Working with a User-defined FromTo Object on a PCB in Altium Designer

User-defined FromTo

Summary

A User-defined FromTo allows you to create specific net topologies within a design giving you total control over the arrangement or pattern of pin-to-pin connections in a net. They are different from system-generated FromTos, added and arranged by the PCB Editor to give the shortest overall connection length in each case - a net topology referred to as Shortest. Displayed in the design space as pin-to-pin connection lines, FromTos are collectively referred to as the 'ratsnest.'

Availability and Placement

User-defined FromTos can be added for part or all of a net using the From-To Editor available in the PCB panel.

Non-Graphical Editing

A user-defined FromTo object cannot be edited with respect to properties in the usual manner. It cannot be selected in the design space, has no corresponding mode in the Properties panel and cannot be edited graphically.

FromTos can only be viewed when the PCB panel is configured in From-To Editor mode.

Notes

• A system-generated FromTo does not appear in the design space as a separate entity. Only the associated pin-to-pin connection line for the FromTo is displayed, which is used for interactive routing/Autorouting guidance.
• A User-defined FromTo appears in the design space as a dotted line, separate and distinct from the pin-to-pin connection line that is also displayed when the FromTo is added. The user-defined FromTo line controls where the associated pin-to-pin connection line starts and finishes. This is best demonstrated by example. Consider a user-defined FromTo added between the logically connected pins of two components. A connection line is also added and displayed (PCB panel configured in Nets mode):

• The pin-to-pin connection line - used for routing purposes - conceals the presence of the distinctly separate user-defined FromTo line. However, as you start to route the connection, you can see the distinct and separate nature of the two lines:

• If the routing is now suspended, the Connectivity Analyzer adds a connection line so as to maintain the required topology, shown as a dotted line (called a Broken Net Marker), indicating that the net should be routed between these two points to maintain the topology determined by the user through the addition of the user-defined FromTo:

• If you specify user-defined FromTos for only part of a net, the PCB Editor will set the remaining pin-to-pin connections (system-generated FromTos) to the Shortest topology.
• The type of FromTo determines how the Connectivity Analyzer treats the connection line in the design space when, for example, a net object is moved or part of a net is manually routed:

• System-generated FromTo - the connection line can be moved as required as part of the Connectivity Analyzer's re-optimization to keep the default topology of the net (i.e., Shortest).
• User-defined FromTo - if the FromTo is not the result of selecting a predefined topology, the connection line is not considered as part of the Connectivity Analyzer's re-optimization process. If the FromTo is part of a predefined net topology (other than Shortest), the Connectivity Analyzer can include it in re-optimization, as long as the chosen topology is kept.