Communicating the design intent, clearly and concisely.
The CAD system can do a lot for you; then you’re on your own. Eyeballing the layers two or three at a time will help you find the hidden traps. A camera-ready board is just the beginning. Documenting the PCB requirements with dimensions and other details, including hole chart(s), stack up diagram(s), a list of intentional shorts, etc., puts the necessary guardrails around the fabrication and assembly.
Fabrication notes will change with the technology used for the PCB. The general thrust of this list of example notes is for a multilayer board targeted for consumer electronics with components on both sides and controlled impedance on inner- and outer layers.
Flex circuits or high-reliability boards would have significantly different callouts. In any case, all the attributes of the drawing need traceability. When calling out a specific process, such as cleaning with “ultra pure water,” it should be accompanied by a requirement for a Certificate of Conformance. Otherwise, who could tell if the process was followed?
Note 1A (below) covers a lot of ground by itself. The notes that follow are best used to describe options within the spec and exceptions to the spec. For instance, you may call for “Class 2 (as shown)” but do not want to allow 90° break-out of the drilled hole from the pad. In that case, a note calling for “no break-out, tangency permitted” would be necessary and sufficient for that exception to the general Class 2 fabrication rules. If that option is requested, make sure it is possible by increasing the pad size so that the tolerance stack makes sense.
Figure 1. A gleaming high-tech sensor factory.
Standard fabrication notes (unless otherwise specified).
- Standards:
- Fabricate PCB in accordance with current revision of IPC-6012, Class 2.
- Interpret dimensions and tolerances in accordance with the current revision of ASME Y14.5.
- Do not scale drawing.
- Material:
- Laminate and prepreg material shall be woven “E” glass/epoxy in accordance with IPC-4101/126 or equivalent.
- Equivalent material shall be RoHS compliant, halogen-free, with a minimum Tg of 170°C and approved by company.
- Thickness of individual copper-clad sheets shall be as defined in stack-up diagram.
- Flatness:
- Bow and twist of assembly subpanel or singulated PWB shall not exceed 0.025cm per cm.
- Test in accordance with current revision of IPC-TM-650, method 2.4.22.
- Etch geometry:
- Measure width from the base of the metallization.
- Minimum line width: 0.nn mm outer, 0.nn mm innerlayers.
- Finished line width and terminal area shall not deviate from the 1:1 master pattern image by more than +/-0.025mm or 20%, whichever is less.
- Surface finish (select appropriate finish):
- ENEPIG plating in accordance with current revision of IPC-4556. Exposed metal shall have 118 to 236 microinches electroless nickel, 2 to 6 microinches electroless palladium, and 1.2 microinches gold.
- ENIG plating per current revision of IPC-4552. Exposed metal shall have 118 to 236 microinches electroless nickel and 2 to 5 microinches gold.
- Destructive testing:
- Microsection sample and report shall be provided to company design engineering.
- Solder sample processed through lead-free soldering shall be included with each shipment.
- X-out panels may be used for solder sample.
- Holes:
- Plating in holes shall be continuous electrolytic copper with 0.025mm minimum barrel thickness.
- Minimum finished hole size: 0.nn mm.
- Hole size measured after plating.
- See drill chart for finished hole size and tolerance.
- All holes shall be located within 0.08mm of true position as supplied in CAD data.
- Solder mask:
- Solder mask over bare copper (SMOBC) on primary and secondary sides using supplied artwork in accordance with current revision of IPC-SM-840 type B.
- Color: matte green.
- Liquid photoimageable (LPI) 0.001mm to 0.002mm thickness, halogen-free.
- No bleed-out allowed over exposed SMD pads.
- No exposed traces.
- Silkscreen:
- Silkscreen primary and secondary side with white epoxy, nonconductive, non nutrient ink.
- Any unspecified stroke width shall be 0.13mm.
- Clip silkscreen away from any exposed metal.
- Vendor date code, logo, UL and any additional marking to be located on secondary side.
- Bag and tag acceptable for PWBs that are too small for marking.
- Remove all burrs and break sharp edges R0.01 min.
- Nondestructive evaluation:
- All PCBs shall pass 100% electrical test using supplied IPC-356 netlist in accordance with current revision of IPC-9252, Class 2.
- Certificate of conformance shall be supplied with each shipment.
- X-outs:
- X-out boards that do not meet all specifications using permanent marking on both sides of affected PCB.
- Panels that do not have any X-outs shall be packaged together.
- Panels that have n or fewer X-outs shall be packaged separately from non-X-out panels.
- Panels with more than n X-outs shall be rejected.
- Packaging requirements:
- PWBs shall be packaged in vacuum-sealed inner containers.
- Outer containers shall be sufficient to prevent damage during shipping and handling.
- Impedance (all tolerances +/-10%):
- All 0.nn mm wide traces on outer layers shall be 50Ω.
- All 0.nn mm wide/0.nn mm space pairs on outer layers shall be 90Ω.
- All 0.nn mm wide/0.nn mm space pairs on inner layers shall be 90Ω.
- Vendor may adjust design geometries up to +/-20% to achieve target impedance. Adjustments beyond 20% of line width, spacing or dielectric thickness shall require approval from company engineering.
FIGURE 2. Assembly drawings come in two main types: SMT assembly and (like this one) second-operation drawings. Note that the details use third angle projection. (Source: Velodyne)
Assembly drawings. Another inspection document is the assembly drawing (FIGURE 2). The primary goal is to show what the finished assembly looks like. If you read my columns, you probably know that I insist that this is a what-is, not a how-to document. How-to documents are subject to frequent revision as the process evolves through continuous improvement. Don’t get yourself wrapped around that axle.
Projecting views. There will always be a topside plan view of the PCB outline. It may be augmented with a side or cutaway view to show details, such as the beveled edge for gold fingers. The US, Australia and possibly some other locations use what is called “third angle projection,” while “first angle projection” is the norm in Europe and elsewhere (FIGURE 3).
For third angle projection, imagine the board at the bottom of a bowl. The top and side views are created by sliding and rotating the view up the sides of the bowl, so the side seen in the edge view faces toward the plan view. On the other hand, first angle projection inverts the imaginary bowl and allows the additional views to slide off the bowl.
Figure 3. The graphics in the upper left corner of these views are included in the title block to establish the projection of various views. (Source: Practical Machinist)
Standard assembly notes (unless otherwise specified).
- Interpret drawing in accordance with ASME Y14.5M, 1994.
- Workmanship shall be in accordance with current revision of J-STD-001 and IPC-HDBK-001.
- Inspection shall be in accordance with current revision of IPC-A-610, Class 2.
- The controlling document for component placement shall be xy-nnn-nnnn-nn.
- Mark dash and revision level in permanent black ink as shown.
- Affix barcode, date code and serial number labels on secondary side as shown. Bag and tag acceptable for assemblies that are too small for labels.
- Company reference documents as follows:
-
- Bill of material nnn-nnnn-nn
- Placement file nnn-nnnn-nn
- Paste stencil nnn-nnnn-nn
- Schematic nnn-nnnn-nn
- FPGA programming nnn-nnnn-nn
- Test procedure nnn-nnnn-nn
- Whatever else is relevant and not documented elsewhere.
Formatting data. The industry has used Gerber data about as long as it has used computers to aid our design efforts. Gerber data has evolved to permit unlimited apertures. Originally, this was a mechanical process that involved aperture wheels with 24 different openings used to generate the phototools.
The aperture wheels evolved to an electronic equivalent. Every PCB design was taped out with a separate file for the apertures. The aperture list is now embedded with each artwork layer to make it more resilient. The information conveyed in this standard is just the raw geometry. File names supplemented with a readme.doc help the fabricator determine how to use the data.
Eventually, a de facto standard came along from Valor (now part of Siemens). It is native to the software used in the front-end of the fabrication process. The format is called ODB++ and it has some intelligence along with the geometry data. Fabrication and assembly data can be combined in a single archive. Most PCB factories prefer this type of data. This was acceptable when Valor was a standalone enterprise.
The ECAD industry has come together around a new specification that adds more intelligence and is not encumbered by commercial interests. This new spec is IPC-2581. Want a good time? Hook up with an outfit that will talk IPC-2581 with you. The artwork still must be camera-ready; it’s not doing your drawings. What it will do is a thorough extraction and allow the designer to define what goes to the manufacturing partner.
According to my colleague, Hemant Shah, “IPC-2581 not only makes design data handoff efficient, it also makes manufacturing the board more efficient. IPC-2581 connects to IPC-CFX to help with smart factory automation. With IPC-2581 revision C, manufacturing partners can provide technical queries in the 2581 format, making it very easy to cross-probe, track, resolve, approve and reject TQs.”
Many fabricators rely on Gerber data because they have a different CAM tool. A majority of high-capability shops use ODB++ and prefer it. It will be up to us, the design community, to help launch the new CAD-neutral IPC format. •
Related documents. Standards and specifications that cover PCB documentation and electronics data transfer include:
- IPC-D-325, Documentation Requirements for Printed Boards.
- IPC-2581, Generic Requirements for Printed Board Assembly Products Manufacturing Description Data and Transfer Methodology.
- IPC-D-310, Guidelines for Phototool Generation and Measurement Techniques.
- IPC-2514, Printed Board Manufacturing Data Description.
- IPC-2513, Drawing Methods for Manufacturing Data Description.
- IPC-2615, Printed Board Dimensions and Tolerances.
John Burkhert Jr. is a career PCB designer experienced in military, telecom, consumer hardware and, lately, the automotive industry. Originally, he was an RF specialist but is compelled to flip the bit now and then to fill the need for high-speed digital design. He enjoys playing bass and racing bikes when he’s not writing about or performing PCB layout. His column is produced by Cadence Design Systems and runs monthly.
