Some tips to avoid a few of the more common problems that occur with PCB designs.
If board outline is provided on the silkscreen layer, please isolate its aperture size from other elements on the layer - a one mil outline is a good choice.
Remember that for standard 0.062" material the standard via hole size is 20 mil. If you put 18 mil holes on that board, there will be an added cost.
Keep to just one size via hole unless the design requires more.
Generate gerber data with enough precision - if the precision is too low, round-off errors will occur and object placement can be off by a few mils.
Try to keep to regular pads like round and square - oblongs and teardrops are possible, but introduce more potential errors. Only use irregular pads when necessary for design reasons. Doughnuts - round pads with a clearance in the middle for the drill hole - are never helpful.
Also, only one flash is needed. There is no advantage to building a square pad out of 4 smaller squares, or making a 100 mil round pad by superimposing a couple of hundred 40 mil pads.
Cross-hatching planes with an open grid is strongly discouraged, as it can potentially cause all kinds of problems, including the connected gap problem. Use a solid ground plane fill unless the design specifically requires otherwise.
Tooling Holes: 2 x 0.062" holes on opposite corners of the board for routing. If we cannot add any holes to the board for design reasons, we need to be told.
Logo and Date Code: Due to ISO requirements, we need a 0.6" x 0.2" space to put our logo and date code. This is usually in the copper on the solder side. If any extra copper might cause a problem with the design, we need to be told - we can put our logo and date code in the silkscreen.
UL Markings: If UL markings are required, we need a 0.5" x 0.3" space.
We can leave all mfg markings off the boards, but this must be explicitly requested. Also, remember that if we omit our markings, it cannot be proven we manufactured the boards.
Too much text on a copper layer causes excessive interference with design rule checking (eg unterminated traces, tight gaps, etc...).
Incomplete Fab Information
Including a readme.txt file is highly recommended, a sample is available here. A fab drawing is also useful if it can be generated from software.Copper to the edge of the Board
There should be at least 0.010" between copper and the edge of the board. If copper runs to the edge of the board, the soldermask will begin to flake off the edges during the routing stage. Exposed copper on the board edge will oxidize, and can lead to shorts.No Board Outline
We need either a board outline or a (0,0) reference with measurements. Otherwise we will have to contact you to get it.If board outline is provided on the silkscreen layer, please isolate its aperture size from other elements on the layer - a one mil outline is a good choice.
Mask Expansion
We recommend you do not expand your pads for the solder mask file (ie 0 mil expansion). Our CAM department would prefer to deal with the expansion themselves. You can spec a maximum expansion.Use a Gerber Viewer
Every now and then we get a board with layers that do not seem to go together, or some other feature that doesn't look right. If you have any doubts about what your layout package is going to put out, we recommend you use a third party gerber viewer. A very good one can be found here.Inner Layer Clearance
Plated through-holes on multilayer boards need to be cleared from internal planes by at least 15 mil, 20 mil is better. There are several reasons for this, all to do with inner layer heat expansion and layer to layer misregistration.Unneeded Tool Sizes
The tolerance on hole size is generally +/-2 mil, so there is no point is putting 37 mil and 38 mil holes on the same board - might as well make them the same size.Remember that for standard 0.062" material the standard via hole size is 20 mil. If you put 18 mil holes on that board, there will be an added cost.
Keep to just one size via hole unless the design requires more.
Gerber Format
The preferred data format is GBX, or RS274X - most recent layout packages support it. Also, using the same data precision for both gerber and drill data is recommended.Generate gerber data with enough precision - if the precision is too low, round-off errors will occur and object placement can be off by a few mils.
Drawn SMT Pads
Flashing, as opposed to drawing all SMT pads is highly recommended. Drawn pads usually have to be converted to flash in CAM, which takes extra time and introduces the possibility of operator error.Try to keep to regular pads like round and square - oblongs and teardrops are possible, but introduce more potential errors. Only use irregular pads when necessary for design reasons. Doughnuts - round pads with a clearance in the middle for the drill hole - are never helpful.
Also, only one flash is needed. There is no advantage to building a square pad out of 4 smaller squares, or making a 100 mil round pad by superimposing a couple of hundred 40 mil pads.
Silkscreen on Pads
Generally silkscreen on pads is not needed. We only clip silkscreen off the pads when bare board testing has been ordered. Also, silkscreen on SMT pads will make soldering more difficult. Also remember the silkscreen placement tolerance is +/- 5 mil, so a pad outline can intrude on the pad itself. Some parts libraries are not well designed; check your design carefully.Technical Contact
Often all our information comes from the purchasing dept, not engineering. Putting the engineering contact in with the data is a good idea, as it can speed up the resolution of technical problems. In the case of rush work, giving us off-hours engineering contact information has saved jobs from delay.Inefficient Ground & Power Planes
When generating a ground plane, using inefficient parameters like 0.5 mil steps will create large gerber files, which increase DRC times, etc... without any advantage to the design. Use a reasonable line width and step size, comparable to your chosen design rules.Cross-hatching planes with an open grid is strongly discouraged, as it can potentially cause all kinds of problems, including the connected gap problem. Use a solid ground plane fill unless the design specifically requires otherwise.
Connected Gap
Keep to the minimum trace/space parameters, even if two close elements are electrically connected elsewhere. A 1 or 2 mil airgap can result in a piece of photoresist film tearing off, and falling across the design, possibly creating opens or shorts.Thermals in Vias
Thermal reliefs on inner layers are needed only for soldering purposes, so they serve no purpose on a via. A solid connection makes CAD work easier.Manufacturing Features
We need some board space for manufacturing features.Tooling Holes: 2 x 0.062" holes on opposite corners of the board for routing. If we cannot add any holes to the board for design reasons, we need to be told.
Logo and Date Code: Due to ISO requirements, we need a 0.6" x 0.2" space to put our logo and date code. This is usually in the copper on the solder side. If any extra copper might cause a problem with the design, we need to be told - we can put our logo and date code in the silkscreen.
UL Markings: If UL markings are required, we need a 0.5" x 0.3" space.
We can leave all mfg markings off the boards, but this must be explicitly requested. Also, remember that if we omit our markings, it cannot be proven we manufactured the boards.
Labels on Gerber Layers
It is a good idea to put some text on each gerber layer. This will make it obvious which way is right reading. The text can even be placed off the edge of the board if no text is wanted on the board itself.Too much text on a copper layer causes excessive interference with design rule checking (eg unterminated traces, tight gaps, etc...).