This section will describe the data needed to manufacture a circuit board; data that YOU will be providing to your customers.

Let's hope that by the time you are reading this, the industry will have adopted universal data formats for board manufacturing, all CAD software packages will be able to output these formats into a single file that any manufacturing partner can use, and you won't have to know too much about this subject. Some people are diligently working towards this goal, but at the time of this writing there are still many considerations that need to be resolved.

In the meantime,
you need a basic overview of what is required.

What you will be supplying for manufacturing is DATA, which can be divided into two major categories; data used to manufacture the bare-board, and data used for the board assembly and test

In addition to the data needed to manufacture the final product (which you will be generating at the end of the design cycle), you may be asked for various types of data along the way. Let's take a brief look at some of these first:

BILL-OF-MATERIAL (BOM)

When packaging a design, your software will evaluate the schematic diagram and map the symbols into actual components. After the packaging is complete, each component is given a unique identifier called a reference designator. Since the system now knows how many of each type of component is required to build the product, a part list or Bill Of Material (BOM) can be generated. Even before you start the design, several people may need this information, so you may want to send it out as soon as you have it.

The BOM will have different fields of information either in spreadsheet form, or seperated by commas or tabs in ASCII files. Each entry will contain at least a part number and a reference designator, but may have additional fields of information that may be of interest to different people, like company part number or manufacturer numbers. Here's an example:

# These comment lines should contain design number 
# and revision level (and date)
#
ITEM QTY P/N  LIB     DESCRIPTION     REFDES
  1   3  235  c0805   cap,0.01uF,25V  C1 C2 C3 
  2   1  674  tsop65  ram,custom3708  U1
  3   1  519  db25ra  connector,db25  J1  

If there is no formal Design For Manufacturability (DFM) review, you may be able to help by scanning the result before forwarding it to other departments. One improvement you should look for is similar parts that could be combined into a single part number. For example, say you noticed that two different part numbers were calling for .1uf capacitors, and they are similar enough that they can use the same part number. This saves money by being able to buy common part numbers in higher quantities, and improves efficiency by making one less reel of components to stock, transport, and load onto the assembly machine. Look for inconsistencies. For example, if the design is primarily surface mount technology, but you see a through-hole resistor in the BOM (or on your layout screen), it might be worth asking if it is correct.

Others may want this information to begin looking at components that have long buying lead-times, for cost analyisis, for inventory control, or for an obsolescence study. Once you are confident that your BOM matches the design intent, Get the BOM to the people who can use it as soon as possible.

MECHANICAL

If the CAD system you are using can import and export a file format compatible with the CAD system used for mechanical design work, your job may get a lot easier. Using the power of your tools to collaborate throughout the design process can save time and effort, and reduce the chance of introducing errors into the final product.

For example, many companies that I have worked for have CAD systems that support data sharing using the Intermediate Data Format (IDF). This format uses two files, an Electro-Mechanical Part file (file extension .EMP), and an Electro-Mechanical Neutral file (file extension .EMN).

The .EMP file contains a primitive description for each type of part in the design, consisting of a polygon shape of the maximum size of each part and its maximum height. Here is an example of a simple .EMP file containing only two types of components, an integrated circuit P/N1001 using a TSOP65 land pattern, and a capacitor P/N1002 using a C0805 land pattern:

.HEADER
LIBRARY_FILE 2.0 JAXCAD 2010/05/31.12:00:00 1
.END_HEADER
.ELECTRICAL
P/N1001 TSOP65 MM 1.100
0 -3.100 -1.550 0.000
0  3.100 -1.550 0.000
0  3.100  1.550 0.000
0 -3.100  1.550 0.000
0 -3.100 -1.550 0.000
.END_ELECTRICAL
.ELECTRICAL
P/N1002 C0805 MM 0.900
0  1.970 -0.127 0.000
0  1.970  1.143 0.000
0 -1.970  1.143 0.000
0 -1.970 -1.143 0.000
0  1.970 -1.143 0.000
0  1.970 -0.127 0.000
.END_ELECTRICAL

The .EMN (Electro-Mechanical neutral file) contains X-Y coordinates for the board outline, X-Y coordinates for Drilled Holes, and the X-Y coordinate for each component (including rotation and which side of the board it is mounted on). Here is an example of a simple .EMN file:

.HEADER
BOARD_FILE 2.0 JAXCAD 2010/05/31.12:00:00 1
pcb MM
.END_HEADER
.BOARD_OUTLINE
1.600
0 -5.000 -5.000 0.000
0 30.000 -5.000 0.000
0 30.000 40.000 0.000
0 -5.000 40.000 0.000
0 -5.000 -5.000 0.000
.END_BOARD_OUTLINE
.DRILLED_HOLES
4.000  0.000 35.000 NPTH BOARD
4.000 25.000 35.000 NPTH BOARD
4.000 25.000  0.000 NPTH BOARD
4.000  0.000  0.000 NPTH BOARD
.END_DRILLED_HOLES
.PLACEMENT
P/N1001 TSOP65 U1
3.800 5.200  90.000 TOP PLACED
P/N1002 c0805 C1
3.800 5.000   0.000 BOT PLACED
P/N1002 c0805 C2
3.800 5.200 180.000 BOT PLACED
P/N1002 c0805 C3
3.800 5.400   0.000 BOT PLACED
.END_PLACEMENT

Notice that although the P/N1002 was only defined once in the library file (.EMP), it was used repeatedly in the design shown in the example above for C1, C2 and C3.

In a typical design development process, the ME may define the board outline and send it to you with mounting hole locations, you import this information into the design database and add components referenced in the schematic, you send back new data files containing your component placement, the ME uses your new files to create a 3D model to incorporate into the enclosure, he may refine the placement of critical components (like connectors, for example) and send it back with additional data such as height restrictions and keepout areas, you complete the final placement and send it back to him for use in a design review and to support final documentation.

The data shown above is not used in the manufacture of the final product, it is only used in the design development process to collaborate between two different systems. There are other methods to accomplish the goal, and your company or customer may suggest an alternative, but the intent here is to illustrate one of the design data related activities that you may be participating in.

QUOTING

Before the design is finished, the purchasing department may ask you for enough information to get a budgetary quote in advance. A formal Fabrication Drawing provides everything a bare board fabricator needs to know about the product, but the documentation cannot be completed before the layout is finished. In the meantime, cost analysis and paperwork can start if you can provide the basics.

For Quoting, they will want to know:

• Board Size (area) and Thickness
• Board Cut-outs or Slots (if any)
• Number of Layers
• Approximate Number of Holes, and Smallest Hole Size
• Smallest Trace Width and Clearance
• Final Finish Required
• Quantity of Boards and Turn-around Time
• (maybe Number of Lands top&bottom for test purposes)

Even if some of these estimates change slightly before the design is finished, most fabricators are willing to provide a budgetary quote as long as they can adjust the price if there are significant changes (like the number of layers, for example)

DESIGN PROCESS MILESTONES
Throughout the design process there will be several different people using your data. After you work through a few designs, start recording the steps that you did to get from start to finish, and who needed what along the way. Then re-arrange the steps where possible to get the data to the people who need it AS SOON AS POSSIBLE. You don't want to create bottlenecks for others, and it's better for YOU to be waiting on THEM than it is for THEM to be waiting on YOU.
Think about it....

Ok, those data types were needed during the circuit board development cycle, but at the end of the process you need to create two major data packages; one for bare board fabrication and one for assembly&test.

Let's look at each of these packages:

The Fabrication Data Package

Artwork

Most commonly referred to as Gerber Data, the artwork is one or more ASCII data files that describe a graphic image of each conductive layer of circuitry, soldermask layers for top and bottom, and silkscreen layers if desired.

The Gerber data format was developed by Gerber Scientific in 1980 as an input to control a photoplotter. Each plot file describes a single layer. Similar to a pen plotter but instead of using ink on paper, the photoplotter uses a combination of draws and flashes to create the image on film using a beam of light. Different sized apertures were used to control the width and shape of the exposure, so when using the original Gerber format (based on a subset of EIA RS-274-D), an aperture list was also required. Gerber files using the newer format (RS-274-X) have the aperture information embedded in each plot image data file.

To provide the most simple illustration possible, the following commands (in the left column) can be fed sequentially into a photo-plotter to draw a a four inch square with an eight mil line:

Example Gerber Data File Draw a Four Inch Box with an 8mil Line
*G04 "DRAW BOX"	G04 means "ignore", Used for comments
%MOIN*%	Set units to inches (parameters start & end with % character, data ends with * character)
%FSLAX23Y23*%	Format statement: data is formatted with "no leading zeros" and "2.3", (which means 2 digits to the left of the decimal point, and 3 digits to the right)
%OFA0B0*%	no offset (0:0)
%SFA1.0B1.0%	scale factor (1:1)
%ADD24C,0.008*%	Aperture Definition, set D-code position 24 as an 8 mil circle
G54D24	"Get Tool" command, load D-code 24
X0Y0D02*	Travel to starting position with "exposure off"
X4000Y0D01*	Travel to first corner with "exposure on"
X4000Y4000D01*	Travel to next corner with "exposure on"
X0Y4000D01*	Travel to next corner with "exposure on"
X0Y0D01*	Travel to last corner with "exposure on"
M02*	End of data, shut down

In this way, layers of circuitry can be exposed onto film by DRAWING exposures with apertures specified by WIDTH, and FLASHING exposures in specific locations defined by SHAPE (circles, rectangles, etc.)

The same file format is used to define graphic layers for ink legend (silkscreen) and protective coating (soldermask). It is also used to define the paste screen which is used during component assembly.

For more information, download the Gerber Format Specification from Ucamco

MOVING FORWARD.... QUICKLY

The Gerber Format was developed to control a photoplotter using draws and flashes, but modern CAM systems can read in all the data at once and rasterize a complete image for each layer. This is much faster than drawing/flashing each feature sequentially.

Since Gerber files are a bizarre type of ASCII plotting commands, they are difficult to interpret without a viewer. None of the standard computer applications can display them. Fortunately, there are several shareware Gerber Viewers available which you can download and install free of charge. Search the internet for "Gerber Viewer". You can't go wrong using ViewMate or GC-Prevue, but there are others. (not promoting favorites, I just haven't had any experience with the others)

Drill Data

Two more types of ASCII files are used for Numerically Controlled Drilling (NCD) data.

A Tool Table lists the diameter of each drill size and assigns them to tool numbers, and gives instructions about how to interpret the drill data.

DRILL TABLE
Position  Diameter Maximum  Minimum Plated
1         0.03000  0.03300  0.02700    yes   
2         0.05500  0.05800  0.05200    yes   
3         0.15700  0.16200  0.15600     no    
DRILL FORMAT
Drill machine coordinate mode is ABSOLUTE
Drill machine supports INCH units
Scale is 1.000 
Data format is 2.3
Drill machine modal coordinate is OFF
Leading zeros are PRESENT
Trailing zeros are PRESENT
Drill machine origin (x, y) at (0.0, 0.0)
Drill machine command block end char is ''
Drill machine stop code is 'M30'

The Drill Files contain hole locations for each drill sorted by Tool Number, and usually separated into plated and unplated

G90
M72
T1
X01950Y-01900
X02050Y-01900
X02250Y-01700
X02350Y-01700
T2
X01950Y-02017
X01950Y-02217
X01950Y-02417
X01950Y-02617
X01950Y-02817
X01950Y-03017
T3
X01375Y-01450
X01375Y-03750
M30

As a supplement to the ASCII data files, it is customary to provide additional information related to drilling on the fabrication drawing in the form of a HOLE LEGEND or DRILL CHART. During quoting and for quality inspection activities, this summary is easier to read than having to interpret the raw data. Drill sizes are given unique symbols or letters, and the pictorial representation of the board on the drawing will show these symbols as a visual aid. Here is a typical chart:

These examples were shown to familiarize you with the components of a complete data package, but in actual practice you will probably not have to worry about the formats. Once it has been configured correctly, most CAD systems will automate this task for you.

Netlist

The netlist file will also be created automatically by your CAD system, but I placed it last in the list of data files because it is not always included in the data package by every customer. A bare board can be fabricated without a netlist, but if it is available an extra level of checking can help ensure that the product will work as the designer intended.

The netlist file should be in the IPC-D-356 format, but an example will not be shown here because it is too complicated to understand at a glance, and it truly won't help you in your daily life to know the codes. If you want to learn more about netlist formats see the IPC-D-356 specification, but your software will create it for you and you will never even have to open it.

Fabrication Drawing

The Fabrication Drawing fulfills several important functions to support the circuit board manufacturing process:

• It provides enough information about the design for the bare board fabricator to prepare a quote
• It adds all the extra details about the build that aren't easily incorporated into the data files, like material and final finish
• It lists the criteria by which the finished product will be evaluated for acceptability
• It serves as a tool to be used during final inspection
• It is a record or document to store the history of a product by title, part number and revision; physical dimensions, and lists the name of the designer and possibly several other supporting entities as well as the company name and address, etc.

Several different types of information can be found on a typical fabrication drawing, including Design Parameters, Board Details including Construction, Materials and Process Specification, Conductor and Clearance minimums, Fabrication Allowances, Marking Requirements, Soldermask, Silkscreen and Final Finish, Test Coupon requirements, Test requirements, Performance requirements, and a Graphical Representation of the board with Critical Dimensions.

Most of these topics are covered by a few "building blocks" that you will find on most drawings. The DRILL CHART has already been shown in a previous section, and next we will look at a LAYER STACKUP or CONSTRUCTION detail, and a set of typical drawing NOTES.

Here is a good example of a board CONSTRUCTION detail taken from the IPC-2614 publication "Sectional Requirement for Board Fabrication Documentation" (not all designs will need to have precise dielectric spacing or impedance control).

The notes area is like an Instruction Manual for manufacturing your product. Many of them will reference acceptability requirements that will be introduced in the next section. For now, just try to get an idea of the type of information they contain. (all dimensions are metric)

NOTES - UNLESS OTHERWISE SPECIFIED:

FABRICATE TO MEET OR EXCEED THE REQUIREMENTS OF
IPC-6012 FOR CLASS 2 AS DEFINED IN IPC-6011. 
MINIMUM TRACE WIDTH .15, MINIMUM CLEARANCE .15 

MATERIAL: LAMINATE FLAME RETARDANT EPOXY-GLASS 
PER IPC-4101/126, 170 DEGREE C MINIMUM Tg, 
DECOMPOSITION TEMPERATURE 340 DEGREES C MINIMUM,
T288 DELAMINATION TIME OF 35 MINUTES MINIMUM, 
MAXIMUM THICKNESS EXPANSION OF 3% FROM 50?260 
DEGREES C.  
PREPREG MATERIALS PER /126 SHALL MEET THE SAME 
REQUIREMENTS. 
INNER LAYER FOIL PER IPC-4562, TYPE E, GRADE 3,
CLASS 2. 

PLATING: ELECTRO-DEPOSITED COPPER, HOLE WALL 
PLATING AVERAGE MINIMUM .030, NO LESS THAN .025

FINISH: IMMERSION SILVER PER IPC-4553.

REGISTRATION: MINIMUM ANNULAR RING .0254, NO 
BREAKOUT ALLOWED, TEARDROPPING ALLOWED IF MIN 
CLEARANCE MAINTAINED.

FABRICATION: NON-FUNCTIONAL INNER-LAYER PADS 
SHALL NOT BE REMOVED FROM LAYERS 1, 2, 3, N-2,
N-1, AND N. 
THIEVING IS ALLOWED IF 2.54 MINIMUM CLEARANCE 
TO CONDUCTIVE FEATURES IS MAINTAINED

SOLDER MASK: LPI BOTH SIDES OVER BARE COPPER 
PER IPC-SM-840, CLASS T, .02-.05 THICK, COLOR:
MATTE GREEN. ALL FIDUCIALS, LANDS AND HOLES, 
EXCEPT VIAS, SHALL BE FREE OF MASK MATERIAL.

SILKSCREEN: WHITE NON-CONDUCTIVE EPOXY. INK 
MUST WITHSTAND PEAK TEMPERATURE OF 260 DEGREES 
C 60 SECONDS, 3 CYCLES WITHOUT DISCOLORATION.  

MARKING: VENDOR LOGO FOLLOWED BY 94V-0 AND 
FOUR-DIGIT DATE CODE.

FINISHED THICKNESS 1.6 +/-10%

There are many other types of notes and infinite variations (refer to IPC-2614 Fabrication Documentation for more examples and in-depth explanation), but this set is fairly standard and simple. The exception above is that the Material note is calling for laminate and prepreg materials that are suitable for higher temperature Lead-Free processes to meet RoHS requirements (Restriction of Hazardous Substances). More about that later...

ReadMe.txt

Including this file into your data package gives you an opportunity to cover anything else that cannot be addressed by one of the other files. For example, you may have intentionally shorted two nets together (like AGND and DGND) and you don't want the fabricator to put your job ON HOLD because of a netlist discrepancy. A README.TXT is the place to include additional notes that you may not want to show in the final documentation. This is also a good place to list yourself or someone else as a contact, with name, phone number and email address.

The IPC developed a "PWB Fabrication Data Quality Rating System" called IPC-2524, which describes common problems with fabrication data and includes a form which can be used as a checklist when setting up your data output process. It is distributed FREE of charge and is available HERE.
Left-click to VIEW, Right-click to SAVE

The Assembly/Test Data Package

Assembly Drawing

The centerpiece of an assembly drawing is a pictorial representation of what the finished electronic assembly should look like. The graphics will clarify component polarity, and provide details specific to the assembly. It will also list any special instructions and indicate what level of workmanship and acceptability is expected.

SolderPaste Data

If surface mount components are used in the design, they will be attached to the board using solderpaste. This solderpaste is applied to the surface of the board using a stainless steel paste screen, created with a Gerber file in the assembly Data Package. This gerber file is a graphic showing only the spots on the board where the paste needs to be. For each side of the board needing surface mount parts (two paste screens are required if there will be surface mount parts on the other side of the board) paste will be screened onto the land patterns, parts will be placed on to the paste, and then the whole assembly will be heated until the paste melts, which is called "reflow soldering".
Paste screen technology is quite sophisticated, and unless you really know what you are doing, you should provide paste screen apertures that are the same size as the lands you will be soldering to. This will give the paste screen manufacturer a known starting place to begin making modifications for various technologies.
An article about screen technology with some good photographs and useful illustrations was published recently by EMS007.
If that link doesn't work, try HERE.
Paste screen data file is in the same Gerber format as the artwork files in the bare board fabrication data package.

Component Placement Data

Components needed for the assembly are purchased in quantity, loaded onto reels of tape ("tape n' reel") or in plastic tubes ("sticks"). A component pick and place (PNP) machine has a specific number of feeders that are loaded with these tubes and reels. After solder paste is applied to the land patterns of a bare board, it is loaded into the pick-and-place machine where a camera aligns the board using little metal targets called fiducials (usually 1mm diameter round dots etched into the surface conductor layer). Then components are picked up one at a time and placed on the board in specific locations at the proper rotation. An ASCII data file contains these X and Y coordinates and rotation for each part, and it looks like this:

FD1  0       b_fmark  0       0.15    1  0  
FD2  0       b_fmark  0       7.25    1  0  
FD3  0       b_fmark  5       0.15    1  0  
C1   pn1001  c0805    1.8125  2.2100  2  180
C2   pn1001  c0805    1.5000  1.9500  2  90 
C3   pn1001  c0805    1.4000  1.9500  2  90 
U1   pn1002  tsop65   1.3000  1.9500  1  90 

The first three lines are fiducial locations used by the camera to align the bare board precisely before component placement begins. After that, each line is a separate part number listing the reference designator, the land pattern name, the X and Y coordinates, which side of the board the component is on, and the rotation of the part. The three capacitors are mounted on the other side of the board. Top and bottom components would usually be separated into different groups, but are shown together in the example above for illustrative purposes.

Netlist

A netlist may be not be required to complete the assembly, but should be included as a reference for the design intent. Most CAD systems can export a netlist in IPC-D-356 format, but if yours is not one of them (Mentor BoardStation, for example), sometimes they can extract what they need from the ASCII database (Mentor Neutral file, for example).

If a netlist is available, the bare board fabricator can compare the connectivity of the Gerber Data to the design intent, and alert you about any discrepancies before time and materials are wasted.

Test Point Data

If the development of an In-Circuit Test (ICT) is planned, a list of test point locations will be used to position the test probes in the fixture. Here is a brief example of the Test Point file:

TESTPOINTS REPORT
Total via testpoints: 6
Total pin testpoints: 2
Name   X-Loc  Y-Loc  Side    Rotation  TestSet
t3708  0.0    0.0    Bottom  0         None
X-Loc  Y-Loc  Net    Side    Pad Style Pin   Probe
0.925  1.525  RESET  Bottom  Thru-Via  U1-2  p100
1.5    2.325  CLOCK  Bottom  Thru-Via  U1-3  p100
8.675  5.9    +5V    Bottom  Thru-Pin  C1-1  p100
8.55   6.8    +5V    Bottom  Thru-Via  U1-8  p100
10.25  0.05   DATA1  Bottom  Thru-Via  U1-6  p075
9.1    3.325  DATA2  Bottom  Thru-Via  U1-7  p075
0.775  2.15   GND    Bottom  Thru-Via  U1-4  p100
6.525  1.525  GND    Bottom  Thru-Pin  C1-2  p100

Many of the details related to Design For Testability (DFT) are beyond the scope of this tutorial, but here is a brief list of the parameters you should keep in mind if a test fixture will be developed for your design:

Design for Testability

• Keep components and test points at least 3.2 mm (.125) from board edges (preferably 3.8 mm or .150 in)
• Provide at least two unplated 3.2 mm (0.125) diameter tooling holes, preferably in opposite corners, and leave 3.2 mm annular area around them free of components and test points. Consider using a "keying" pattern so boards can't be inserted backwards
• A double-sided test fixture is more expensive, so try to put all test points on one side of the board, usually the bottom or the side with the least circuit complexity. If top-side of board must be used for probe sites, use top only for non-critical nets. Keep test points for clocks, control pins, programming pins, serial data and boundary scan on bottom.
• Test point sites can be through-hole leads, dedicated pads or small diameter vias, but avoid placing test points on surface mount lands or gold-plated edge fingers. Don't use larger via diameters as test probe sites. Via hole size should be 0.36 mm (.014) or less
• For 100% testability, provide at least one test pad for each net
• Provide two pads on nets tied to critical low impedance devices (four-wire Kelvin testing)
• Provide 2-10 probe sites for primary power, and two test points each for isolated power/grounds. For primary ground provide many probe sites, one test point for every twenty grounds, or consider a grid of at least one per square inch
• Probe sites with 1.0 mm (.040) pad diameters are preferred, 0.9 mm (.035) is acceptable, 0.8 mm (.031) can be used if tooling holes are available for alignment, but smaller diameters will reduce contact repeatability
• Try to space probe sites at least 2.5 mm (.100) apart, center-to-center. In reality, 0.9 mm (.035) pads spaced 1.8 mm (.070) is considered standard by many. Closer spacing is possible but will require using thinner, less reliable and more expensive probes.
• Test points should be evenly distributed over the surface of the board. High stress in congested areas can cause board to warp.
• Keep tall components on the side that is not probed. The platen has to be cut out in places where components are over 6.4 mm (.255) tall on the probed side. For these, keep test points at least 5.0 mm (.200) away.
• For components taller than 2.6 mm (.100), maintain minimum 2.0 mm (.080) clearance edge-to-edge. For all other components, keep test pads at least 1.0 mm (.040) from component body, edge-to-edge.
• If Component Through-holes are used for test probe locations, make sure leads are robust enough for compressive force (be careful using LEDs or some types of transformers). Also, make sure PTH leads will be present on all versions of assembly (not depopulated)
• If design is panelized, try to include at least one tooling hole on each board in addition to the tooling holes in rails

Those are the most basic rules for test point assignment and placement, but much more information can be found in the Surface Mount Technology Association publication SMTA-TP-101 "Testability Guidelines", available HERE

ReadMe.txt

This is the place to include additional notes that you may not want to show in the final documentation (most of the notes should be listed on the assembly drawing). This is also a good place to list yourself or someone else as a contact, with name, phone number and email address.

Compressed Archives

To keep related files together, these sets of data are often combined into compressed archives (with file extensions ZIP, RAR or TAR). The resulting archive is a single file that can be transferred easily between customers or suppliers, and the individual files can easily be restored at the destination.

Three of the most important advantages of compressed archives are:

• Compressed archives keep necessary components of a package together, making organization easier and reducing the chance of missing files
• Compressed files are much smaller, needing less storage space, less time and less network usage for transfers
• The software that compresses and uncompresses archives has automatic built-in error checking

Thanks to all the fabricators who have helped me get my data OFF HOLD