Frequently Asked Questions
Controlling default track widths
[ PCB Design / General Design Editing ]
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], [Design Technology] and open the [Net Classes] tab. This screen has columns for 'Name', 'Type', 'Min. Track', 'Nom. Track', and 'Via'. The remaining columns for 'LenDiff Enabled', 'Length Diff', 'MinMax Enabled', 'Min', 'Max', 'Own Colour' and 'Colour' are not relevant here but you can learn more about their use by pressing <F1>.
The column for 'Name' is self explanatory. For 'Type', two are available at present, 'Signal' and 'Power'. Although at present the type is mostly used as a label (the only place where it makes a difference at present is when reverse engineering), 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 manual routing, it is the track style under 'Nom. Track' for the appropriate net class linked to the selected net 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. Double clicking on a cell will give a pull down list of the available options for that cell.
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], [Defaults] ([Remeebered Styles] in early versions), on the [Nets] tab. 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 available net classes are also found under [Settings], [Design Technology], [Net Classes] tab. Again, the default used for new nets will be defined under [Settings], [Defaults] (/[Remembered Styles]) on the [Nets] tab and will be the last used, except for the first net, when again, the default from the technology file is used. Note that the setting under [Defaults] only updates when adding a new track (or connection in a schematic). It does NOT update when an existing one is just being edited.
There is a technique to alleviate the worst effects of this structure (which is dictated by the need for autorouting control). It is this:
Under [Settings], [Preferences] on the [PCB Tracks] tab is a setting to 'Use Selected Track Style'..For pcb designs, create a series of tracks to one side of the design, one for each track style required. The net class each uses is irrelevant as this technique doesn't change the default.. To set the required width for the next track to be laid, just click on the track of the desired width, then start routing the desired track. Use any 'Add Track' method to start the new track, including hot keys but NOT double clicking as this moves the focus away from the previously selected track and defeats the utility..
For translated designs, also create the net classes, but in this case in both the schematic and pcb files. In the schematic, there's no equivalent method of easily choosing the net class to be used, but you can set up a hot key for this. Under [Settings], [Customise] on the [Keyboard] tab, set the 'Commands' box to 'All commands', then scroll down to 'Remembered Net Class' and select it. Now you can set up your own shortcut key to display the default net class dialogue, allowing you to change to the desired default with ease. Use <F1> for full instructions for this dialogue.
There's a further option when routing PCBs. Under [Settings], [Preferences], again on the [PCB Tracks] tab is an option to 'Don't use Track and Via Styles from the Net Class'. This causes the styles defined under net classes to be ignored. Instead the sizes defined under [Settings], [Defaults] on the [Track] and [Via] tabs are used.Whilst laying tracks, any change ibn track style, layer or via style updates the settings under [Defaults], so effectively the program will always resume with the last style used.