Panel Geometry

• Panel (or board) must have two (2) parallel edges preferably running the length of the panel to accommodate the handling rails of various manufacturing equipment. Other shapes may require special tooling and/or carriers
  

Board Thickness

• Standard board thickness is 0.062” [1.6mm]
• Thickness less than 0.031” [0.8mm] may require special tooling.
• Thickness greater then 0.093” [2.4mm] may require special tooling.

Panel Size

• 8” X 11.5” [203.2mm X 292.1mm] optimal.
• Less than 2” X 4” [50mm X 101.6mm] should be panelized else may require special tooling.
• Maximum panel size for standard equipment is 14” X 18” [356mm X 457mm].

Gerber Layers

• Verify file name matches actual Gerber layer.
• Layer weights should be symmetrical from the core.
• Stack-Up window designed into PCB allows for visual verification that the layers are in the correct order.
• If solderwave masking is required, add a peelable solder mask layer and let the board house apply it. This will cost less than applying it by hand.
• WEEE symbol "crossed out wheelie bin" etched in copper. (Electronics disposal and recycling services are Free to REDCOM EMS customers.)

Edge Clearance

• It is important to realize edge clearance is the distance from the edge of the board to the Component Outlines. Many component bodies are wider than the pads that they are being placed on (i.e. electrolytic capacitors). Placing tolerance should also be taken into consideration.
• If single sided: 0.150" [3mm] "Do Not Populate" zone is required along the edges that will support the assembly as it travels through conveyors, clampers, depanel or other handling.

• If two sided: The first side to be populated (usually bottom side) should have a clearance of 0.190" [4.826mm] to accommodate the oven chain during reflow. (Must determine direction of travel and if it will be properly supported).
• UL requires minimum of 0.060" [1.542mm] clearance between any conductor and the edge of a PCB.

Tooling Holes

• Three corners are optimal for fixturing.
• 0.197" [5mm] from each edge.
• Non-plated
• Diameter; .0158" [4mm]

Depanelization

• Preferred: Straight edges with no overhanging components, V-Score 1/3 depth each side at 45 degrees.
• Otherwise: Pre-route under the overhanging components and use perforated tabs "mouse bites".
• Look For: No chips within 0.188"[4.8mm] of a V-Score. No mouse bites within 0.100"[2.5mm] of drilled holes or traces.

Fiducials

• Minimum: Three on opposite corners of the panel.
• Shape: Solid Round. 0.039"-0.118" [1mm-3mm] diameter with 0.020"[0.5mm] mask relief.
• Fiducials must be located on BOTH top and bottom side (even singl-sided assemblies) to accommodate Flying Probe.

Component Fiducials (Local Fiducials)

• Recommend 2 per fine pitch part (<=20 mil lead pitch) and all QFPs, BGAs, LGAs & QFNs.
• Opposite corners
• Shape: Round preferred. 0.039” – 0.118” [1mm – 3mm] OD with 0.020” [0.5mm] mask relief to provide contrast.
• No Fiducial should be located under any component.

Solder Mask

• Liquid Photo Imageable (LPI)  with laser defined features is preferred. Max t=0.003" [.076mm]
• Soldermask Dams between ALL fine pitch pads down to and including 6mil. (Do Not "window" out the mask between fine-pitch pads)
• Prefer unmasked via hole except when via is under a component or within 0.100" of a through hole lead. Unmasked vias provide more access points on a Flying Probe tester.
• Plugged vias allow for better vacuum utilization on a clamshell tester. Should not plug both sides of a via hole.

Materials

• High Temperature FR4 preferred. Other material may require special processing.
• Symmetrical stackup of 2 to 24 layers with evenly distributed copper to reduce warpage.
• Finish: Immersion Gold over Nickel (ENIG)

Weights (standard)

• 1 oz.   Foil /  .0040" or greater trace width and space
• 2 oz.   Foil /  .0055" or greater trace width and space
• 3 oz.   Foil /  .0075" or greater trace width and space
• 4 oz.   Foil /  .0095" or greater trace width and space

Silk Screen

• Should be present
• Weight, Size and Font should be legible
• Part orientation should be clearly designated with part outlines where appropriate.
• All locations should have a reference designator silk screened.
• All silkscreen should be visible after component placement.

Component Spacing

• Adequate clearance for SMT placement (see IPC-SM-782).
• Adequate cut/clinch clearance for through-hole auto insertion.
• Adequate clearance for inspection, cleaning, and/or rework.
• 0.100" [2.5mm] clearance around 16mil (or smaller) pitch land patterns required for step-down on screen-print stencil.

Thermal Balance

• Components with high thermal mass (i.e. PLCCs) should be replaced with thin packaged component or spaced about 0.350"-0.400" apart.
• Plane layers should not contain large voids. Surface area of Power and Ground planes should be distributed as evenly as possible and on symmetrical layers. This will help minimize warp and signal noise.

Component Placement

• Components should be oriented in the same direction to aid inspection efforts
• Through-hole components should not be placed on both sides of the PCBA.
• Components should not be placed on top of other components making them inaccessible for rework or inspection.
• Is the board double sided when it can be single sided?
• Is placement density affecting thermal properties or ability to inspect?
• Tall components should remain on topside to reduce damage during handling.

Modifications

• If this assembly is a revision of a previous design, verify all wires, trace cuts, kluges and any other modifications have been incorporated into this design.

Component Process Compatibility

• Components should be able to withstand 250C for 10 sec. 260C is Ideal.
• Through hole components that meet this criteria are capable of being assembled using Pin in Paste methods.

Component Technology

• If assembly is primarily SMT with few through hole or vice versa, effort should be made to convert the assembly to all one technology. Doing so will reduce the number of manufacturing processes.
• Components with tight positional tolerance or that require hand placing should have guide posts.
• Tape and Reel or Matrix tray packaging options should be available for all parts.
• If planning a pin-in-paste process, Through hole parts such as headers and connectors should not sit flush to the board. Stand-off options are usually available for each part. (See Intrusive Reflow Requirements)
• Metalized components should have insulators where minimum electrical clearance with traces or other components may be violated.

Arrays & Leadless Technology

• Area array components (BGAs, LGAs, QFNs) are preferred over fine pitch leaded components. Utilizing area arrays can help recover valuable real estate on your PCB.
• Placement Verification: Silkscreen outline of component with polarity indicator.
• Perimeter Clearance: 0.125"[3.2mm] no populate zone along BGA perimeter to accommodate both rework nozzles and endoscope inspection.
• X-Ray Inspection: Prefer no parts placed on opposite side of assembly under component to aid with x-ray inspection and allow support if rework is required.
• Pad Type: Copper defined pads are preferred. Mask defined pads are acceptable.

Adjustable Components

• Use fixed value components where possible. Adjustable components require teaking during test and may change value over time. (i.e. Potentiometers).

Connectors

• Connectors should be locking and quick disconnect.

Press Fit Technology

• Preferred when the component must mount to the bottom side of the assembly.
• Should also be used if it will eliminate the solder wave process.
• Rule of Thumb: Pressfits require about 8 lbs of force per pin of the component. Capable insertion equipment should be verified prior to design.

Networked Components

• RNETs CNETs, et. al. should be utilized where like components are in close proximity to each other. Doing so reduces machine cycle time during manufacturing.

PCB Thickness

• 0.062"[1.6mm] or less is ideal and minimizes required paste deposit.
• Greater than 0.062"[1.6mm] may require SMT Solder preforms.

Process Compatibility

• All components should withstand 250C for 10sec minimum. 260C is Ideal.

Component Underside Clearance

• Intrusive components that do not have stand-offs will squeeze out paste, possibly causing solder shorts during reflow. Stand-offs will allow paste to reflow smoothly into the apertures as it is intended.

Plated Through Hole Clearance

• Nothing that can wick away solder (SMT pad, open via hole) should be allowed within the component outline.

Thermal Mass

• Components with low thermal mass will follow the curve of the oven profile more efficiently.
• Components with high thermal mass will require more heat and greater delta T which can possibly overheat other components on the assembly.

Component Lead Considerations

• Lead Length should protrude from the bottom side of the assembly by 0.030"-0.060"[0.8mm-1.6mm]
• Cross sectional shape of lead should be round or square. U-Shaped leads do not work well.
• Lead diameter should be approximately .019"[0.5mm] smaller than the diameter of the hole.

Volume

• Wave Solder is ideal for high pin count, high volume soldering.
• Selective Solder is more appropriate for fewer pin counts, high mix, low-mid volumes.

Component Orientation

PCB direction of travel through a wave solder machine should be considered during the design process. Components that come into contact with the wave should be oriented as follows:

• SMT chips should be parallel with the wave.
• SMT ICs should be parallel with the direction of travel to promote lead to lead drainage.
• T/H ICs should be parallel with the direction of travel to promote pin to pin drainage.

Aperture Size

• Apertures for through hole technology should be 0.019"[0.5mm] larger than the leads of the components that are being populated. This allows for automation of the insertion process.

Solder Thieves

• ICs that are being wave soldered and T/H devices with a lead pitch of <0.100"[2.54mm], should have a set of "dummy pads" on the trailing end of the component as it travels through the wave. These pads aide in drainage, pulling solder away from the part, thus reducing solder bridging. 
• Solder thieves should be 0.030"[0.76mm] away from the last pad or annular ring on the device.

Thermal Relief

• Through Hole leads connecting to Power or Ground planes should have thermal relief designed in. This reduces poor top solder flow and insufficient solder.

Solder Wave Masking

• If Bottom side SMT components are on the board, fixturing is recommended.
• If specific apertures are to be left unsoldered and no fixture is used, Peelable Solder mask may be applied by the board house. This generally will cost less than doing it by hand during board assembly operations.

Wave Solder Fixture Requirements

• 0.100"[2.54mm] space between bottom side SMT pad edge and the edge of the through hole land is ideal. This allows for sturdy fixture walls to maintain good gasketing between the board and the fixture. Less than this space may require the use of special materials such as titanium inserts.
• Component height should not exceed 0.200"[5.08mm] else special fixture material may be required.

Standardize

• Use off of the shelf Hardware.
• Reduce Line Items by minimizing nuts, bolts, washers etc. Utilize the same hardware in as many locations as possible.

Adhesives

• Hardware is preferred over adheasives whenever possible.
• Thermal pads preferred over thermal grease.
• Specify screws with pre-applied threadlocker if threadlock is required.

Reworkability

• Screws preferred over rivets
• Broaching preferred over swage fasteners
• Philliips & Hex driver preferred over Slotted or Torx screws.
• Hardware must be accessible and not require special tooling.

Labels

• Should all be oriented such that they are legible in a normal operating environment. (Not upside down or sideways to the user)
• PCBA labels must not cover test points on the assembly.
• Lables should be located on the assembly such that the end user can easily obtain relevant information that may be required in the field.

Metalwork

• Finish:
• Plating: Zinc plating should meet or exceed the testing requirements of ASTM-B-633, Type II, SC3, Blue-Bright to clear, using Trivalent Chromate (or equivalent) for RoHS compliance.
• Top coats of silicate, wax, acrylate or any other material are not recommended.
• Powdercoat is preferred over paint.

Access Points

Prefer more than 1 access point per net.

Order of Preference

• Test Pads: Min Diameter of 0.035"
• Vias (unmasked)
• Exposed Traces
• Connector Pins
• Component Pads

Power Test Points

• One for each 2-4 square inches of board surface.
• Multiple power and ground test points.

Flying Probe VS. Clamshell

• Flying Probe has the flexability to quickly adapt to artwork changes. It is more suited for a High Mix-Low Volume Environment.
• Clamshell tests are generally faster than FP but Artwork changes may require a new bed of nails to test with. Clamshell testing is more suited for a high volume run.

Fiducials

• Minimum: Two on opposite ends of the panel.
• Solid Round shape preferred with 0.039"-0.118" [1mm-3mm] diameter and a 0.020"[0.5mm] mask relief.
• Fiducials must be located on BOTH top and bottom side to accommodate Flying Probe.

Test Point Criteria

• Max 40 test points per sq in
• Ideal spacing is 0.100" center to center.
• Do Not cover test points with solder mask or any protective surface coating other than the surface finish of the conductor pads.
• Test Points should be indicated in the schematics.

When submitting a Request for Quote to your Manufacturing Department or your CM, having as many of these components as possible in your information package will help eliminate questions and increase the speed and accuracy of the quote process.

• Request for Quote (RFQ): State your general requirements: IPC Class? Flux Chemistry? RoHS? Test Requirments? Quantities?
  
• CAD Output: Many times CAD can be imported directly into a machine program and/or translated such that the manufacturing process details can be generated very quickly. Supplying a CAD output can save the manufacturer substantial time in getting the product up and running.
• Gerber Files: Not to be confused with CAD, Gerber files are the individual layers of the PCB. There should be 1 file per layer. Gerber files are required to obtain a quote from the raw PCB manufacturer. They are also used to purchase SMT stencils, design any required tooling, and it is possible to program some equipment using these files.
• Centroid Data (X-Y Coordinates): Used for programming various placement machines.
• Fabrication or Drill Drawing: Illustrates bare board requirements. This information is required by the PCB manufacturer to create the PCB.
• Panel Drawing: Any panelization or breakaways that have been added to the PCB must be part of the documentation package. This drawing is critical to ensuring that the PCB panel, the stencils, fixtures, tooling, and the Machine programs all match when the product starts production.
• Manufacturing Assembly Drawings: Should contain detailed illustrations of the assembly, notes for areas of concern, and a revision history page to track changes.

• Bill of Materials (BOM): The BOM should be verified against the assembly for accuracy. Things to look for include:

  • Inconsistencies between the line quantity and the actual number of reference designators.
  • All reference designators on BOM are on the assembly drawing.
  • There is a unique reference designator for every quantity of every line item on the BOM. Hardware, wires, adhesives, etc should have reference designators.
• Mechanical Detail: Any custom metal, plastic, etc components will require detail drawings in order to be quoted.
• Test Requirements: All test instructions and required operational parameters should be provided to the manufacturer for purposes of specifying required equipment and estimating labor.