Netline Optimizer — User Guide

1Introduction

Netline Optimizer is a productivity tool for Siemens Xpedition PCB designs. It helps you clean up the unrouted connection lines — often called netlines or the ratsnest — that fan out from a heavily connected part such as a connector, an FPGA, or a memory device. When many nets run from one of these parts to the rest of the board, their netlines frequently cross over one another, which makes the area difficult to route and forces unnecessary trace jogs and layer changes.

The tool takes advantage of the fact that, on parts like these, a given signal can usually be assigned to any of several interchangeable pins. It looks at the nets you have selected, works out which pin each net should connect to so that the netlines stop crossing, and then reassigns the nets to those pins. Because a pin reassignment has to be reflected in the logical design as well as the layout, the tool also pushes the changes back into the schematic and forward‑annotates them so that the schematic and the PCB stay in agreement.

Tangled, crossing netlines fanning out from a part — Netlines crossing heavily as they fan out from the part — difficult to route.

Untangled netlines fanning out cleanly from a part — After optimization the same connections fan out cleanly, with the crossings removed.

In short: select the tangled nets on a common part, let the tool untangle them by swapping pins, and let it update the schematic to match. The result is a cleaner ratsnest that is far easier to route.

Important: The tool reassigns a net to whichever pin removes a crossing — it does this purely from the geometry of the netlines and does not require the pins or parts to be formally defined as swappable. That makes it flexible, but it also means it is up to you to apply it only where moving a signal to a different pin keeps the design functionally correct (for example, interchangeable connector pins, FPGA user I/O within the same bank, or other genuinely equivalent pins).

2Requirements and Setup

Before you start, make sure the following are in place. The tool connects to your running design automatically when it opens.

Xpedition must be running with the PCB database open. The tool reads the selected nets, the pins, and the routed traces directly from this open design. If Xpedition is not running when you launch the tool, it will tell you to open the design and start over.
The schematic tool must be running (with the matching project open) when you ask the tool to update the schematic. The schematic update and forward‑annotate steps talk to the schematic environment, so it needs to be open for those steps to work.
A valid ExactCAD license must be applied to your machine. If no license is found, the tool will ask you to apply your license code with the ExactCAD Licensing tool. When a valid license is present, the licensed user name and the expiration date are shown in the title bar.

Tip: Keep the tool window where you can see it. It stays on top of the Xpedition window so that its status messages and progress bar remain visible while you work.

3The Main Window

When the tool opens it shows a compact window with three main actions. Each action has a small square button on the left; click that button to run the action. The text beside each button describes what it does.

Netline Optimizer main window, standard view

The main window in its standard view, with the three core actions.

A few items on the window are shared by every action:

Item	Purpose & Behavior
Status light(colored square)	A simple busy indicator near the top‑right of the window. It is green when the tool is idle and ready, and turns red while an operation is running. Wait for it to return to green before starting the next action.
Status message(text line)	The line of text near the bottom of the window. It reads `Ready` when idle and otherwise describes what the tool is doing right now, such as collecting net data or calculating swaps.
Progress bar(below the status message)	Fills as a long operation works through the selected nets, so you can see that the tool is making progress.
Exit button(red, top‑right)	Closes the tool. It first removes any temporary review lines the tool drew on the layout, so your design is left clean.
Show / Hide Advanced Options(wide button)	Expands or collapses the lower part of the window to reveal the advanced options described in Section 5. The window grows or shrinks to fit.

4Standard Actions

The three core actions are normally run in order: first calculate the swaps on the PCB, then apply them to the schematic. The tool keeps the calculated result in memory between steps.

4.1 Get Selected Nets and Calculate Net Pin Swaps

This is the heart of the tool. Run it after you have selected, in Xpedition, the nets you want to untangle. Here is what it does:

Finds the common part. It looks at every selected net and identifies the part that the most of those nets connect to — typically the connector or device you are trying to fan out. If two parts are tied for the most connections, it asks you to type in which one to use.
Builds a netline for each net. For every selected net it draws an imaginary line from the common part’s pin to the far end of the net, following any traces and vias that are already routed.
Untangles the netlines. It compares the netlines in pairs and, wherever two of them cross, it swaps which pin each of those two nets connects to on the common part. It keeps doing this until the netlines no longer cross.
Lets you review the result. You are first offered a chance to see the original netlines drawn on the layout, and afterward to see the new, untangled netlines. You can stop at this point if you do not want to keep the result.
Optionally saves a report. It offers to save a text file listing each net and the pin number it has been assigned to.

Close-up of netlines crossing between routed traces — A close look at the netlines before optimization — several connections cross.

Close-up of netlines running parallel without crossing — After the swap the same connections run side by side with no crossings.

Note: At this stage the new pin assignments exist only as a calculated plan held by the tool. Nothing is changed in your schematic until you run the schematic update in Section 4.3 (or turn on automatic updating in Section 5.1).

4.2 Swap Two Nets

Use this when you simply want to exchange the pin assignments of exactly two nets on the common part, rather than letting the tool work out an automatic untangle. Select two nets in Xpedition first, then run this action. The tool finds the common part and swaps the two nets so that each takes the other’s pin.

Warning: This action does nothing unless exactly two nets are selected. If you have a different number selected, nothing happens.

4.3 Swap the Schematic Nets

Run this after a calculation (Section 4.1) or a two‑net swap (Section 4.2) to write the new pin assignments into the schematic. The tool connects to the schematic, finds the affected part, and re‑labels the appropriate pins with their new net names. It also keeps any matching off‑page connector labels in step with the new net names, and it builds a “was / is” record of every change.

If any change cannot be applied, the tool warns you at the end and notes the failures in the report so you can review them.

Tip: After the schematic is updated you will normally forward‑annotate so the PCB picks up the new connectivity. The tool can do this for you automatically — see Section 5.1.

5Advanced Options

Use the Show Advanced Options button to reveal the extra settings and tools. The window expands to show two checkboxes and two additional actions.

Netline Optimizer main window, advanced view

The window with the advanced options shown.

5.1 Auto Update Schematic and Forward Annotate

When this box is checked, the tool runs the whole sequence for you in one pass. As soon as a calculation or a two‑net swap finishes, it automatically updates the schematic and then forward‑annotates the changes back to the PCB, so the layout and schematic end up in agreement without your having to run each step by hand. When the box is unchecked, you run each step yourself.

Note: Because this option chains the schematic update on automatically, make sure the schematic tool is open with the correct project before you run a calculation with this box checked.

5.2 Save Pin Swap Reports after Schematic Updates

When this box is checked, the tool automatically saves the “was / is” report each time it updates the schematic, prompting you for where to save the file. This gives you a permanent record of exactly which pins changed and how. When it is unchecked, no report file is written for the schematic update.

5.3 Export Pin List

This produces a text file that lists, for a single part, every pin number alongside the net currently connected to it. When you run it, the tool asks you for the part’s reference designator, then saves the list to a location you choose. It is a handy way to capture a snapshot of a part’s connections — for example, before and after a set of swaps.

Tip: Export a pin list before you start and another after you finish, then compare them with the next tool to confirm exactly what changed.

5.4 Compare Pin Lists

This compares two pin‑list files that you exported earlier and reports the differences. When you run it, the tool asks you to pick the two files, then produces reports covering:

Nets that appear in the first file but not the second — and, where such a net still exists on the current PCB, the pins it connects to.
Nets that appear in the second file but not the first.
A pin‑by‑pin “was / is” comparison showing every pin whose net assignment differs between the two files.

You are prompted to save each report so you can keep a clear before‑and‑after record of the changes.

6Typical Workflow

A common end‑to‑end session looks like this:

In Xpedition, open the design and select the nets that fan out from the connector, FPGA, or other part whose netlines you want to untangle.
Launch Netline Optimizer. Confirm the status light is green and the message reads Ready.
Run Get Selected Nets and Calculate Net Pin Swaps. If asked, choose the common part. Review the original netlines if you wish.
Review the new, untangled netlines. Continue if you are happy with them, or stop to discard the result.
Save the pin swap report if you want a record of the new assignments.
Run Swap the Schematic Nets to write the changes into the schematic, then forward‑annotate so the PCB matches. (Turn on Auto Update Schematic and Forward Annotate first if you would like steps 6 chained automatically after step 3.)
Close the tool with the red exit button when you are done.

Tip: You can run the tool on the same part more than once. Because each pass works from the netlines as they currently stand — following whatever has already been routed — re‑running it as your routing progresses lets you progressively unscramble the connections. As traces get closer to the source or destination of the affected signals, the netline geometry sharpens, and a fresh calculation can refine the pin assignments further. Running it a few times over the course of routing often produces a cleaner result than a single pass at the start.

7Tips & Troubleshooting

The tool closes immediately or says Xpedition is not running: Open your PCB design in Xpedition first, then launch the tool. It needs an open design to connect to.
It asks you to apply a license: Run the ExactCAD Licensing tool and apply your license code, then reopen Netline Optimizer. The title bar will show your name and the expiration date once the license is recognized.
Nothing happens when you try to swap two nets: That action needs exactly two nets selected. Check your selection in Xpedition and try again.
The schematic did not change: The schematic update and forward‑annotate steps need the schematic tool open with the correct project. Open it and run the schematic update again.
Some swaps were reported as failed: Open the saved report to see which pins did not update, then address those nets individually.
The status light stays red: An operation is still running — large net selections take longer. Watch the progress bar and wait for the light to return to green before starting another action.
You want a clean record of the changes: Export a pin list before and after, then use Compare Pin Lists to document exactly what moved.