Avanthon Engineering, Inc.
HomeEmbedded SystemsProductsNetEDAProcessForumAbout Us
Process OverviewSchematic ChecklistLayout ChecklistDVT Checklist
Engineering Process

PCB Layout Check List

  1. The most common layout error is reversed diodes and polarized capacitors. Double and triple check the polarity of these parts. Check the pin numbers between the schematic symbol and the PCB decal
  2. Write up layout instructions before going to layout. Include board thickness, number of layers, layer stack up, power and ground instructions, a list of critical nets, trace thickness and spacing, instructions for autoroute or no autoroute, logos and part numbers, mechanical constraint drawings, bypass capacitor instructions, any special instructions and a hard copy of the schematic.
  3. Check the PCB decals very carefully. Use the NetEDA Decal Report Generator to speed up decal checking. Visually inspect the decals, place a part on a 1-to-1 plot if possible.
  4. Check all mechanical constraints. It is very expensive to rework an board to move a connector a few millimeters after it has been routed.
  5. Run the NetEDA Netlist Compare Utility between the PCB netlist and schematic netlist. Pay attention to the decal name and resolve all differences.
  6. Check all pin 1 orientation on all IC's and connectors. Try to have the CAD designer limit the orientation of IC's to two axis. This will speed up manufacturing and reduce the chance of errors. Verify proper silkscreen annotation.
  7. Check all bypass capacitor placement and power/ground connections.
  8. Check for mechanical conflicts with components, especially connectors. Verify that the mating half of the connector will clear surrounding components.
  9. Check for any component height limitations, especially heat sinks.
  10. Check the power layers and power distribution
  11. Check all polarized capacitors, Verify proper silkscreen annotation.
  12. Check all transistors, capacitors, diode routing. Often the PCB designer has to interpret netlist as to gate source, drain, emitter, cathode and anode.
  13. Check all key signal routing. Verify high speed signals are short. Verify signal pairs and busses have matched lengths.
  14. Check for sloppy routing, excessive vias, etc.
  15. Check for proper via selection. You don't want a microvia connecting two large power traces.
  16. Check hole drawing. Verify all connector holes are proper size. Remember a 0.025 square pin requires a 1.414 x 0.025 or 0.035 hole (0.040 when tolerances are considered).
  17. Check silkscreen. Verify all reference designators are visible and not under components.
  18. Check part numbers, logos, etc.
  19. Check for clearance problems with screws and mounting hardware.
  20. Check for nets routed too close to mounting holes. These may become shorted when the mounting hardware is installed.
  21. Hold placement reviews and routing reviews.
  22. Run the NetEDA Netlist Compare Utility against the new and old PCB netlist when making changes to the layout. Turn on the Check Component Placement and verify that only the changes you want were made.
  23. Complete all of the items above. Be VERY careful, skipping these double checks is often incredibly expensive. Always try to get an independent party to triple check your design. Use all tools available.
Copyright Avanthon Engineering, Inc, 1999-2002
Home Embedded Systems Design Products NetEDA Process Forum About Us

Avanthon Engineering, Inc.
Lake Oswego, Oregon 97034
Tel: +1 (503) 313-2738 E-mail: sales@avanthon.com