Cost Reduction Ideas

Pad Sizes:

• External Pads = Finished Hole +0 .019”(min)
• Internal Pads = Finished Hole + 0.021”(min)
• Internal Ground Clearance = Finished Hole +0 .030”(min)
• Solder-mask Pads = Solder Pad + 0.006”(min)

Draws vs. Flashes:

When possible, use a flash for pads and features instead of draws. Draws require a lot of memory and slow programming time considerably. If we must adjust a pad size for manufacturing, a flashed pad is easily changed by changing the D-code whereas a drawn pad requires extensive manipulation.

Silk-screen:

Never program silk-screen over a soldered pad. This may effect the soldering process and the quality of the solder joint. Leave silk-screen nomenclature at least .006” from any pads. Nomenclature line width should be no less than .006” lines and character height at least .060” high.

Print quality is adversely affected by high copper features and may be partial or illegible. When using heavy copper designs (i.e.. >2 oz), consider using no silk-screen or place component designators in areas of ground plane or bare laminate, avoid printing over traces.

As standard procedure, we clip silk-screen from soldered pads. Please Contact Us if for some reason you require silk-screen on your pads.


Routing:

To aid in programming, add a borderline to one of your files. This gives us a quick reference for the rout program.

If your design requires stitch routing, please allow for the use of 0.093" or 0.125" cutters.
This will increase stack height and speed up routing time.

Standard cutter diameters are:  0.032", 0.040", 0.050", 0.062', 0.093", 0.125".

Ditto for internal radii, please allow for the use of a standard cutter diameter.

These guidelines are intended to help assist you in your design and are not meant to be the only workable solution.

1. The distance between tabs along the periphery of the board will vary depending to board thickness. Typical spacing: for an 0.062" board, one tab every 2.5" to 3.0", for 0.031" thick, one tab every 2.0" to 2.5". Remember, the tabs are designed to support the weight of the board and components through the reflow or wave soldering while still being relatively easy to break.
   
   
2. Usually, the "mouse-bite" tab consists of a series of holes(3-5) drilled side by side along a flat section of the board outline in an un-routed area of the base material. Rule of thumb: Pitch of the holes should be 2x the hole diameter (i.e. for .020" holes, center-to-center spacing should be .040"). The idea of the tab is that it may be snapped off manually, either by hand or by flexing the tab with a pair of needle nose pliers. The weakest part of the tab is along the diameter of the row of holes. To help minimize the cost in drilling you might use the smallest via hole size already used on the board so the fabricator will not have to add additional drill sizes. Typical : 0.030" holes on 0.050"-0.060" centers.
   
   
3. To minimize tab residue, drill the breakaway holes with their diameter or hole center along the board outline. When the tab is broken off, part of the drilled hole will be on the inside of the board outline, and the tab residue outside the outline will be negligible.
   
   
4. Tab location: tabs should be as far as possible from small SMD components as practical because the flexing of the board during remove the board out of the array could fracture adjacent solder joints or the component body itself. No component within .300" radius of the tab should be mounted perpendicular to the edge of the board.