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.
StandardsThe 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:
- The standards reflect industry best practices, and are constantly being updated as technology changes
- The vendor will be more familiar with a standard than your individual requirement
- 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-6012There 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
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.
MaterialDo you specify the PCB material using something like the following?
- "Hi-Temp FR-4, 170Tg"
- "FR4, 135Tg"
- "Rogers 4000"
- Exactly defines key specifications
- Easier for PCB fabrication houses
- No single-vendor lock-in
- Reinforcement (paper, fiberglass, etc.)
- Resin (phenolic, epoxy, etc)
- Copper peel strength
- Moisture absorption
- Tg, Td, CTE
RoHS ComplianceWhen 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, 22.214.171.124. 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.
- 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
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 ConstructionNext, we have several requirements to ensure that the PCB is fabricated the way we want it:
RoHS Compliance ClauseWe 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-UpDefine 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.
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 ThicknessIPC-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.