Ignore PCB Layout Drill Back Off Warnings

If you read no further, here is the summary: Ignore drill back off errors.

Here is an explanation of what drill back off is, and why just about anyone can ignore warnings about it, today.

Here is a simple schematic, just a capacitor, and a connector.
default layout
If you had your software automatically route a PC board, it might look something like this. The pads for the capacitor are 100 mils in diameter, and the traces are 10 mils wide.  What doesn’t show is that the traces actually have rounded ends, and extend all the way into the exact center of the pad.
250 mil traces
Let’s say we were dissatisfied with the narrow traces of the previous layout, and decided to widen the traces to 250 mils, to carry more current.  In looking at the trace to the top pad of the capacitor, we can now see that the trace actually goes all the way to the center of that pad, and has a radius about  that point.
actual copper
Layout software often won’t show copper in a hole, under the assumption that the hole will be drilled out, anyway. This is what the copper layer around the upper pad of the capacitor will really look like if the design is fabricated as-is, but not drilled.
pad in outline
The pad is shown as an outline here, for greater clarity.  In the old days, when a human operator might be manually drilling the holes, there might be need for a clear target for the drill.  In this case, and operator could still make out where the center of the hole is, but in the case where the trace was actually wider than the hole, there would be no target at all.
thin trace backed off
Here is what some brilliant production engineer might do.  They might “back off” the trace in the direction from which it came in, just enough to clear the hole and leave a perfect target for the drill operator.  In fact, they could run a script on the entire design to back off all traces automatically for drilling.
wide trace
Here is the same pad as above, with a super-wide trace going to it.  The trace is actually larger than the pad, and covers it completely.
wide trace backed off
The trace has to be backed off quite a bit to clear the hole.
backed off beyond pad
Part of the radius of the trace is shown in outline to better illustrate what is going on.  The trace is backed off so far, that the end point does not even lie within the pad.  In fact, if the trace was short (like the one on the lower pad of the capacitor), the back-off could create a zero or negative-length trace (that is, a trace in the other direction).  A trace in the other direction is very bad, as it could unintentionally short some other components.
dimension formula
In packages like DesignSpark, in mathematical terms, a drill backoff error is generated when t > (p – h)/2, that is, when the trace is wider than the annular ring of the pad.

The reason we need not worry about this error today is that no contract manufacturer is going to alter the layout by backing off traces in such a manner. As the drilling is done by an NC (Numerically Controlled) robot drill, there is no need for a visible target. In fact, the drilling will typically be done on the board blank before any copper patterning even takes place.

Why this design rule check is still available in packages like DesignSpark is unclear to me, but fortunately, the check is optional, and can be turned off by unchecking a box. Most other layout software doesn’t even have the check at all.

(Visited 1,839 times, 1 visits today)
  1. Thanks for that. I’m using Design Spark and there seems to be no way of routing without drill back off errors whether I’m routing manually or not. Now I don’t need to worry. Except of course I do. In which case I’ll try your formula out. Shame the DesignSpark help pages and fora don’t seem to have a clue about this.

    1. Glad to help. I went through the same anguish on my design, and had to hunt a bit to figure out what was going on. I thought that I posted this tip to one of the DesignSpark forums (fora?), but my memory at this age isn’t what it used to be. I’m old enough to remember the era when a production engineer might actually do a drill back-off. (In fact, I remember when boards were laid out manually with physical tape – no gerbers involved.)

  2. Okay so now I’ve had a good play in DesignSpark and finally cracked it. Your formula is wrong. The correct formula (at least for DS8.1.1) is t must be equal to or less than p – h. Works every single time. Why this should be makes no sense to me. Your equation made more sense but doesn’t work in DS. Now I need to work out erroneous cm-cm errors when components are miles apart! I’ll get there…eventually…

  3. More investigations…apologies I had the wrong pdf output settings in DS. Your formula does work after all! So does mine as far as back off errors in DS are concerned, which was all I was thinking about from the title of your blog. Why these back off warnings matter in DS is if you’re outputting to a pdf to etch your own boards – the pad holes are obscured by the tracks so you can’t see where to drill precisely. Both your and my formula work to back off the tracks to leave the pad holes perfectly visible. What your formula does (and mine doesn’t) is that it takes care of drill breakout in addition to drill back off. Most excellent indeed.

Leave a Reply

This site uses Akismet to reduce spam. Learn how your comment data is processed.