Friday, December 18, 2015

Insert Assembly Copy

Solid Edge has had the command Insert Part Copy for a long time.  Insert Part Copy functions by allowing you to insert the geometric body of an existing Part, Sheet Metal or Assembly file into another Part or Sheet Metal file.  The geometric body can be optionally inserted associatively as an Ordered feature, or non-associatively in Synchronous mode and supports several options such as making the body a construction, scaling, or mirroring the inserted body.


A similar command was made available in ST5 and later versions called Insert Assembly Copy.  Insert Assembly Copy functions by allowing you to insert an existing Assembly file into another Assembly file.  Unlike Insert Part Copy which inserts a body, Insert Assembly Copy inserts the actual assembly structure under an Assembly Copy node in Pathfinder.  The resulting Assembly Copy is associative to the original such that any changes or additions to the original will be reflected in the copy.   You can of course freeze or break the link of the Assembly Copy which results in the Assembly Copy node becoming non-associative to the original.



The Insert Assembly Copy command has several options which are:
  • Add new components on update (If this is unchecked, adding new parts in the copied from assembly does not update the Assembly Copy with the new parts)
  • Include assembly features
  • Mirror about (uses the same wizard as the Mirror Components command)
  • Exclude Components



Uses for the Insert Assembly Copy include:
  • Creating a mirrored assembly (Left Hand vs. Right Hand)
  • Inserting a base 80% assembly into multiple assembly files and adding optional parts in each to produce 100% configured assemblies.
  • ???  If you can think of any other novel uses, please comment them on this article.

The Assembly Copy function is also used by:
  • The Mirror Components command in Assembly to associatively mirror assembly structure/components.
  • The Multi-Body Publish command to build an assembly of the published bodies for downstream use.

Wednesday, December 09, 2015

Solid Edge Wins Big at the “Slots”!



Solid Edge ST5 introduced a new “Slot” feature to make creating slots much more efficient than past methods.  You may have overlooked this feature in ST5 and future versions due to its nested button location on the ribbon, so I thought I would reintroduce this useful feature.

Prior to the new Slot feature, one would have to use the Cutout command and then create a sketch of the slot’s profile by hand or by using the Symmetric Offset sketch command.  If the slot needed to be counter bored for a head of a fastener, then additional sketching and features were needed.  The new Slot command simplifies this process greatly.

The Slot command is located under the Hole fly-out menu.  It is available as both an Ordered and Synchronous feature.

Invoking the command produces the Slot Command Bar that contains the typical command steps and option button that we are familiar with from other features (Ordered shown).

The Option button produces the standard Option form allowing us to set the active feature options as well as save them for later use.  The Slot command has the following options:

  •  Slot Width
  • Flat or Arc end
  • Counter bore/boss and corresponding offsets

The only sketch input needed for the slot is an open path for it to follow, which also defines its length (width is defined in the Options).  Tangent connected lines and arcs are supported.  As typical to sketch based features in Ordered, the sketch may be pre-created as a standalone Sketch feature or created during the Slot feature.  As typical in Synchronous, the sketch must be pre-created as a Sketch.

Monday, November 09, 2015

Dimension Projection Line Breaks

Often when placing dimensions on drawings, the projection lines of some dimensions will cross the projection lines of other dimensions as shown below.

Solid Edge provides a function to automatically create breaks in one extension line where it crosses another. This function is called "Add Projection Line Break". It is accessible from the Shortcut Menu when you have a dimension highlighted.




The result is shown below.


If you wish to remove the projection line break, highlight the dimension, invoke the shortcut menu, and select "Remove Projection Line Break".