The Netline Optimizer automatically calculates pin swaps by swapping netlines that intersect.
Swapping Nets using Netlines
First, determine which pins can be swapped in your design. The Netline Optimizer will try to swap any and all nets that are selected, so it is important to only select nets with pins that you want to swap.
Using the Net Explorer in Layout, you can filter out any nets that you do not want to be selected. While this is not necessary to use the Netline Optimizer, it can be very helpful to save a filter scheme so that you don’t accidentally swap the wrong pins.
Get Selected PCB Pins and Calculate Net Pin Swaps
Once you’ve determined which pins can be swapped, simply select the netlines, pins, or traces of those nets and hit the ‘Get Selected PCB Pins and Calculate Net Pin Swaps’button.
When netlines are traveling to many parts, the program will swap pins on the part that the nets’ connections all have in common. In a case where a group of signals are only traveling between two parts, you will be given an option of which part to swap the pins on.
Swap Two Nets
If you just want to manually swap two nets without having the tool analyze the netlines, you can simply select the nets and hit the ‘Swap Two Nets’ button.
Swap Nets on Schematic
Once you have used the tool to calculate pin swaps, you can use this function to swap the pins on the schematic.
To begin, make sure you have the schematic open in Designer, and that you have read/write access. Press the ‘Swap Nets on Schematic’ button to begin. The tool will find the part symbols and swap the nets.
Press the ‘Show Advanced Options’ button to show additional features.
Auto Update Schematic and Forward Annotate
By checking the ‘Auto Update Schematic and Forward Annotate’ box, the schematic will be changed, and the design will forward annotate immediately once pin swaps have been calculated. Once you are familiar with the Netline Optimizer, this option can make swapping netlines very quick and easy.
As always, make sure you have the schematic open in Designer and that you have read/write access.
Settings for forward annotation should also be configured in the Project Integration window before beginning.
Save Pin Swap Reports
Check the ‘Save Pin Swap Reports’ box to save a report of the net changes when using the ‘Get Selected Nets and Calculate Net Pin Swaps’ function.
Export Pin List
Use this function to export a pin list for a given component. When you select the ‘Export Pin List’button, the following dialog will open and allow you to enter the part Ref Des that you want a pin list for:
Compare Pin List
With this function you can open two pin lists, and the tool will compare and report the changes. The report is a text file; when the comparison is done, you will be prompted to save the file wherever you want it. The report file will have 3 lists in it:
1. A list of nets that were in the first pin list, but are no longer in the second one.
2. A list of nets that are in the second file, but were not in the first.
3. A list of the modified pins, showing the before and after net names of each pin. This list is sometimes referred to as a “was/is” list.
Prerequisites & Conditions for this tool:
The tool was designed to be as simple as possible. However, it’s approaching a very complex task, so there are a few things to consider and do before using it:
1. It will work on any schematic symbol. It does not care what the symbol looks like or how it is built.
2. The pins that will be swapped do not need to be defined as swappable in the component PDB. This tool does not depend on any native information in the symbols or footprints to determine what it can do and what it can’t do.
3. The PCB designer must know what pins & nets are swappable, and select them accordingly. This is normally accomplished by working with the electrical engineer, FPGA designer, or anyone else who will know with certainty what pins & nets are allowed to be swapped with each other.
4. The net & pin swapping on the schematic is done by changing net names. Net segments are not moved, pins are not renumbered. The net segments are just renamed.
5. Because of item 4, the net segments on pins that will be swapped can’t be connected between the component of interest (for example, an FPGA) and some other parts, such as series resistors, capacitors, or anything else. Those parts can be attached to the nets, but they need to be separated by an off-page or on-page connector symbol
Examples of schematic nets that can and can’t be used by this tool:
Pins U29, U23, U21, and U22 can’t be swapped, because they are directly connected to a resistor or physical test points.
Pins V30, Y30, and W30 can all be swapped, because they are connected to the FPGA pins on one end, but only to off-page connectors on the other ends. The net names on these segments can be changed without altering the connection to any parts on those nets except for the FPGA.
Of course the functionality of the device needs to be considered. That’s where the EE or FPGA designer comes into play, to help the PCB designer know which nets and pins can be swapped, and which need to be left alone. The pre- and post- operation pin lists generated by this tool can assist in verifying that any non-swappable pins and nets remain the same throughout the process of the PCB layout.