PCB Fabrication Notes for 2016, Part 2

This is the second part of a series about PCB fabrication notes. As we mentioned previously, your requirements may be different, but these are based on what works best for our projects.

Finish

There are many different surface finishes, each with their own benefits and drawbacks. We use either:

• HASL for the few low cost non-lead-free boards where we don't have any fine pitch components
• ENIG, for most of our projects

One of our CMs explained to me that they prefer ENIG because it is ruler flat and is easier to work with. In low to moderate quantities the cost difference between ENIG and HASL will not be much.

We had one project where we specified "FINISH IS ENIG AS PER IPC-4552" and nothing else. The CM went to build the boards and was having a tough time getting the solder to adhere. It turns out that IPC-4552 has two acceptable plating thicknesses: a thinner plating for devices that will be soldered soon, and a thicker plating for devices that won't be soldered soon. The PCB Fabrication house used the thinner plating thickness but did not plate enough so the gold baked off and the solder was not able to adhere to the nickel below. So, now we specify the following:

FINISH IS ENIG AS PER IPC-4552 WITH 2 TO 5 MICROINCHES OF GOLD OVER 120-230 MICROINCHES OF NICKEL.

Solder Mask & Silkscreen

The solder mask is the protective paint like layer that is on top of the copper traces, and is often green but is also available in red, blue, black, white, purple, etc. You need to specify the type of soldermask, the color, and how it shall be applied. If you are building a PCB that will operate at a high temperature (like an LED board) and you want a white soldermask then you should also specify a non-browning type.

Silkscreen is the lettering and printing that is on the PCB, and is usually a contrasting color to the soldermask. So if the soldermask is red, green, or blue then the silkscreen should be white or yellow. Contrastingly, if the soldermask is white then the silkscreen should be black. While our design shouldn't have silkscreen on any component pad, we want to ensure that the PCB fabrication house will catch any errors, so we add the requirement below.

   SOLDERMASK SHALL MEET IPC-SM-840E, CLASS T REQUIREMENTS, COLOR BLUE. APPLY OVER BARE COPPER AS PER IPC-6012, CLASS 2.
   SILKSCREEN SHALL BE WHITE, PERMANENT, ORGANIC, NON-CONDUCTIVE INK. APPLY AS SHOWN IN FILES. THERE SHALL BE NO SILKSCREEN ON ANY SOLDERABLE COMPONENT PAD.

Bow and Twist

The most important part of specifying bow and twist is defining how it is tested. IPC-TM-650 is an IPC defined test method.

BOW AND TWIST SHALL NOT EXCEED 0.75% AS PER IPC-TM-650 2.4.22.

Cleanliness

Different boards will have different cleanliness requirements. If you are building low power devices that are designed to operate on a battery for a long time then you will want to ensure that the board is very clean, otherwise any residue can cause a current path and shorten battery life. There's considerable debate in the industry about how to measure cleanliness. IPC-6012 requires using Resistance of Solvent Extraction (ROSE) but many in the industry find issue with that, and recommend using Ion Chromatography instead. Again, we want to reference a test method for how to measure cleanliness so we specify IPC-5704 which requires Ion Chromatography and defines the maximum amount of residue of various types.

PCB SHALL COMPLY WITH IPC-5704 CLEANLINESS REQUIREMENTS.

Electrical Test

Unless you are building a very low cost board, you should always have the bare boards electrically tested. This verifies that the fabricated PCB matches your netlist. This is done with very fast flying probe testers, which test for continuity between the pads.

ALL BOARDS ARE TO BE 100% ELECTRICALLY TESTED USING SUPPLIED IPC-D-356 NETLIST ACCORDING TO IPC-9252, CLASS 2.

UL Marking & Vendor Markings

It's fairly standard to require a UL marking on the PCB, to verify that there is traceability. The PCB fabricator will also typically want their own markings on the PCBA, like a job number or date code. We require all vendor markings to be in silkscreen (not metal) so that we can ensure that they don't put metal where it is not wanted, like beneath an antenna, or in a keep-out area.

FINISHED BOARD SHALL MEET THE REQUIREMENTS OF UL796 WITH A FLAMMABILITY RATING OF UL 94V-0 OR BETTER. VENDOR'S UL LOGO AND/OR DESIGNATION AND DATE REQUIRED, TO BE LOCATED IN SILKSCREEN ON THE SECONDARY (BOTTOM) SIDE OF PCB. ANY VENDOR MARKINGS ARE TO BE SILKSCREEN ONLY, BOTTOM SIDE. NO COPPER MARKINGS BY VENDOR ARE ALLOWED.

Miscellaneous

If you have internal cutouts then you should specify the maximum radius used in the cutouts. Otherwise your nice rectangular cutout will end up having significantly rounded corners and whatever needs to go in there may not fit.

MAXIMUM RADIUS ON ALL INSIDE SHARP CORNERS TO BE .045" (1.15MM) MAX.                                                   

ALL DIMENSIONS ARE +/-0.010" (0.254MM)