When you create alternate assemblies in Solid Edge, functionality in other areas of the Solid Edge product is impacted. This impact is typically felt as a restriction on whether certain functionality is available when an assembly has been converted to an alternate assembly. This topic documents this impact in one central location.
You can only create new 3D section views with the Section command when the Apply Edits to All Members option on the Alternate Assemblies tab is set.
You can use adjustable parts in a family of assemblies. You can edit the assembly variable used to control an adjustable part on a per member basis by clearing the Apply Edits to All Members option.
Because there are two distinct types of assembly-based features: assembly features, and assembly-driven part features, they are discussed separately.
You can use assembly features in a family of assemblies. For example, you can use the Delete key to exclude a cutout feature on a per member basis while the Apply Edits to All Members option is cleared (you are working locally). The assembly feature is added to the Excluded Assembly Features list for the member.
Because it is possible to create inter-part links when creating an assembly feature, and alternate assemblies do not allow inter-part links, the inter-part links are deleted when you convert the assembly to an alternate assembly. For example, if you place a positioning dimension or geometric relationship between a profile for an assembly feature and a part edge, an inter-part link is created.
To delete the inter-part links, any dimensions and geometric relationships that were placed to part edges are deleted. You can add the dimensions and relationships to an assembly sketch or an assembly reference plane to constrain the profile.
With assembly-driven part features, the profile geometry (such as lines, arcs, and circles) is copied to the part documents that were modified by the feature. Then the assembly-driven part feature and all dimensions and relationships are deleted from the assembly document. You can open the part documents and add the necessary dimensions and relationships to constrain the profile.
For more information, see the Assembly-based Features Help topic.
You can place new patterns, and delete or modify existing patterns on a per member basis when the Apply Edits to All Members option is cleared (you are working locally). For example, you can use the DELETE key to exclude one bolt in a pattern of bolts when working locally. You can then place a different bolt in that position on the pattern.
When you delete an entire pattern of parts, it is added to the Excluded Pattern Occurrences list on the Alternate Assemblies tab. When you delete a pattern item, it is added to the Excluded Occurrences list.
You can only modify the inputs for a pattern of parts when the Apply Edits to All Members option is set (you are working globally). For example, if an assembly pattern of parts originally included a bolt and nut, you cannot modify the pattern to add a washer to the pattern unless you are working globally.
A Drop Pattern command is available on the shortcut menu when the Apply Edits to All Members option is set (you are working globally). This command allows you to drop an assembly pattern and the parts that were contained in the pattern are now positioned using a ground relationship. Dropping a pattern allows you to place a part formerly contained in the pattern onto the Excluded Occurrences list when working locally.
The Save As Part option on the Interference Options dialog box is not available when the Apply Edits to All Members option is set. If an interfering volume is created as a part while working in the local mode (the Apply Edits to All Members option is cleared), the part is added to the Excluded Occurrence list for the inactive members.
Coordinate systems, layouts and reference planes can be edited only when the Apply Edits to All Members option is set.
Display configurations are available when working with alternate assemblies. The behavior of display configurations based on whether you specify that the alternate assembly is a family of assemblies or an alternate position assembly.
For a family of assemblies, a display configuration is member-specific. In other words, the family of assembly member which is active when you create the display configuration is the only member in which you can use the display configuration later. The Assembly Configuration list on the Select Tool command bar filters the available display configurations automatically.
For alternate position assemblies, display configurations are not member-specific. In other words, you can use any display configuration for any active member. The Assembly Configuration list on the Select Tool command bar displays all the display configurations.
The Disperse command is only available when the Apply Edits to All Members option is set.
You can use fasteners created with the Fastener Systems command in a family of assemblies on a per member basis. You can delete or place fasteners to only the active member by clearing the Apply Edits to All Members option first. The Excluded Fasteners option on the Alternate Assembly tab lists excluded fasteners for an alternate assembly member.
When an alternate assembly member has been placed in a higher level assembly, you cannot in-place activate the alternate assembly. You can use the Open command on the shortcut menu in PathFinder to open the assembly instead.
Because inter-parts links are not allowed in an alternate assembly, when you create the first two members of an alternate assembly that contains inter-part links, a dialog box is displayed to warn you that inter-part links will be deleted. You can use the Inter-Part Manager dialog box to review the inter-part links.
You can only create and edit motors when the Apply Edits to All Members option is set.
If a motor is applied to a part, and that part is deleted when the Apply Edits to All Members option is set, the motor will show as failed in all members.
If a motor is applied to a part, and that part is deleted when the Apply Edits to All Members option is cleared, the motor object is removed from the display in PathFinder. If an excluded part which is a motor is re-included in a member, the motor will be displayed in Assembly Pathfinder.
In the Occurrence Properties editor, the X, Y, and Z translation and rotation occurrence property cell values will be unique for each Family of Assembly member or Alternate Position member. All other values can be set as either unique or global.
The default alternate assembly member is opened when a file is opened using Windows Explorer. When opening a file using the Open File dialog box in Solid Edge, the Assembly Member dialog box is displayed so you can select the assembly member you want.
When creating a part copy using an alternate assembly document, the Assembly Member dialog box is displayed so you can select the assembly member you want.
If you convert an existing assembly to an alternate assembly, and that assembly was used as the basis for a part copy document, the default member is used.
The commands you use to create 3D path segments for tubes, wires, and piping routes are available only when the Apply Edits to All Members option is set. For example, the Path Xpres, Line Segment, Split Segment, and Move Segment commands are available only when the Apply Edits to All Members option is set (you are working globally).
This restriction also applies to the commands you use to dimension 3D path segments, such as SmartDimension. After you create and dimension the 3-D paths, you can clear the Apply Edits to All Members option to define tubes, wires, and piping routes on a per member basis as long as you follow the guidelines for tubes, wires, and pipe routes discussed elsewhere in this document.
You can use the Piping Route command to define a piping route (the pipe and fittings) on a per member basis by clearing the Apply Edits to All Members option. You can also create a piping route that applies to all members by setting the Apply Edits to All Members option. After you create a piping route, the 3-D path segments you used are automatically hidden to prevent you from reusing the selected segments on a different piping path. It is recommended that you do not reuse path segments to create unique piping routes for individual alternate assembly members.
Although you can redisplay the segments using the Show All Paths command, and then reuse them, in some cases, reusing segments can result in a piping route with piping couplings you may not expect.
For example, when you connect one line segment to the midpoint of a second line segment, the second line segment is automatically split at the midpoint. When you define the piping route, a coupling is using to connect the pipe components together where they meet.
If you then try to create a new piping route for a different alternate assembly member that does not include the first segment, a coupling will be added to connect the segments of the line that was split. Typically, a coupling is not wanted in this situation. To avoid this, draw a separate line segment in this type of situation.
Part placement obeys the current setting of the Apply Edits to All Members option. When this option is set, the part is added to all assembly members. When this option is cleared, the part is added to the active member, and the part is added to the Excluded Occurrence list for the other members.
When you place a subassembly that has alternate assembly members defined into a higher level assembly, the Assembly Member dialog box is displayed so you can select the member you want.
This command is available only when the Apply Edits to All Members option is set.
When you use the Reports command to create an assembly report from within the assembly, the report is created for the active member.
When you use the Reports command to create an assembly report from within Windows Explorer, the FOA Member Names dialog box is displayed so you can select the member you want to create the report for.
When an alternate assembly is opened in Revision Manager, the file list is a compilation of all the members contained in the assembly.
When an assembly containing a subassembly that is an alternate assembly is opened in Revision Manager, the subassembly reflects the file set contained in the member that was placed into the higher level assembly.
The Motion command is not available for an alternate assembly. You can use the Save Member As command on the Alternate Assemblies tab to save an alternate assembly member as a normal assembly document. You can then access the Simply Motion environment.
You cannot create a simplified representation of an assembly that is an alternate assembly. If you have already simplified an assembly, then try to convert the assembly to an alternate assembly, a message is displayed to warn you that the simplified assembly representation will be deleted if you continue.
You can use structural frames in a family of assemblies. You can place structural frame components on a per member basis when the Apply Edits to All Members option is cleared (you are working locally)
You can also exclude a complete frame component from an individual family of assembly member when the Apply Edits to All Members option is cleared. You cannot exclude individual part documents that make up a frame component.
The Transfer command is only available when the Apply Edits to All Members option is set.
The Undo command is not available when working with an alternate assembly.
Each tube that is created in an alternate assembly file must be controlled by a single member. The reason for this is that the parts that contain ports that drive the tube path (that in turn drives the tube) can be positioned differently in various members through techniques involving excluded relationships and overridden variables, causing the potential for any one tube part to assume different geometries depending on the active member. The following rules govern XpresRoute behavior:
When a tube part is created, it is created in the context of a single member. The tube part is automatically placed on the exclude list of all other members, but the tube part is hidden in the exclude list so that it cannot be removed from the exclude list of non-driving members.
Occurrence one of a tube created through XpresRoute is always the driven occurrence, and may only exist within the driving member.
All commands which create and manipulate tube path elements are available when working globally (the Apply Edits to All Members option is set).
The Tube command is available only when the Apply Edits to All Members option is cleared (you are working locally).
All tube paths are seen in all members.
If an assembly that contains a tube part that is driven by a path existing in the file, and that assembly is converted into a alternate assembly, the default member becomes the driving member for the tube. The tube is automatically placed on the exclude list and hidden in the second member. If you want to include this tube part in other members, you can place it using the Parts Library tab. This places an occurrence that is not a child and therefore will not trigger an update of itself when the Update All command is run. This assures that a tube part is not updated unless the member in which it was created is currently active, and consequently, each tube part is driven only in context of a single member.
When a new member is created while the active member contains a tube that is driven by that member, the driven tube is placed on the exclude list of the new member and hidden on the list so that it cannot be taken off the list. The effect will be that the tube part does not appear in the new member.
In version 17, if you convert an assembly to an alternate assembly after you create tube paths and tubes in XpresRoute, the links to the tubes will be broken. If you convert the assembly to an alternate assembly before you create tube paths or tubes, the links to the tubes you create later will function properly.