Some people online say that acute angles in trace routing will cause these problems:

  • "Acid Trap" - PCB etchant gets stuck in the corner, and eats away too much, causing open circuit
  • "Peelable" - Narrow strip of photoresist falls off the board before or while the etchant is applied, causing too much etching and thus open circuit

Some people online say these are real problems, others say they are old wives' tales. Are they real or not? Or are they only real if you use a low-cost fab house that might use older processes?

Please avoid answers like "ask your fab house". I'm looking to learn in general, not just get one design out the door.

  • \$\begingroup\$ Related/duplicate: electronics.stackexchange.com/q/102910/2028 \$\endgroup\$
    – JYelton
    Commented Jun 17, 2014 at 5:53
  • 3
    \$\begingroup\$ Also note that most board houses with tight design rules (think 4/4 and tighter) use photoactivated etchants exactly to avoid the issue of acid traps. With that process, the etchant is not very reactive unless excited with some specific wavelength of light, so any etchant in non-illuminated corners will not eat away too much at the sides. This also produces much better quality traces when dealing with tight design rules and thicker copper (2 or 4oz copper) \$\endgroup\$
    – user36129
    Commented Jun 17, 2014 at 7:18
  • \$\begingroup\$ @user36129 Thanks, that's very good to know! \$\endgroup\$ Commented Jun 17, 2014 at 7:54
  • 2
    \$\begingroup\$ blame me, but at first i read the title as "are acid trips real?" \$\endgroup\$
    – noncom
    Commented Jun 17, 2014 at 12:56

4 Answers 4


In order to combat acid traps, underetching of thick copper layers and other such problems with traditional thermally activated etchants, a lot of board houses have switched to photoactivated etchants. These etchants are much more active under the influence of light than just by themselves, which means you can get cleaner edges on thick copper layers. Also, etchant trapped in sharp corners in the design doesn't eat away at the sides nearly as much as it would with traditional methods.


Are they real or not?

These are general design guidelines that reduce the incidence of problems. However, today's PCB fabrication processes have improved to the point where good PCB fab lines can manage any trace angle that doesn't violate any of their other design rules, such as trace width.

Today's masks also provide substantial mechanical support to traces, so you can add some confidence that this won't happen to your design if you specify a mask.

are they only real if you use a low-cost fab house that might use older processes?

I'm sure there are fab houses with processes that will have a slightly higher failure rate with sharp angled traces than otherwise. It doesn't matter whether this is due to poor process, materials, or skills.


The US-based assembly house I work with will complain and ask for corrections in PCBs with acute angles.

Whether their complaints are over-cautious or not, I do not know. They contract to several different PCB vendors both US and overseas, so it could be an issue of making sure that ANYONE can build the part.

I finally just set an Altium rule and it hasn't been a problem since. I typically spend 10 minutes or so cleaning up acute angle errors to pad entries at the end of a moderate sized layout if I haven't been watching it along the way.


Generally problems of this nature can occur in really cheap fab houses in china, although they are rare otherwise.

One disparity I notice in the explanations is the Peelable. If too much enchant is applied, how could it possibly result in a short circuit? It would be etching away MORE than it should be, not not etching what it should.

  • 1
    \$\begingroup\$ @David I think specific countries are ok since the question is specfic to this year (2014). \$\endgroup\$ Commented Jun 17, 2014 at 7:45
  • 1
    \$\begingroup\$ @Shannon thanks for catching my mistake about the peelable, I fixed it \$\endgroup\$ Commented Jun 17, 2014 at 7:46

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.