Ronja Twibright Labs

Ronja Guidelines

Creating a SMD PCB footprint for construction class 4

Construction class 4 is 0.3mm copper, 0.35mm gap, 0.2mm silkscreen.

  1. Set grid to unit according to source drawing
  2. Draw the pads on the solder layer using the line tool and pins using the via tool. Use CTRL-m to measure and precisely position.
  3. For pins, set annulus inner size by ("changedrillsize(...)") and annulus outer size by ("changesize(...)")
  4. Draw the silkscreen with 0.2mm line thickness on silk layer. The centerline of the silkscreen to be the outermost possible edge of the component. The silkscreen thickness is an allowance for positioning error.
  5. Draw an alignment cross in the component reference point (usually the centroid). Use two rectangles placed on "unused" or "unused1" layer
  6. Check all dimensions according to drawing using CTRL-m
  7. Go over each pad or pin, press 'n' and enter the pin/pad number.
  8. ALT-a, go at the alignment cross, CTRL-x
  9. Buffer -> Convert buffer to element
  10. Screen -> Grid setting -> 100mil or 2mm
  11. Place the element somewhere apart from the original drawing
  12. Press 'q' on all pins/pads which should be square, or over the symbol if all pads should be square.
  13. Go over every pin/pad, press 'n' and reenter the presented number
  14. Turn on soldermask by Screen -> Enable view soldermask
  15. Now you need to change soldermask for all pads. Always select all pads with the same thickness (measure in muls using CTRL-r). Execute "changeclearsize(selectedobjects, thickness/2+4,mil)".
  16. ALT-SHIFT-a
  17. Turn off soldermask by Screen -> Enable view soldermask
  18. Turn off silk
  19. Select solder layer
  20. Draw a big rectangle over the footprint
  21. ALT-a
  22. Press ':', enter "changeclearsize(selectedobjects, 0.35, mm)"
  23. Remove the big rectangle
  24. Turn on silk
  25. Press 'n' over the silk and for a resistor enter R000, capacitor C000, coil L000, transistor Q000, soldering point T000, diode D000 etc.
  26. Place the label suitably near the footprint
  27. Press 'd' over the footprint, check the numbers, press 'd' again
  28. Select the whole footprint
  29. Go at the middle of the diamond, CTRL-x
  30. Save buffer elements to file, enter desired filename
  31. File, Quit Program, OK to lose data? OK.
  32. Add your created file into your revision control system and start pcb again.
  33. Load element data to buffer, enter the name of the file
  34. Click somewhere and check the footprint looks as expected
An expected information missing here?