Frequently Asked Questions

Controlling default track widths Back


Many users feel that the default track width in Easy PC is stuck at a single value and cannot be changed. This is not correct, but the mechanism for controlling the default width is complex This document attempts to unravel this complexity.


The most important thing to remember is that track width is controlled by net class. The first part of the explanation discusses how this works, then continues by describing where net classes originate, and finally describes a strategy for reducing the confusion.

With a pcb design open in Easy-PC, go to Settings, Net Classes. This screen has columns for 'Name', 'Type', 'Min. Track', 'Nom. Track', and 'Via'. The column for 'Name' is self explanatory. Two types are available at present, 'Signal' and 'Power'. Although at present the type is only used as a label, it may be used in future for other purposes as well, so it should be defined appropriately. The most important settings are in the remaining three columns. These boxes should contain style names - track styles under 'Min. Track' and 'Nom. Track', and pad styles under 'Via'. During routing, it is the track style under 'Nom. Track' for the appropriate net class that determines the default track width. This also applies to autorouting, but there is an autorouting option to use the style defined for 'Min. Track' instead. All the available styles will be found under Settings, Design Technology, on the relevant tab. It is also here that new styles can be defined as required.

The awkward point is determining which is 'the appropriate net class' (as mentioned above). For a pcb being laid without a schematic, each track when it is started will use the net class defined by [Settings], [Remembered Styles], [Net Classes..]. This will be either the last net class used, or if it is the first track, the default net class defined by the technology file used. This setting can also be changed manually from the menu. If the pcb was translated from a schematic or project, the net class used will be the one defined in the schematic for that net. When drawing the schematic, the same principle applies, in that the default net class is also found under Settings, Design Technology, Net Classes. Again, this will be the last used, except for the first net, when the default from the technology file is used instead.

There is a technique to alleviate the worst effects of this structure (which is dictated by the need for autorouting control). It is this:

For pcb only designs, create a series of net classes, where the default width is one of the required track widths. To one side of the pcb design, place a short piece of track, one for each net class, set to the default width. To set the required width for the next track to be laid, just double click on the track of the desired width, then press Esc.

For translated designs, also create the net classes, but in this case in both the schematic and pcb files. In the schematic, draw a series of lines, each associated with a particular net class, and with the same name as the net class. For each line, right click and choose to display net name. Again, double click and Esc will cause the next connection to be drawn to use the chosen net class.

Back | Contents KB020010 / 02-Apr-2010 / Keywords: pcb styles widths