|
1. File format
The documentation required for producing a printed circuit board setup and the boards themselves can be provided on disk or CD, or sent via e-mail to the addresses indicated on our Website. Our standard format for the realisation of the systems is the extended GERBER format (i.e. RS-274-X, absolute, in inches, with coordinates expressed in 2 whole numbers and 3 decimal numbers).
We will be also glad to accept the ODB++ format (all modern CAD systems have this format available among the output options). Also permitted are HPGL-1 and Gerber RS-274-D formats. In the latter case, remember to send the aperture list as well and avoid the use of customised apertures, using only D-codes in square, rectangular, circular, oval, octagonal or thermal form.
2. Files required
The files required to realise the PCB are those for the printing faces (component side and solder side plus any inner layers for the multilayer circuit boards), the solder resist mask, the simbology layer, the peelable mask when required. In the case of a circuit board with SMD components, it would be appropriate to send the solder paste layer as well.
The various layers must have all the squares to indicate the board edge, they must all be overlayable and visible from the same side, i.e. they must all be on the component side or all on the soldering side (it must however be clear which side the view is).
We also require the drilling data which generally consists of a drilling drawing and the actual drill file.
2.1 Drill files.
The positions and diameters of all the holes must be indicated in the drilling drawing (generally a Gerber file), also specifying what type of hole it is (plated or not). If possible, also summarise the number of holes for each diameter.
The drawing can also act as a mechanical drawing. In this case, it must contain the profile of the board with relevant dimensions, any breaks, slots or bevels, cracking holes, internal milling lines, scoring lines, etc. If the dimensions requested in the order or indicated on the mechanical drawing disagree with those we find by measuring the squares in the Gerber file, we will always consider valid the measurements taken from the Gerber file.
In addition to the Gerber files for the realisation of the systems, we require the drill file which will be the direct input for the NC drilling machines. The preferable format for the drill file is SIEB & MEYER 3000 (with absolute coordinates – incremental coordinates are not acceptable – expressed in mm with 3 whole numbers and 2 decimal numbers without omitting the insignificant zeros before and after the point), but also other formats such as EXCELLON (again with absolute coordinates without omitting the insignificant zeros) can be used. The diameter of each bit used and the number of holes drilled with each bit must be indicated, possibly in a separate text file. If it is not possible to provide a drill file in Sieb & Meyer or Excellon format, it can be provided as a Gerber file with the pads in exactly the same dimension as the corresponding hole.
The minimum workable diameter for the metallized holes is 0.25 mm. Bear in mind that small-diameter holes affect the price of the board. The smallest diameter that does not require special working (and hence does not affect the price) is 0.50 mm. Our standard drilling diameter tolerance is +/- 0.06 mm.
2.2 Component side and soldering side.
There must not be any pads near non-plated holes. The pads of the plated holes should preferably have a diameter 0.60 mm (0.45 mm accepted) larger than the relevant hole (unless for specific requirements where a hole without annular ring but plated is required: we consider unplated a hole with a pad of the same diameter without specific requirements).
The minimum spacing values required between tracks and pads, pads and pads, tracks and tracks are the following: 0.008 inches preferable, 0.005 inches accepted (spacing under 0.008 inches may affect the price).
The minimum pattern distance (tracks, pads, ground plane) from the board edge must be 0.008 inches in the case of routing and 0.019 inches in the case of scoring. It must be clearly indicated which side is the component side and which the soldering side, also indicating the right side for each of them. In particular, the text must always be legible on the printing side.
2.3 Inner layers.
In the ground layers, the clearance pads must have a diameter 0.80 mm larger than the diameter of the relevant holes. In the signal inner layers, however, a diameter which is 0.50 mm larger than the hole diameter is sufficient. In the ground layers, it is preferable that the pattern (in this case the ground planes) is 0.020 inches from the board edge: this is to prevent the copper from reaching the board edge and hence creating short-circuits between the inner layers in the milling phase. It is important to always indicate the build-up of the various layers of a multilayer board (for example, if you send the TOP, BOT, PWR, GND layers, specify that the stacking order is TOP ? PWR ? GND ? BOT).
2.4 Solder mask
The pads for the solder resist must be provided by the customer in the same dimensions as those of the top and bottom layer pads (unless there are special requirements): we will enlarge the solder pads according to our standards (the solder pads are enlarged up to a maximum of 0.010 inches in diameter, however, maintaining a clearance of 0.007 inches between the solder pads and between solder pads and tracks or adjacent copper area).
If these solder modifications are not desired, the solder must be provided by the customer as desired and will not be modified by us (clearly specify this in the documentation provided). Near the non-plated holes, the solder pads must be at least 0.016 inches larger than the hole. This is important, since if the solder pads are smaller they serve no purpose and the solder paste adheres to the inside of the unplated hole reducing the diameter. To prevent the solder on the board edge from cracking during board routing, the outrmost face of the circuit board must not be covered with solder for a distance of 0.016 inches.
2.5 Simbology
The simbology layer tracks must have a minimum thickness of 0.008 inches and a maximum of 0.013 inches. We advise using characters at least 0.060 inches tall so that they are legible. It is essential that the text (and the lines) do not overlap onto the holes, otherwise they will not be legible and the ink will drop into the hole and may cause problems in the soldering phase because of bad of the soldering alloy.
In the case of boards with SMD components and with electrical test, it is important that the simbology does not go over the pads (both SMD and not) in order not to hamper conducting the electrical test and the subsequent mounting of the SMD components. If the data provided does not respect this condition, we will automatically correct this error.
3. Other information required for the realisation of a printed circuit board.
The minimum data required in order to proceed with execution of the order are the thickness of the base laminate, the type of material (FR4, Cuclad, ...), the base copper, the final copper (i.e. the electrolytically applied copper plus the base copper), the number of pieces and the finishes required (solder masks, simbology, hot air levelling or chemical silver-plating, electrical test, gold-plating, etc.).
It is very important to provide at the outset any specifications for circuit multiplexing on a panel. This involves establishing the number of circuits on a panel (i.e. indicate the maximum dimensions of this panel), the presence and characteristics of the fiducial marks, and the feed holes.
It would also be useful to have additional technical data, such as: any tolerance limits in the hole diameters, the hole positions, the cutout dimensions (our standard tolerance is +/- 0.02 mm); minimum spacing between track and track, minimum size of the tracks and any other special requirement or technical data considered useful. When documentation is provided for a new version of a circuit board that we manufacture, the order must indicate whether the new version cancels and replaces the previous version, in which case we will return the old version (or destroy it if you prefer) in order to prevent misunderstandings in the event of subsequent reorders. Should you wish to keep the old version as well, it must be clearly indicated in all subsequent orders which version you desire, referring to our DNC alphanumerical code which is different for each version of the circuit board. In the event of substantial modifications to a circuit board (e.g. elimination of a track), in accordance with UNI EN ISO 9001 standards, a new code will be assigned to the circuit board, while the customer must provide a new serial number.
|