Section 15 – PCB Design: Creating a Document Package
This is the fifteenth section in the back-to-school series for PCB Designers and those who may want to know more about it.
Contents
- Creating a Document Package
- Standard Fabrication Notes
- Assembly Drawings
- Projecting Views
- Standard Assembly Notes
- Graduate School Zone - Formatting Data
Creating a Document Package
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 multi-layer board targeted for consumer electronics with components on both sides and controlled impedance on inner as well as outer layers.
Flexes or high reliability boards would have significantly different call-outs. In any case, there needs to be traceability for all of the attributes of the drawing. If you’re calling out a specific process like cleaning with “ultra pure water”, then it should be accompanied by a requirement for a Certificate of Conformance. Otherwise, who can tell if the process was followed?
Note 1A 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 the class 2 (as shown) but not want to allow the 90 degree 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 you ask for that option, you then have to make sure that it is possible by increasing the pad size so that the tolerance stack makes sense.
Figure 1. Image Credit: Author - A gleaming high-tech sensor factory
Standard Fabrication Notes
Notes: unless otherwise specified.
- Standards:
a. Fabricate PCB in accordance with the current revision of IPC-6012, class 2.
b. Interpret dimensions and tolerances in accordance with the current revision of asme y14.5m.
c. Do not scale drawing - Material:
a. Laminate and prepreg material shall be woven e-glass / epoxy in accordance with ipc-4101/126 or equivalent.
b. Equivalent material shall be rohs compliant, halogen free with a minimum tg of 170 degrees c and approved by company.
c. Thickness of individual copper clad sheets shall be as defined in stack-up diagram - Flatness:
a. Bow and twist of assembly sub-panel or singulated pwb shall not exceed .025 cm per cm.
b. Test in accordance with the current revision of ipc-tm-650 2.4.22 - Etch geometry:
a. Measure width from the base of the metallization.
b. Minimum line width: 0.nn mm outer, 0.nn mm inner layers.
c. Finished line width and terminal area shall not deviate from the 1-to-1 master pattern image by more than +/- 0.025 mm or 20%, whichever is less. - Surface finish: (select appropriate finish)
a. Enepig plating in accordance with the current revision of ipc4556. Exposed metal shall have 118–236 micro inches electroless nickel, 2–6 micro inches electroless palladium, and 1.2 micro inches gold.
b. Enig plating per current revision of IPC-4552. Exposed metal shall have 118–236 micro inches electroless nickel and 2–5 micro inches gold. - Destructive testing:
a. Micro section sample and report shall be provided to company design engineering.
b. Solder sample processed through lead-free soldering shall be included with each shipment.
c. X-out panels may be used for solder sample. - Holes:
a. Plating in holes shall be continuous electrolytic copper with 0.025 mm minimum barrel thickness.
b. Minimum finished hole size: 0.nn mm
c. Hole size measured after plating.
d. See drill chart for finished hole size and tolerance.
e. All holes shall be located within 0.08 mm of true position as supplied in cad data. - Solder mask:
a. 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.
b. Color: matte green
c. Liquid photo-imageable (lpi) 0.001 mm to 0.002 mm thickness, halogen free
d. No bleed-out allowed over exposed smd pads.
e. No exposed traces. - Silkscreen:
a. Silkscreen primary and secondary side with white epoxy, non-conductive, non-nutrient ink.
b. Any unspecified stroke width shall be 0.13 mm
c. Clip silkscreen away from any exposed metal.
d. Vendor date code, logo, ul and any additional marking to be located on the secondary side.
e. Bag and tag acceptable for pwbs that are too small for marking. - Remove all burrs and break sharp edges r0.01 min.
- Non-destructive evaluation:
a. All pcbs shall pass 100% electrical test using supplied ipc-356 netlist in accordance with current revision of ipc-9252, class 2.
b. Certificate of conformance shall be supplied with each shipment. - X-outs:
a. X-out boards that do not meet all specifications using permanent marking on both sides of the affected pcb.
b. Panels that do not have any x-outs shall be packaged together.
c. Panels that have n or fewer x-outs shall be packaged separate from non-x-out panels.
d. Panels with more than n x-outs shall be rejected. - Packaging requirements:
a. Pwbs shall be packaged in vacuum sealed inner containers.
b. Outer containers shall be sufficient to prevent damage during shipping and handling. - Impedance (all tolerances +/- 10%)
a. All 0.nn mm wide traces on outer layers shall be 50 ohms.
b. All 0.nn mm wide/0.nn mm space pairs on outer layers shall be 90 ohms.
c. All 0.nn mm wide/0.nn mm space pairs on inner layers shall be 90 ohms.
d. 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.
Assembly Drawings
Figure 2. Image Credit: Velodyne - Assembly drawings come in two main types, SMT assembly and 2nd-operation drawings like this one. Note that the details use third angle projection.
Another inspection document is the assembly drawing. The primary goal is to show what the finished assembly looks like. If you read my blogs, 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. I urge you not to get yourself wrapped around that axle.
Projecting views
There will always be a top side plan view of the PCB outline. It may also be augmented with a side view or a cutaway view to show details such as the beveled edge for gold fingers. The United States along with Australia and possibly some other locations use what is called third angle projection while first angle projection is the norm in Europe and elsewhere.
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 that the side you see in the edge view faces towards the plan view. On the other hand 1st Angle Projection would invert the imaginary bowl and allow the additional views to slide off the bowl.
Figure 3. Image Credit: Practical Machinist - The graphics in the upper left corner of these views are included in the title block to establish the projection of various views.
Standard Assembly Notes
Notes unless otherwise specified.
- Interpret drawing in accordance with asme y14.5m 1994.
- Workmanship shall be in accordance with the current revision of j-std-100 and ipc-hdbk-001
- Inspection shall be in accordance with the 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
Graduate School Zone - Formatting Data
We have been using Gerber data for about as long as we have been using computers to aid us in our design efforts. Gerber data has evolved to allow unlimited apertures. Originally, this was a mechanical process that involved aperture wheels with 24 different openings that were used to generate the photo tools.
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. 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 ok as long as Valor was a stand-alone enterprise.
The ECAD industry has come together around a new specification that adds more intelligence and is not encumbered by commercial interests. This new thing is the IPC-2581 spec. If you want to have a good time, hook up with an outfit that will talk 2581 with you. The artwork still has to 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 revision C of IPC-2581, manufacturing partners can provide technical queries in 2581 format making it very easy to cross probe, track, resolve, approve, reject TQs.”
You’ll still find many fab shops relying on Gerber data since they have a different CAM tool. A majority of the high-capability shops are using Valor and prefer that. It will be up to us, the design community, to help launch the new CAD-neutral IPC format.
Related Documents:
- 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