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)

PCB Fabrication Notes for 2016

Have you looked at your PCB fabrication notes lately? I recently went through our standard set of notes and did a ton of research to see what is best. This is the first of a two-part post about standard PCB fabrication notes, explaining the reasoning for each note. Your requirements may be different, but these are based on what works best for our projects. Most of our projects are fairly run of the mill, industrial type products, 2-4 layers, 6/6 width/spacing, etc. Nothing too fancy, but need to be decent quality and last a few years. Nowadays everything is going RoHS, so we include that into our standard drawing package too.

When developing standard notes, be sure to talk to your CM and PCB vendor - they have lots of good advice since they've seen what works and doesn't work. But keep in mind that they're goals may not be the same as yours.

Standards

The Association Connecting Electronics Industries (aka IPC) has many standards that you can reference when specifying PCBs. There are many advantages of referencing a standard instead of specifying every little detail about a board:

1. The standards reflect industry best practices, and are constantly being updated as technology changes
2. The vendor will be more familiar with a standard than your individual requirement
3. In the event of a dispute, you can have a 3rd party verify standard compliance easily

The current revision of standards can be checked on this page. To ensure that your product is always being built with the most recent version, you can either manually update the note each time a standard is changed, or just add a note requiring the current version. Note that even in the standards, some specifications are "As Agreed Between User and Supplier", or AABUS for short.

IPC-A-600 vs. IPC-6012

There are two standards frequently specified when ordering PCBs: IPC-A-600 and IPC-6012. IPC-A-600 is an inspection criteria and defines how the board should look when it is complete. It is less stringent than IPC-6012, and is usually the governing specification for prototype PCB houses. On the other hand, IPC-6012 defines how the PCB is constructed, and goes into much greater detail. It also includes requirements for inspections and coupons. Inside IPC-6012, there are three main classes, depending on how stringent the standard should be:

• Class 1, low quality
• Class 2, industrial quality
• Class 3, high performance

If you're not making cheap toys or avionics, then you'll probably want to use IPC-6012, Class 2. Refer to this chart for a comparison between the three main classes.

Summary

The way that we specify the standard to use is:

1. STANDARDS: USE CURRENT REVISION OF ALL STANDARDS. FABRICATE PCB ACCORDING TO IPC-6012, CLASS 2.

Material

Do you specify the PCB material using something like the following?

• "Hi-Temp FR-4, 170Tg"
• "FR4, 135Tg"
• "Rogers 4000"

If so, then you are making life more difficult for yourself. The IPC has developed standards for materials. There are many different types that are specified (called "slash sheets" in IPC parlance) but using these can make your life much easier for the following reasons:

• Exactly defines key specifications
• Easier for PCB fabrication houses
• No single-vendor lock-in

The IPC-4101 standard (Specification for Base Materials for Rigid and Multilayer Printed Circuit Boards) defines the various types very specifically. These define the characteristics of the material in great detail, including:

• Reinforcement (paper, fiberglass, etc.)
• Resin (phenolic, epoxy, etc)
• Copper peel strength
• Moisture absorption
• Tg, Td, CTE

RoHS Compliance

When it comes to lead-free compliance for PCB material, things get confusing. A PCB type may in and of itself be lead-free, but it may not be able to survive the higher process temperatures of lead-free assembly. So it gets confusing, but suffice to say that we want a material that is both lead-free and is compatible with a lead-free process.  There are many specifications to look at, but the most important are the glass transition temperature (Tg) and minimum decomposition temperature (Td).

Glass transition temperature is defined in IPC-TM-650, 2.4.24C and is the temperature where the rigid PCB becomes flexible. Materials with a higher Td are more stable, but you don't get something for nothing: these materials have some drawbacks as I'll explain below.

The minimum decomposition temperature is defined as the temperature at which point the weight of the PCB material changes by 5%, according to IPC-TM-650, 2.4.24.6.  These relate to the T260 or T288 characteristics, which is the time until delamination at 260C or 288C, respectively.

The higher-end phenolic materials (Tg > 170C & Td > 340C, aka IPC-4101/126 or /129 have great thermal properties but have poor moisture absorption and copper-to-laminate adhesion. So you can have your cake but you can't eat it too. Specifically:

• Moisture Absorption: Standard 130Tg FR-4 materials have moisture absorption of 0.20% vs. 0.45% for the fancier high Tg phenolics.
• Peel Strength: Standard 130Tg FR-4 materials have peel strength of 8-10 lbs. vs. phenolics have a peel strength of 3-4 lbs.

For example, compare Isola DE104 (135Tg, 315Td, /21) and Isola 370HR (180Tg, 340Td, /126): the former has peel strength of 9.0 lb/inch vs. 6.5 lb/inch for the higher temperature material. When it comes to IPC-4101 grades that are compliant with lead-free processing, there are generally four groups of material. Refer to the IPC standard for the details, or this handy chart.

• Low temp: /23, /24
• Ok (110C Tg): /101, /121 - note, these have largely been ignored in US
• Better (150C): /99, /124 (these are best for our applications)
• High: (170C): /126, /129

Summary

The way that we specify the PCB material is:

2. MATERIAL: COPPER CLAD PLASTIC SHEET PER IPC-4101/99 OR IPC-4101/124 ROHS COMPLIANT.

Board Construction

Next, we have several requirements to ensure that the PCB is fabricated the way we want it:

RoHS Compliance Clause

We have an omnibus clause stating that everything must be RoHS compliant, and defining exactly what that means. This is good just as a double check to ensure that we don't miss anything. The vendor will alert us if we have something that is not RoHS compliant.

   ALL PARTS & MATERIALS SHALL MEET THE RoHS DIRECTIVE 2011/65/EU.

Board Stack-Up

Define the thickness of the PCB, if not defined in the layer stack-up. Try to avoid having non-stand thicknesses. Be sure to include a tolerance. Just to avoid confusion, I also like to define that the board stack-up should be according to the table in the PCB fabrication drawing:

   OVERALL BOARD THICKNESS TO BE 0.062 INCHES +/- 0.005 INCHES.
   REFER TO LAYER STACK-UP TABLE FOR LAYER CONFIGURATION. ALL LAYERS VIEWED FROM THE PRIMARY (COMPONENT) SIDE.

Hole Dimensions

Most of this is called out in IPC-6012, but we specify some here to be more exact. In IPC-6012 it sometimes says "this parameter is AABUS, but if not specified then standard X applies". When it comes to hole location tolerance, if none is specified then IPC-2221 applies. It requires 0.00984 for Type A,  0.0079" for Type B, and 0.00591 for Type C.

   UNLESS OTHERWISE NOTED ALL HOLE DIMENSIONS APPLY AFTER PLATING.
   ALL HOLES SHALL BE LOCATED WITHIN 0.006" OF TRUE POSITION AS SUPPLIED IN CAD DRILL DATA. LAYER TO LAYER REGISTRATION SHALL BE WITHIN 0.005".

Hole Wall Thickness

IPC-6012 Class 2 calls out 0.00071" minimum and 0.00079" standard for plating thickness, but we want to ensure that we have plenty of copper.

ALL HOLES SHALL HAVE A WALL THICKNESS OF 0.0008".

That's all for now, next we'll talk more about surface finish, cleanliness, and testing.