Requirements for Artwork, Solder Mask, Silk Screen
Thru-Hole Printed Circuit Board

This is a basic list of requirements for printed circuit board layout. This list should be considered a baseline or checklist that can be added to depending upon the specific needs of the current design. This list is tailored for thru-hole designs. Click here for the basic guidelines for SMT PCBs.

1. No sharp right angle bends or conductors when spacing is closer than 0.012 in.
2. Use circular pads for all pad/vias except pin one (1) on thru hole components, which should be square.
3. All signal traces must originate or end at a pad or via (no `T' connections permitted).
4. T's are permitted on power and ground wiring.
5. All power and ground traces must be a minimum of 0.050 in. wide except for tie ups and tie downs.
6. Maintain consistent orientation of similar components on the card.
7. The component silk screen must indicate the following on the component side:

(a)  Component outline.
(b)  Component identification code from schematics (i.e. U1, R1, ....)
(c)  Orientation of component (notch or pin 1).
(d)  Diodes must have anode/cathode marked.
(e)  "+" indicating polarity of polarized capacitors.
(f)  Card name, part number .
(g) Bright white indelible ink is to be used for the marking.

8. Refer to board outline drawing for required component placement.
9. Number components to read like book (upper left to lower right). Provide updated information in Protel format.
10. Decoupling capacitors have a .300 spacing. Place at roughly 1 capacitor for every   I.C. equivalent.
11. Provide 2 .040 holes .1" apart for ground at 1 place on the PCB.
12. Put PBC part number "100000 Rev. X" in copper.
13. PCB is to be XXX Layers SMOBC .062 thick.

Thru-Hole Spacing Requirements - Vias, Conductors, Foot Prints

1. 0.040 in. plated through hole (PTH) has a 0.060 in. pad.
2. 0.018 in. PTH has a 0.030 in. pad (for vias).
3. 0.040 in. PTH has a 0.070 in. diameter clearance on ground and voltage planes.
4. 0.018 in. PTH has a 0.050 in. diameter clearance on ground and voltage planes.
5. The power and ground connection pads are to use a three wheel spoke pattern for thermal relief to improve solderability.
6. Minimum conductor width for signal traces is 0.012 in.
7. Minimum distances:

(b) Line to line is 0.012 in.
(c) Line to pad is 0.012 in.
(d) Pad to pad is 0.030 in.

8. One line per channel allowed for pin-in-hole 0.100 in. grid.
9. Minimum conductor width for power traces is 0.030 in (highlighted in yellow).

Summary of Spacing Requirements

FROM	TO	MIN. SPACING (in.)
CONDUCTOR	CONDUCTOR	.012
CONDUCTOR	PLATED THROUGH HOLE PAD	.012
CONDUCTOR	BOARD EDGE	.020
PLATED THROUGH HOLE PAD	BOARD EDGE	.020
COMPONENT BODY	BOARD EDGE	.050
COMPONENT PAD	COMPONENT PAD	.040
(SIDE TO SIDE)
COMPONENT PAD	COMPONENT PAD	.140
(END TO END)
COMPONENT PAD	COMPONENT PAD	.040
(DISCRETE)	(DISCRETE)

Copyright (C) 2002 Electro Technical Products, Inc.