4
\$\begingroup\$

in the PCB I am designing there is 0.88mm between one track and a through hole pad. Between the track and the pad there is a DC voltage difference of around 425V.

Clearance calculators like this one specify a minimum clearance of 0.8mm for 500V if "external conductors coated" are used. If that is the case, I am safe, but I am not sure about what "external conductors coated" refers to.

The track and the pad are in the top layer, so I assume they are external, but are they coated? that coating is referred to a standard solder mask or is it a special one?

EDIT:

If the clearance is not enough I have two options: 1. Apply a coating after soldering. (I am not sure how yet) 2. Cut the problematic track and use a wire instead

What do you think it is best? this is the problematic track:

enter image description here

\$\endgroup\$
4
  • 2
    \$\begingroup\$ IPC-2221A (6.3 - Electrical Clearance): Typical applications (like yours) are in the category B4 "External Conductors, with Permanent Polymer Coating (Any Elevation)". This is a pcb with solder resist. Clearance rule is 301-500V : 0.8mm. I think you can leave it as it is without conformal coating. \$\endgroup\$
    – Batuu
    Nov 23, 2017 at 13:33
  • \$\begingroup\$ Now that you explained that the solder mask is the "Polymer coating" it looks better.. :) Thanks! \$\endgroup\$
    – jap jap
    Nov 23, 2017 at 14:48
  • 2
    \$\begingroup\$ In this particular case, you can solve this by routing the track around. \$\endgroup\$
    – Simon Richter
    Nov 23, 2017 at 15:30
  • \$\begingroup\$ Yes, that would be the safest solution, sadly the PCB is already if the manufacturing process and it can not be changed. \$\endgroup\$
    – jap jap
    Nov 23, 2017 at 16:00

1 Answer 1

Reset to default
8
\$\begingroup\$

The standard solder mask is not a conformal coating.

IPC-SM-840C:

Solder mask materials covered in the standard are not intended for use as a substitute for conformal coatings that are applied after assembly to cover components, component leads/terminations and solder connections.

Related to IPC-2221A (4.5.2.1) there are some types and requirements for the thickness:

  • Type AR - Acrylic Resin : 0.03 - 0.13 mm
  • Type ER - Epoxy Resin : 0.03 - 0.13 mm
  • Type UR - Urethane Resin : 0.03 - 0.13 mm
  • Type SR - Silicone Resin : 0.05. - 0.21 mm
  • Type XY Paraxylylene Resin : 0.01 - 0.05 mm

IPC-2221A (6.3.4):

Typical applications are computers, office equipment, and communication equipment, bare boards operating in controlled environments in which the bare boards have a permanent polymer coating on both sides.

After they are assembled and soldered the boards are not conformal coated, leaving the solder joint and soldered land uncoated.

Note: All conductors, except for soldering lands, must be completely coated in order to ensure the electrical clearance requirements in this category for coated conductors.

"permanent polymer coating" stands for solder mask / solder resist.

So when you don't do a conformal coating after the component assembly, you only can relate on the uncoated or with Permanent Polymer Coating categories for your clearances.

\$\endgroup\$

Your Answer

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

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