PCB WIZARDS.COM

 

Last update:

10/25/2006

  Checklist
Site Map Location FAQ

  Site Map Menu

Home
Predesign Check

 

 

 

 

   

 

Checklist for PCB Designs             

 
 

 

Board Information

  Rev

ECO Number

Board Material =  

Constraints Drawing No.  Rev

The Constraints Drawing shows mechanical clearances, mounting holes, heat sink locations, etc…

Material Thickness =

Copper thickness inner layers = oz.

Copper thickness outer layers = oz.

Number of layers =  layers

Soldermask

Silkscreen Legend  =

 

 

Product Performance Classification

PCB Producibility Level

Class 1 General Electronics Products

Level A General Design Complexity

Class 2 Dedicated Service Electronics

Level B Moderate Design Complexity

Class 3 High Reliability Electronics

Level C High Design Complexity

 

 

Board Type Classification

Environmental Requirements

Type 1 - Single Sided PCB

Unit Upper Temp Limit 

Type 2 - Double Sided PCB

Unit Lower Temp Limit 

Type 3 - Multilayer PCB without Blind or Buried Vias

Vibration requirements 

Type 4 - Multilayer PCB with Blind or Buried Vias

Humidity requirements 

Type 5 - Multilayer Metal-core PCB without Blind or Buried Vias

Heat sinking

Type 6 - Multilayer Metal-core PCB with Blind or Buried Vias

Air Flow for Convection Cooling

 

Thermal Path of Conduction Cooling

Conformal Coating

Location of Hot Components

Circuit Density L M H

Location of Heat Sensitive Components

EMI- EMC Susceptibility, or Radiation

 

ESD Handling Requirements

 

 

 

 

 

Remember - Checking requires putting on your thinking cap and putting yourself in the shoes of the manufacturer, assembler, and end user or customer. The human engineering aspects of design require that you be able to put the part on the board with a tool or your fingers and still have room to do so. You should never have to remove a part to get at another part. Good design takes into consideration the sequence of assembly as well as the tooling requirements. After the board is assembled, it must be tested. Plan for the type of tests to be required, leave ample space for test probes or pogo pins if you have a bed of nails test fixture. Remember when making changes to an existing board how the test fixture or tooling will be affected by the changes to the board.... component clearances, heights, spacing, electrical voltage spacing... etc.

Safety requirements... look at Shock hazard, and Fire Hazards. Is the material flame retardant? The end result from manufacturing must conform to your fabrication specs... did you specify it correctly and completely? If you cut and paste notes from another design, did you check to make sure they are still valid?  Do you need test points or a JTAG test connector? How will you get heat out? Will the board survive in the hot and cold environments it will be exposed to? How about Vibration? Have you specified the correct materials, how will you de-panel the boards after they are assembled in panel form? Do you need test coupons? Etc.. Etc...

 

Fabrication Notes: (Examples)

NOTES: UNLESS OTHERWISE SPECIFIED

  1. INTERPRET DRAWING, DIMENSIONS, AND TOLERANCES PER ANSI Y14.5M.  DIMENSIONS ARE IN INCHES [MM].
  2. MATERIAL: COPPER CLAD PLASTIC SHEET PER IPC-4101/26 (TYPE GFN, NEMA FR4) 170 deg C Tg MIN.
  3. LAMINATE USING B-STAGE PRE-PREG MATERIAL PER IPC-4101/26, (TYPE PC-GF)
  4. MANUFACTURE IN ACCORDANCE WITH IPC-6012A, TYPE 3, CLASS 2.
  5. INTERNAL LAYERS SHALL BE 1 OZ (.0014 IN [0.035mm]) COPPER MIN.
  6. EXTERNAL LAYERS SHALL BE 1 OZ (.0014 IN [0.035mm]) COPPER MIN.
  7. BOARD THICKNESS TOLERANCE SHALL BE .0625 IN [1.6mm] +/- .007 IN. [0.18mm].
  8. SEE STACK UP DETAIL FOR LAYER CONFIGURATION.
  9. ALL LAYERS VIEWED FROM THE PRIMARY (COMPONENT) SIDE
  10. ALL HOLE DIMENSIONS APPLY AFTER PLATING.
  11. ALL PLATED THRU HOLES SHALL BE IN ACCORDANCE WITH IPC-6012 AND HAVE A WALL THICKNESS OF .0008 IN  [0.020mm] TO .0012 IN [0.035mm]
  12. ALL HOLES SURROUNDED BY A LAND SHALL HAVE A MIN ANNULAR RING OF .001 IN [0.025 mm]
  13. LAYER TO LAYER REGISTRATION SHALL BE WITHIN .003 IN. [0.08mm].
  14. ALL HOLES SHALL BE LOCATED WITHIN A DIAMETER OF .006 IN [0.15mm] OF TRUE POSITION AS SUPPLIED IN CAD DRILL DATA
  15. FINISHED BOARD TO COMPLY WITH IPC-A-600E, CLASS II.
  16. FINISHED CONDUCTOR WIDTH AND SPACING SHALL BE WITHIN 10% OF SUPPLIED ORIGINAL CAD DATA.
  17. BOW AND TWIST SHALL NOT EXCEED 0.75% (.0075 IN PER IN) IN ACCORDANCE WITH IPC-A-600F FOR SURFACE MOUNTED BOARDS WHEN MEASURED USING IPC-TM-650, METHOD 2.4.22.
  18. 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 ON THE SECONDARY (SOLDER) SIDE OF THE BOARD.
  19. MAXIMUM RADIUS ON ALL INSIDE SHARP CORNERS TO BE .063 IN [1.6 MM]
  20. SOLDERMASK USING LPI OVER BARE COPPER PER IPC-SM-840, TYPE B, CLASS 2, COLOR: TRANSPARENT GREEN.
  21. ALL EXPOSED CONDUCTIVE SURFACES TO BE ENIG (ELECTROLESS NICKEL / IMMERSION GOLD) AFTER SOLDERMASK.
  22. ALL EXPOSED CONDUCTIVE SURFACES TO BE DIAGONAL HASL (HOT AIR SOLDER LEVELED) AFTER SOLDERMASK.
  23. APPLY COMPONENT LEGEND(S) USING WHITE NON-CONDUCTIVE EPOXY BASED INK AS REQUIRED BY CAD DATA. USE OF WHITE LPI MASK FOR LEGENDS IS ACCEPTABLE.
  24. ISOLATED OR UNUSED INTERNAL PADS MAY BE REMOVED AT MANUFACTURER'S DISCRETION.
  25. COPPER THIEVING ON EXTERNAL LAYERS IS ACCEPTABLE FOR UNIFORM PLATING OUTSIDE THE BOARD AREA. THIEVING MUST BE OUTSIDE THE BOARD AREA.
  26. PLUG ALL VIAS WITH SOLDERMASK TO CONFORM WITH CAD DATA.
  27. BARE BOARD ELECTRICAL TEST IS REQUIRED. VENDOR TO SUPPLY CERTIFICATION OF BOARD CONTINUITY BASED ON CAD DATA SUPPLIED.
  28. SEE SHT 2 FOR ASSEMBLY PANEL DETAIL.
 

 

 

Here are a list of check boxes you can go through to remind you of what to think about... If they do not apply, simply skip over them.

 

Mechanical Board Constraints

Board outline

Mounting holes

Connector locations

Hardware clearances and fasteners

Max height of components

Board Material  

 

Mounting Holes

Clearance for Hardware and components

Lock washers

Screws

Plastic Snap Fit hole sizes

Clearances for Standoffs

Global Fiducials for surface mount parts?

Sufficient Land area for Swage

Plated Non-Plated

Grounding

 

Material Requirements

 

Material appropriate to environment?

Tg of material appropriate for the maximum environmental temperature?

Thickness of material compatible with lead length?

Plating requirements for surface treatment?

Bow and Twist requirements?

Prepreg for multilayer construction?

Dielectric constant?

 

Connectors and Brackets

Clearance for components and hardware

Mating Dimensions and tolerances

Connector Orientation

Finger or tool clearance

Environmental sealing

EMI Shielding

Filtering

Holes sized properly for hand/machine installation

Strain relief for cables

Clearance for bend radius of cables

Can it be assembled? Tool Interference?

 

 

Components

Footprints match the manufacturers specifications?

Component to component clearance?

Fiducials for fine pitch parts?

Component to Mounting Hole or board edge?

Component height clearance?

Pin one or Polarity clearly marked?

Common orientation possible?

Common components or special order?

Ordered Long lead time items?

All parts on the BOM?

All Parts have company part numbers?

 

Tooling Clearances

Wave Solder

Pick and place

Screening

IR Reflow Machine

Test Fixtures

Registration pins

Holding Fixtures

Soldering Iron Clearances

Test Probe clearances

 

 

Trace Geometries

 

Trace Widths appropriate to current carrying?

Trace to Trace spacing less than 7 mils?

Trace to Pad less than 7 mils?

Trace sized for Impedance?

Acute Angles or etch traps that cause undercut?

Break out from pads sufficient? Fillets needed?

Matching Trace lengths?

Buses run together with terminations?

 

Inner Planes

Clearance to board edge and cutouts at least 25 mils?

Thermal pad design? clearances? connects or spokes?

Direct connections for vias to ground? Inner Pad removal?

Split planes? isolation, clearances and return path for signal traces? Mecca?

Thermal vias?

Capacitance Plane?

Symmetrical Stackup? (avoid warped boards)

Even Copper Distribution?

copper thickness?

 

Multilayer Board Stackup

 

Thermal Core?

Symmetrical Stackup? (avoid warped boards)

4 layer

6 layer

8 layer

10 layer

12 layer or greater

 

 

Board Outline

Can the board be trimmed with a standard .100  or .125 router bit?

Can the board be panelized?

Radius appropriate for routing tools?

Can the board be v-scored?

Are inner layers relieved of copper a minimum of 25 mils around the perimeter and any cutouts?

 

Board Information and Text

Board name and part number with revision in etch or silkscreen?

Company name, address, contact name, telephone and fax?

Title Block and Rev Block filled in.... page numbers, drawn by, dates, etc.?

Drill Table filled in with finished hole size, code, quantity and plated thru or non-plated indicated?

Make a 'read me' text file to be included in the Gerber package listing all the files it takes to make the board.

 

 

 

Testability

Test points located with sufficient clearance to allow the test probe to contact the board?

JTAG ports located near power supply connector and near the Chip under test?

Has a test plan been submitted and complied with?

 

 

 

 

 

 

 

 

 


 

 
 

 

 

 

Hit Counter

Copyright © 2004 PCB Wizards.COM
 Back Home Up