I'm using DesignSpark to lay out a PC board, and am getting lots of "drill back off" errors during DRC (Design Rule Check). I understand from the web the theory behind these warnings, but wanted to ask whether a fabrication house generally will back off traces in that manner. Seems to me that a manufacturer should be able to provide WYSIWYG (what you see is what you get) traces to match the Gerber plots. Is this just a deprecated check from old days when there was a human that needed to see an actual lack of copper to know where to drill? I'm assuming that any board house is going to have a machine do the drilling, using the NC Excellon file.

I also notice that other tools such as KiCAD don't even seem to perform this check.

 

I have had a role in the a fair number of PCBs and have never come across this error.

 

I have had a role in the a fair number of PCBs and have never come across this error.

Thanks for responding. Actually, even a "never seen that" is very helpful.

Any other people out there who made PC boards? Even if only to add that you've never seen this error, either.

 

Most every house will just run your Gerber as delivered. They would question you before making a change, which slows things down, so normally they just run them as is. High quality houses ($$$) you have a relationship with may call you first.

I would not see that problem in the packages I have used (Orcad, Kicad) because a backed off trace would fail the Netlist check, as a trace must end on the center of a pad to be considered connected.

Get a good third party viewer such as GC Preview (free) and zoom in on your pads to see if you have back off nicks. if not, sleep sound.

If it was my board I would be extending all my traces right into the pad center, which not only clears that error but is where I actually want them.

 

Thanks for responding. Actually, even a "never seen that" is very helpful.

Any other people out there who made PC boards? Even if only to add that you've never seen this error, either.

I have done some weird things with DesignSpark and never had that error. Does it only come when you make the Gerber File (or run design check?). Or does it come when printing the file as well?

 

One reason to have a gap of more narrow trace between a trace and pad of the same dimension is thermal relief. This term usually applies to pads in power and ground planes, but it also applies to large pads and heavy copper traces, or a wide trace with a small diameter hole in it. The pad might not solder properly because the trace is acting as a heatsink.

ak

 

I have done some weird things with DesignSpark and never had that error. Does it only come when you make the Gerber File (or run design check?). Or does it come when printing the file as well?

It's DesignSpark 6.0, not the most current version. When I run Design Rule Check (DRC) with the PCB file open in the current window, one of the Manufacturing checks is for Drill Backoff. That box is not checked (ticked) by default. On screen or in plots, the artwork looks just the way I want it to look.

I'm also getting Trace-to-Shape errors all over the place, but those I understand. I intentionally want these copper rectangles to short to the traces, as they are part of the heat sink for surface-mounted DPAK transistors that could potentially dissipate 1-2 watts.

 

One reason to have a gap of more narrow trace between a trace and pad of the same dimension is thermal relief. This term usually applies to pads in power and ground planes, but it also applies to large pads and heavy copper traces, or a wide trace with a small diameter hole in it. The pad might not solder properly because the trace is acting as a heatsink.

ak

I thought about using spoked thermal relief pads, but ultimately decided that I would just deal with the difficulty in hand soldering, in exchange for a possibly lower resistance electrical connection. These are 50-farad supercapacitors, and I need 48 amps of surge current through them at times. The board is 2 oz copper, with 250-mil traces running on both sides of the board to carry current from the supercaps. The traces are on the outside of the board, not internal planes.

 

Most every house will just run your Gerber as delivered. They would question you before making a change, which slows things down, so normally they just run them as is. High quality houses ($$$) you have a relationship with may call you first.

I would not see that problem in the packages I have used (Orcad, Kicad) because a backed off trace would fail the Netlist check, as a trace must end on the center of a pad to be considered connected.

Get a good third party viewer such as GC Preview (free) and zoom in on your pads to see if you have back off nicks. if not, sleep sound.

If it was my board I would be extending all my traces right into the pad center, which not only clears that error but is where I actually want them.

Yes, DesignSpark runs all traces to the center of the pad, or else will throw a DRC error of Gap in Net. I suspect that someone at some time faced a board house that backed off traces, otherwise, why would programmers bother to put the check in as an option?

EXCELLENT advice on using an external Gerber Viewer to look at things! Why didn't I think of that?

 

Run your gerbers through Advanced Circuits FreeDFM and see if it kicks anything back at you.

 

Run your gerbers through Advanced Circuits FreeDFM and see if it kicks anything back at you.

I viewed the Gerbers on the GC prevue viewer, and they looked perfect. No surprises. Thanks, ErnieM!

That FreeDFM is free, but kind of like letting a salesperson into your home for a free demo. It required all kinds of information, including email and phone number. I'm waiting for results, now. Truth be told, that 4pcb.com looks like a high-class operation, with all kinds of certifications and capabilities. To torture an analogy, they are a Tesla, but all I really need is a bicycle.

 

I viewed the Gerbers on the GC prevue viewer, and they looked perfect. No surprises. Thanks, ErnieM!

That FreeDFM is free, but kind of like letting a salesperson into your home for a free demo. It required all kinds of information, including email and phone number. I'm waiting for results, now. Truth be told, that 4pcb.com looks like a high-class operation, with all kinds of certifications and capabilities. To torture an analogy, they are a Tesla, but all I really need is a bicycle.

Nothing is ever really free, is it? Advanced Circuits is a good group. Very professional and they don't spam or call you incessantly. I've used them for in excess of 10 years.

 

Thanks, joeyd. Freedfm.com did catch one minor thing, although it would not have affected the functionality of the board. There was exactly one spot where the solder mask was 1.5 mil too small for the pad, caused by a tiny stub of trace that I didn't see because it was under the pad. Actually, it was a via, so as long as the hole wasn't covered by solder mask, who cares. I fixed it up, of course, and it went through a second pass without any problems detected.

So in final summary, guess I'll be sending it off to fab soon. Since it's just a hobby job, I'm going to sleep on it overnight before submitting.

 

Since it's just a hobby job, I'm going to sleep on it overnight before submitting.

Sleeping on it is quite an excellent technique when inspecting your own work.

If the task it still current in your mind yo will repeat your own mistakes over and over. If you let yourself forget the details (by allowing enough time to pass by going to sleep for a night or a week) you get a fresh set of your own brain cells to work the problem over once more.