Solid Edge

Solid Edge Introduces Systems Library

28 Feb, 2003 By: J. Fred White

We are seeing Solid Edge users creating extremely large assemblies, some topping 100,000 parts. One of several new innovations in Solid Edge to help manage and speed such design efforts is the Systems Library.

When building an assembly, you often need to use the same group of parts more than once or create the same set of feature modifications in the mating parts to facilitate placement. This is typical of both universal standard-components and company-specific standard-components. For example, it's common to have a bracket that mounts hardware onto a frame or plate within your assembly, as shown in Figure 1. In order to mount the bracket into the assembly, you may need hole, slot, or boss features in the mating frame or plate along with bolts, washers, and nuts.

Figure 1. In order to mount a bracket into an assembly, you may need hole, slot, or boss features in the mating frame or plate along with bolts, washers, and nuts, as shown here. In Solid Edge Version 14, you can now create or use existing standard assembly components and placement features to define a Systems Library.

With the introduction of Systems Library in Solid Edge Version 14, you can now create or use existing standard assembly components and placement features to define a Systems Library document. More than a typical sub-assembly, Systems Library provides the ability to define and store complex "systems" of parts to be "snapped" into place, while automatically applying assembly relationships and building supporting features.

Systems Library can both add and remove material, doing the operation as a "system" with a many-to-many approach. For example, you might need to bolt Part A to Parts B and C, while riveting Part D to parts F and G and adding some strengthening gussets to Part Z.

The Systems Library can handle this type of complex interaction between the system and the target assembly--a huge time-saver that dramatically speeds up your assembly design by capturing and storing known design parameters and rules for reuse.

The basic steps for defining a Systems Library is as follows.

  • Create or use an existing assembly that contains the standard components.
  • Create inter-part features in mating components to capture (optional).
  • Create a Systems Library document from the assembly.
  • Reuse the Systems Library document in other assemblies.

Creating a Systems Library Document

When you click the Create Systems Library button, a SmartStep ribbon bar guides you through the steps required to create the systems library document.

Select the standard assembly components you want to capture. This will automatically capture relationships to the selected components for reuse. The captured relationships are categorized as internal (to the selected components) and external (to mating components).

Select the features you want to capture (optional). This is automatic when identifying mating components that have inter-part relationships to the selected components.

View the captured relationships.

Define the document names and location.

Creating Systems Library SmartStep Ribbon Bar

Select Components Step defines the parts and subassemblies you want in the Systems Library document. This is the set of components you want to reuse in other assemblies. Only parts and subassemblies in the top-level assembly can be included in a Systems Library document. For example, if the active and open assembly is named Assembly1.asm, and it contains subassembly A and B, and within subassembly A is part C, you can include subassembly B and all its parts in a Systems Library document, but you cannot include only part C in a Systems Library document by itself unless you open subassembly B.

Captured Features Step defines the features you want in the Systems Library document. Only features that were created using the inter-part copy workflow are valid for inclusion. If you don't want to include any features in the Systems Library document, click the Next button.

Captured Relationships Step displays the Capture Relationships dialog box so you can review the captured relationships. The ones displayed will be used to place the Systems Library document into other assemblies. While the internal relationships among the selected components are not shown, they will come into the new assembly at placement time. During placement, you can choose to skip captured relationships.

Create Group displays the Create Systems Library Documents dialog box so you can define the assembly document, the feature-part documents, the new file location, and your chosen template.

Now that we've covered the basics of creating a Systems Library document, let's explore placement options into an assembly. A systems document is placed by dragging the systems document from the Parts Library tab and dropping it into the assembly window. When you drop the systems document in the assembly window, a SmartStep ribbon bar guides you through placing the systems document.

The SmartStep Ribbon Bar

Place Part Step specifies the placement of the Systems Library document. You can use the input dialog box to define the target part and target-part element. A dialog is also available to show what captured relationships are being used to position the group of components, as well as an option to skip a given relationship.

Paste Features Step pastes features from the Systems Library document into the selected components. This is done by selecting the mating parts in the assembly and face to define the reference plane for the features to be pasted onto.

Stop stops the place operation and leaves the Systems Library document in the assembly. If you have not fully positioned the part or subassembly documents, you can select them and then use the Edit Definition button on the ribbon bar to complete the positioning process later.

Skip bypasses the current relationship or feature.

Occurrence Properties accesses the Occurrence Properties dialog box for the part to set items such as Quantity, Include In Bill Of Material And/Or Parts List, Display In Drawings, Include In Mass Property Calculations, and so on.

Construction Display specifies which construction elements you want displayed or hidden. Displaying or hiding construction elements can make it easier to position the part.

Offset Value sets the distance the part is offset from the adjacent part in the assembly. This option is available when you are using a fixed offset. You can type a positive or negative number.

Flip repositions the part to the opposite side of the face by changing the mate relationship to a planar align relationship.


The assembly tools in Solid Edge allow you to build and manage complex assemblies from the top down or the bottom up. They are designed to reduce the time you spend creating 2D layouts, ensuring accurate part-fitting, "teaching" parts to automatically snap into position, and handling your Systems Libraries.