The following information may have errors; It is not permissible to be read by anyone who has ever met a lawyer. Use is confined to Engineers with more than 370 course hours of electronic engineering for theoretical studies.
ph +1(785) 841 3089 Email email@example.com
Loading in finished Gerbers for checking is a last step in designing a PCB.
 Related kicad pages
- EE CAD Terminology
- kicad Navigator - the kicad project Manager
- eeschema - the schematic editor
- cvpcb - the component to module (AKA foot-print) editor
- pcbnew - the PCB layout program
- Gerbview - the Gerber file viewer and production notes
- Bitmap2Component Converts bitmap images to filled polygons
- wings3d - 3d view - good way to waste a lot of time..
- Super Money saving tip: print out the artwork on card-stock 1:1 and poke holes and stuff it like a real PCB - find errors - fix them and rework for pennies all the same day..
 Part Placement
- SMD component orientation consistent
- Clearance for IC extraction tools, heatsinks etc.
- Polarization of components checked
- Are components on grid ?
- Check the orientation of all connectors - is Pin #1 where you expect it?
- minimum component body spacing
- Bypass capacitors located close to IC power pins
- Series terminators are located near the source
- I/O drivers near where their signals leave the board
- PCB has ground turrets, power rail test points, and test points for important signals, all labeled
- EMI and RFI filtering as close as possible to exit and entry points in shielded areas
- Potentiometers should increase controlled quantity clockwise
- Mounting holes electrically isolated or not?
- Mounting hole clearance for hardware
- SMD pad shapes checked
- Tooling holes for automated assembly
- Extra clearance for socketed ICs
- Pin one pad indicators
- Digital and analog signal commons joined at only one point - net tie - ground Pavilion
- Check for traces running under noisy or sensitive components
- No vias under metal-film resistors and similar poorly insulated parts
- Traces spaced to max where possible
- Check for dead-end traces, unless used on purpose
- Ensure schematic software did / did not separate Vcc from Vdd, Vss from GND as needed (Not a problem if you don't use invisible connections - it really doesn't save time in the long run )
- Multiple vias for high current and/or low impedance traces - check the current ratings of your via size
 Current rating of Traces, viass
- Component and trace keepout areas observed
- Ground planes where possible
- Hole diameter on drawing are finished sizes, after plating.
- Finished hole sizes are >= 0.25mm larger than lead
- Silkscreen legend text weight, spacing
- Pads >=0.37mm larger than finished hole sizes
- Components spacing from edge of PCB
- Traces to board edge spacing
- Consider Drill size tolerance
- Soldermask clearance and tolerance - often board houses want zero clearance.
- High voltage traces need extra spacing
 Text on Silk Screen and other Layers
- Allign legend text tp read from one or two orientations
- Logo in silkscreen legend
- Copyright notice
- PCB part number and version
- Do parts cover Legend
- Label all layers - Mirror text on back
- Pin one indicators
- High pin count parts can have corner pins numbered for ease of location
- Silk screen tick marks for every 5th or 10th pin on high pin count Parts
- CAD design rule checking must be turned on
- High frequency circuitry precautions observed
- ReadMe for PCB house see Gerbview#What_to_send_the_PCB_house checklist
- Thermal reliefs for internal power layers
- Solder paste mask spacing
- Blind and buried vias on multilayer PCB
- PCB layout panelization
 Standard Sizes
- Drill sizes: Drill_Bit_Conversion_Table
 What to send the PCB house
All the gerbers and a README.txt are packed up into a tar. ark is a great tool for this.
The README.txt should look something like this:
Contact name phone email address >>>- hole dimensions are finished size- <<<<< -PCB Name and revision number: DC_UPS3.1 Use this name on invoices -We provide Gerber files including drill layer Pads 23 Through vias 16 Smallest hole .025" (0.64mm) Specified finished size. 39 holes -FR406 or 370HR 1.57mm[.062"] IPC-4101C Sheet 24 -1 oz copper -Quantity 4 -Sides 2 -HASL -Silk Screen 2 sides (white or yellow) -Solder Mask 2 sides green/matte finish SR1000 over bare copper (same art work) to IPC-7351 -Size 50 x 65mm -To IPC specifications - For productions quantities please Quote - Solder resist (solder mask) is required on both external faces of the printed board, it shall meet the qualification/conformance IPC-SM-840. Coverage, cure and adhesion shall be as defined in paragraphs 3.8.1 to 3.8.3 of IPC-6012, except that no encroachment of solder resist is allowed on any surface mount or ball grid lands, and that ALL pad patterns have solder resist slivers between individual pads. The height of the solder resist should not cause any mounting problems for surface-mount components. Solder resist data is provided as per IPC-7351 standard, 1:1 with the land size, the manufacturer is to oversize these solder resist openings commensurate with their manufacturing procedures ensuring that ALL the above requirements are met, the amount of oversize to take into account the minimum track and gap dimensions as shown on the Printed Boards Master Drawing. Solder resist not related to a component pad is not to be enlarged.
Things to have in the readme :
- Name with version of the board: widget2.3
- Size - outer rectangle dimensions
- Sides 1,2,4 or more..
- plate finish : HASL works for leaded solder - fancy expensive stuff for the insane RoHS
- LPI Silk Screen 2 sides (white or yellow) 1mm tall 0.1mm wide
- LPI Solder Mask 2 sides green/matte finish SR1000 over bare copper (same art work) to IPC-7351 - we provide it with .05mm clearance [0.002"]
- IPC-4101C Sheet 24 - This is a common way to try to get good material
- 1.57mm,[.062"] You need to specify how thick the board is.
- FR4 is the common epoxy fiberglass material, FR406 has replaced it and 370HR is often used for no lead
- Copper thickness 0.0347mm [1oz]
- Quality specifications.
 Notes about Minimum feature sizes
- The days of .25mm[10mil] traces with 250mil spacing are long over. Today (2011 ) Trace minimum of 0.100mm is standard and 0.075 -0.080mm can be had without a premium. Premium minimum air spacings are about 0.050mm. The minimum depends on copper weight - below are approximate limits if you want to pay extra.
- 0.100mm at 17.35um[1/2oz]
- 0.125mm at 34.7um[1oz]
- 0.150mm at 69.4um[2oz]
- Eeschema now has a built-in calculator for trace width and other features. The following link is for an older tool. Also, SaturnPCB has a free calculator that includes differential traces, but runs only on Windows.
- Trace width / current calculator
- Annular ring of 0.5mm[20mil]minimum is a good idea for through hole, but many board houses can go as low as 0.075mm[3mills] Best not to go under 0.25mm without good reason. A 0.457mm pad x 0.200mmhole is usually without extra charge. Be sure to calculate Current ratings of your Vias. via-calculator
- Why not use the smallest size the shop offers at your price point? Because especially at discount houses there are tolerance issues in aligning layers and in drilling. You may find traces disconnected from their vias if the drill was a little off center, or if the etch was a little uncontrolled. Doubly important if you are not paying for full electrical testing.
- Don't use minimum Vias without good reason
- start with Vias 0.75mm[30mil] with a 0.457mm[18mil] drill for simple signal traces.
- Minimum micro via 0.46mmpad x 0.200mmhole
- Minimum coper to board edge - normally .25mm
- Hole size tolerances are usually +/-0.075mm to +/-0.125mm specified finished size.
- Minimum hole size 0.200mm - smaller can be LASER drilled for a price if you really need it.
- Minimum slot width 0.80mm
- Minimum Solder mask Clearance 0.05mm  - special deals can do 0.025mm
- Minimum Silk screen
- This is a bit complicated - the size is three numbers H x W x T (where T is line thickness). It is common to see the limit on line thickness 0.100 - 0.125mm[4-5] but the real limit seems to be 0.075mm. What I recommend is not to IPC specification, but if the idea is to have useful information available for trouble shooting and debugging modern SM, then we need to find the limit and the IPC might catch up with us someday. When going smaller One does need a magnifier to read, but one needs a magnifier to see the components as well! (I'm looking through a 7 or 10 power Optivisor or a Stero-zoom anyway! )
- Some places will say their LPI is limited to a line width of 0.100mm and with that you can get down to a letter size of about 0.9 x 0.7 x 0.1mm
- You can push it by going to 0.075mm line width - and ending up with a 0.8 x 0.9 x 0.075mm
- Anything smaller and you might as well leave it off the board and look at an assembly drawing show the detail. That's just the practical side of it. I will use the above with my 1005M's, but that seems to be todays limit. I don't care if a few end up unreadable, at least there is a clue with the small ones.
- So here is what I suggest - make your library foot-prints with 1.0 x 0.9 x 0.1 mm reference designators and if you have a place where you need something smaller use 0.8 x 0.9 x 0.075mm
If you are using a supper cheap shop that is using obsolete silk screen - you will want to double the size 2.0 x 1.8 x 0.125 mm
 Send Off Check List
 Pre Gerber
- Version strings on the PCB
- Readme.txt quantity and specifications
- Schematic Electrical Rules Check
- PcbNew Design Rules Check
- A tour of a PCB house
 PCB Board houses
Picking a board house depends on what is needed. Cheap boards that have the copper glued on instead of laminated at the same time that they heat cure the epoxy - cheap board traces will come off with just the slightest amount of rework. If they don't spec the Tg of the material, you are getting really cheap junk. Put your favorite place here and add comments - don't delete or reorder other PCB houses with out leaving a good reason on the discussion page or your edit will just get reverted.
The cheapest laminate disappointed me (traces lift if they even see a soldering iron.) - go with the FR406 and 1oz copper. The cheapest laminate could be used for very low cost for things that will never be reworked.
They now offer several laminates and copper thicknesses.
They can do very good work - a bit pricey, but they offer good laminate.
 SINOMICRO PCB
- Sinomicro PCB
Low Cost PCB Prototype,PCB manufacture,PCB Assembly and PCB Design
http://dorkbotpdx.org/wiki/pcb_order Shared PCB orders for hobbyists.
Haven't used - probably too cheap to be high quality. Taiwan laminate - fails to specify Tg - or IPC-4101C
 Multilayer Technology
 Seeed Studio
Located in Hong Kong. Offers single and double sided PCBs with solder mask and silkscreen, a variety of thicknesses and finish colors on quality FR4 material. The quality of the PCBs I've ordered has been as good as anything I've worked with and the price was extremely competitive for small batches of boards. Not particularly fast, takes about a month from submission to receive finished PCBs. Max size offered is 20cm x 20cm.
Taiwan laminate - fails to specify Tg - or IPC-4101C
Provides good quality in affordable cost. Uses FR4 Tg170(S1000-2) and FR4(S1141). Complies with IPC600F standard.
 San Francisco Circuits
 PCB Fab Express
 Advanced Circuit
 Speedy PCB Prototype
 AP Circuits
 Bare Bones PCB
 PCB Express AKA Sunstone
 Sierra Proto Express
 SMTH Circuits
 Quick-teck PCBs
- UK based PCB manufacturer,guaranteed delivery date. Online instant quote, reasonable prices.
 Custom Circuit Boards
Good USA PCB manufacturer. Fast quick turn prototypes, but you need to have a min lot of a panel. Good selection of board materials with extensive capabilities.