3

Is there a way in eagle to center a trace between two pads? and by center, I mean directly center it with even spacing on both sides of it.

I'm asking because its easier to solder pads that aren't too close to another trace and I don't want to create any shorts. Also, I believe having traces too close together introduces on-board capacitance.

  • 2
    Unless you are using *a lot* of different packages and/or trying to build something very compact, this shouldn't be much of a problem if you are using a sensible grid. You might be overthinking the problem. Can you provide a bit more context? What distances are we talking about? – Wesley Lee Nov 05 '16 at 21:41
  • Im interested in centering between two pads of a standard DIP IC. I use restring of 0.25mm and I want to center a 0.25mm trace in-between two adjacent IC pads. –  Nov 06 '16 at 18:08
  • DIP is 2.54mm(0.1in) pitch, if you use a 1.25mm or 0.05in grid tracks will likely be automatically centered. You can use 'alt' key to use a finer pitch grid temporarily, then you can use 0.025in or 0.0125in. – Wesley Lee Nov 06 '16 at 18:29

2 Answers2

3

If you know the x-y coordinates of the two pads, then just draw a trace and then edit its properties so that it is located equidistant from the two pads.

Now if the pads are on grid (e.g. if you are using an 0.05" grid and 0.1" pitch ICs), then you simply draw the trace on-grid and it will automatically be in the centre. This is why trying to stick to grids is a good idea - though I accept it falls down a bit if you are mixing SMD ICs with different pitches.

Beyond that there is no way that I know of to do it directly. Eagle doesn't have a way to align objects to other objects (or distribute equally). If you don't directly know the x-y coordinates of the pads, you need to open up the package (in Eagle 6.x and newer you can right click -> edit package), find the coordinates in the library, and then offset them by the component origin in the board. Then edit the trace properties to be equidistant.

Tom Carpenter
  • 63,168
  • 3
  • 139
  • 196
3

There is no direct way to center a trace between two pads other than manually specifying coordinates. That would be a bit silly. However, there are ways to address your issues.

Actually, ease of solder has nothing to do with how close other copper is, as long as that other copper is covered by solder mask.

Avoiding shorts due to too close traces is handled by defining minimum clearance distances. The absolute minimum is what your board house can reliably do, and that should come from them. Unless you are doing something unusual, use 8 mil minimum clearance. Any board house around the world can do that reliably nowadays.

Additional clearance beyond the board house design rules may be required due to the voltage between traces. 8 mil is fine up to 50 V or so. If your voltage is higher between some nets, then you should create net classes for them and specify a suitably large clearance between those net classes. Do HELP CLASS for details.

Otherwise, don't worry about whether a trace is exactly in the middle between two pads. Specify the rules, and Eagle will follow them. Going between two pads isn't a special case, and you shouldn't try to make it one.

Olin Lathrop
  • 310,974
  • 36
  • 428
  • 915
  • The thing is I make my own single-sided PCBs and I'm getting better at it, I also have a printer that only wants to print at 600 DPI. I'm just trying to produce the best board even if the printer fails to print one pixel properly. I'm used to doing 0.3mm wide traces but now I'm going as low as 0.25mm. I tried a board once with 0.2mm traces, but those traces vanished after trying to remove unwanted photo-resist. Traces wider than that remained. –  Nov 06 '16 at 18:55