful when transferring parts with relationships. You might choose to add positioning relationships to any occurrence that becomes underconstrained after its transfer.
If you transfer a part that is a parent of an inter-part relationship, the link is broken, but not deleted. Inter-part Manager will show the inter-part link as broken, just as if the parent part was deleted from the assembly. You will not receive a warning when the parent part is deleted. You must understand the relationship dependencies within your assembly so that you can avoid breaking links when you transfer parts. You will be warned if you transfer a part that is inter-part child. If you continue with the transfer, the link will be broken and automatically deleted by the command.
Pasted variable links will remain intact during transfer as long as both the parent and child remain anywhere in the assembly.
If you transfer a tube part containing the port that defines a path, the link will be deleted and you will not receive a warning message. If you transfer a part containing a port to a level above the assembly containing the tube path, the tube path becomes non-associative to the part and you will not receive a warning message.
If you transfer a part containing a feature pattern that drives the assembly pattern, the pattern disappears and you not receive a warning message.
Solid Edge allows you to create a new subassembly for parts you want to transfer. The New Subassembly button on the Transfer to Assembly Level dialog box accesses the Create New Subassembly dialog box. You can use this dialog box to specify a template, file name and location for the new database. You can also use the dialog box to define the position of the transferred parts in the new subassembly.
You have two options when defining the part position.
Position First Selected Part at Origin and Others Relative to It
Maintain Current Offsets From Assembly Origin
The first option specifies that if the new subassembly is opened outside of the parent assembly, the parts will be positioned relative to the global reference planes so that when you fit the view, the parts will not be remote from the reference planes. This options provides results similar to creating a new assembly with existing parts. For example, when you create a new assembly and drag the first part in from Parts Library, it is grounded at the origin of the assembly file. The subassembly is then positioned as a whole within the upper level assembly.
The second option specifies that you want to position everything relative to a single global origin. After the new subassembly is created, if you open the subassembly outside of the parent assembly and the fit the view, the parts might be remotely located from the global reference planes.
If you transfer a part from one subassembly to another and there are multiple occurrences of one or both of the subassemblies within the assembly structure, it is very likely that the instances of the transferred occurrence will change. For example, if a part in subassembly A, which occurs only once, is transferred into subassembly B that occurs five times, the effect is that four instances of the transferred occurrence is added. Likewise, if there are more occurrences of the source subassembly than there are of the target subassembly, the number of occurrences instead could be reduced.
There are several things you need to consider when transferring parts. It is important that you understand how Solid Edge handles these situations so you get the desired results from your transfer.
The occurrence number of a occurrence after its transfer into the target assembly is the next consecutive number available for the file name that is transferred. If you transfer more than one of the same file name occurrences at the same time, the number that is assigned to each occurrence in the target assembly is determined by the order in which they are numbered in the source assembly.
Existing display configurations become invalid as parts are removed or added during part transfer.
If you transfer a part into a target assembly that contains a style that is assigned to the part in the source assembly, you must reapply the style after the transfer. If the target assembly does not contain the style assigned to the part in the source assembly, the part is assigned the Aluminum style.
Explode configurations become invalid as parts are removed or added during part transfer. In the Draft environment, drawing views will go out-of-date when parts are removed or added from the configuration.
Groups are not maintained during part transfer. Solid Edge handles the transfer of groups the same as if the part was manually deleted from or added to the source assembly.
Since 3D section views contain a list of parts that are cut, they are affected during transfer. Solid Edge handles the transfer of 3D section views the same as if the part was manually deleted from or added to the source assembly.
Sensors are not maintained during part transfer. Solid Edge handles the transfer of sensors the same as if the part was manually deleted from or added to the source assembly.
Motion joints are not maintained during part transfer. Solid Edge handles the transfer of motion joints the same as if the part was manually deleted from or added to the source assembly.
Physical Properties are not maintained during part transfer. Solid Edge handles the transfer of physical properties the same as if the part was manually deleted from or added to the source assembly.
You can use the Disperse command to disperse a subassembly by reassigning the parts to the next highest subassembly and removing the reference to the existing subassembly. The command will disperse only the top-level occurrence of a subassembly. For example, if a subassembly exists as an occurrence within the assembly being dispersed, the subassembly remains unchanged, but is moved up to the next higher assembly level.
The command does not modify the dispersed subassembly on the disk. The part occurrences are copied to the next higher level and the reference to the subassembly is deleted. When you save the top-level assembly, since it is no longer in the assembly structure, the dispersed subassembly occurrence is not saved.
If the subassembly being dispersed contains a pattern, the parts of the pattern are placed at the proper location in the next higher level and a ground constraint is placed on each of the parts. The parts will not be grouped in the PathFinder under a pattern node, but will be ordered the same in the next higher assembly.
If you disperse a subassembly containing a tube part, the tube part and other parts are transferred to the next higher level, but the dispersed subassembly on the disk is not affected. Therefore, the tube part is still associative to the path when you open the subassembly stored on the disk.