| Sending Files At Enigma Interconnect we are continuously striving to meet or exceed your needs. Our ability to provide the highest quality, as well as shorter production cycles, begins with the information package you provide us. We have provided this guide with the intent of answering the most common questions relating to the creation of a complete PCB documentation package as pertains to manufacturing. We have also included a section on manufacturing considerations to be taken into account during the design phase. This guide is designed to be used by our customers and as such, we welcome your input. Any comments or suggestions on the content or presentation of the information herein would be greatly appreciated. We thank you for your cooperation in following the guidelines presented here to help ensure the information we receive is complete and in the required format. Photoplotting Principles © Copyright Graphicode Inc 1990,1996 All Rights Reserved You can use the hyperlinks below to locate a particular topic of interest or read the document from the beginning. What Is A Photoplotter? A Photoplotter is just what the name implies: an plotter that writes using light. A plotter has to be told:
There are two major types of Photoplotters, "Vector" and "Raster" (or "laser"). Each handles apertures differently. 
Vector PhotoplottersVery few vector Photoplotters are in use any more. This information is provided primarily as a historical background for understanding laser Photoplotter terminology. Aperture Wheels Traditionally, the Photoplotter counterpart to a pen plotter's pen rack has been the aperture wheel. The aperture wheel is a disk with 24 or 70 apertures arrayed radially along its circumference. When the Photoplotter selects an aperture, the aperture wheel is rotated to place the desired aperture between the light source and the film. Apertures are themselves pieces of film and can be made to any shape required, although in practice this is a time-consuming process and there is a physical limitation on size. Flash and Draw Apertures To achieve constant exposure on a vector Photoplotter, apertures used for flashing pads are filtered differently than those used for drawing traces. Therefore, Flash and Draw apertures cannot be used interchangeably without risk of localized over-exposure and under-exposure.
Aperture
Wheel Setup for Vector PlottersThe setup of an aperture wheel is an exacting and time consuming process since each aperture in the wheel must be hand-mounted and aligned. In order to avoid repeated setup costs, designers have the Photoplotting vendor keep a wheel on file and are forced to always use that same set of apertures. This has obvious drawbacks, both in terms of design flexibility and the ease of migration to other vendors. RS-274D files were not designed to communicate any information about the apertures in use, only to specify where they are used. This has led to a great deal of confusion between designers and fabricators since designers aren't aware that a Gerber file alone is not sufficient to define the board - an external document describing the apertures is also needed.
Raster (Laser) Plotters Aperture Lists Increasingly, vector Photoplotters are being replaced by the laser Photoplotter, which emulates the older style machine in a raster (bit-map) fashion. While use of the term "aperture" to describe a pad or trace shape persists, the term "aperture wheel" is now being replaced by "aperture list", which implies the greater flexibility now available to the designer. There are four principle advantages with aperture lists on raster plotters:
Flash
and Draw AperturesNo distinction need be made between Flash and Draw aperture types since the light source intensity is constant.
Speed
Advantage of Laser PlottersLaser plotters operate much quicker than vector machines. A complex plot that required hours on a vector machine can usually be performed in ten minutes or less on a laser Photoplotter. This decreases turnaround time and in many markets has driven Photoplotting costs down.
Talking
to PhotoplottersThe de facto standard for Photoplotter data is the Gerber format, more properly known as RS-274D. The term Gerber refers to the Gerber Scientific Instrument company, a pioneer and leader in Photoplotter manufacturing. Popular variants include Extended Gerber ("RS274X") and MDA FIRE AutoPlot, both of which embed the aperture list information in the file. RS-274D is a variation on traditional Numerical Control (NC) machine tool languages. It differs from traditional NC formats (i.e. drill data), as far as its use of tool selection codes but is otherwise compatible. RS-274D data is organized in "blocks". A block consists of a combination of codes:
An RS-274D code consists of a letter D,G,M,X,Y,I or J followed by a numerical value. These codes designate the following: * - End of Block (end of command) D - Select aperture, or set aperture use mode X - Move to X value Y - Move to Y value G - Various setup codes M - Various control codes I - Relative X location for arc center J - Relative Y location for arc center
D CodesD codes have multiple purposes. The first is to control the state of the light being on or off. Valid codes for light state are D01, D02, and D03.
There are two distinct ways to number an aperture list. The traditional 24 aperture system started with D10 - D19, jumping suddenly to D70 - D71, then back to D20 - D29, ending with D72 -D73. This is still a common format for output for CAD packages, and is still mandatory for old 24 aperture Gerber vector Photoplotters. It is now common to start with D10, then increase numerically in steps of 1 (D10, D11, etc.) continuing up to D70 and beyond, rarely beyond 1000 individual apertures.
X
& Y CodesThe X & Y values in the Gerber file determine where the aperture shape and dimension will be positioned and drawn. X & Y values are used as coordinate pairs to determine where the light will be exposed, using the D codes shapes (i.e. D10) and light exposure status (i.e. D01, D02, D03) for drawing lines and arcs, as well as moving between drawing entities. Here are a few examples of using X & Y codes with D codes.
G CodesG codes are used to configure the Photoplotter. Commonly implemented codes include:
A common situation where G codes are mandatory for all machines is when the data is switching from vectors to arcs and vice versa. When switching from drawing vectors (G01) to drawing arcs (G02, G03), the controller must be informed of the change of mode. Another important case for G codes is when determining if the arc is a quadrant (G74) or Full 360 (G75). Quadrant arcs never cross quadrant boundaries, because the center coordinate offsets (I,J Codes) are always unsigned (even if they are negative!). Therefore, it requires at least four G74 arcs to draw one complete circle. Center coordinate offsets for 360 arcs (G75) can be positive or negative, allowing for a single command to draw a complete circle. In either case, the center coordinates are given relative to the start point of the arc. The most dramatic difference between Quadrant and Full 360 arcs is that a Quadrant arc with identical start and end points has a sweep of 0 degrees, whereas a similar full 360 arc is a full circle. The G90 code tells the machine controller that all data following is absolute data. Hence, if following X & Y data follows, the controller will move to the absolute value given by the X & Y value. G91 tells the machine controller that all data following is incremental data. The machine will move the data by the amount of the X & Y value, rather than to the absolute coordinate point. Example: X1000Y1000D02* X3000Y3000D01* In absolute mode (G90), the machine will first move to coordinate point X1000 and Y1000 with the light off, then draw a line to coordinate point X3000 and Y3000 with the light on. In incremental mode (G91) the machine will first move to coordinate point X1000 and Y1000 with the light off, then draw a line to coordinate point X4000 and Y4000 with the light on. This was done by adding X1000 + X3000 = X4000 and Y1000 + Y3000 = Y4000. Here are some more examples of G code usage in conjunction with X, Y, and D code values:
M CodesM codes are used for machine control. Here are the most commonly used:
I & J CodesWhen you encounter an I & J code in a Gerber block, you have found an arc command. Arc commands come in two flavors, Full 360 or Quadrant. The Gerber arc command is very complicated, and this section will only briefly describe usage of the Gerber arc. Full 360 arcs allow the plotter to draw a full circle (360 degrees of arc) in one single command.. Quadrant arcs only allow for an arc to be drawn through a maximum of 90 degrees of arc, never crossing a quadrant boundary. Due to this restriction, I and J arc center offset codes can get away with never having a negative value, even if the offsets are negative! When in a Full 360 arc (G75), only one command is required to draw a circle. In Quadrant mode, the same circle would require at least 4 Quadrant arcs (G74), because a circle goes through all four quadrants. Quadrant arcs will always have positively signed I and J values, even if the center offset is actually negative. Full 360 arc center offsets can be signed positively or negatively. A negative I or J is a sure indicator of Full 360 arcs.
ModalityIt is often the case with Gerber data that when moving from one XY coordinate point to another XY coordinate point, the X or Y value will not change. Likewise, it is likely that if the plotter is drawing a line with multiple segments, the segments will be connected and the light stays on from segment to segment. In both of these cases, there are redundant commands, making the plot data file larger than necessary. RS-274D allows you to omit this redundant data. This example shows a box being drawn with four corners.
For example, in a "2,3" format the value 12.345 is written "12345". In a "2,4" format, the same value is written "123450". Zero suppression comes in three flavors - leading, trailing and none. The idea of zero suppression is to reduce data file sizes by eliminating unneeded 0 characters. The simplest and most common form of zero suppression is leading zero suppression. In a "2,4" format, with no zero suppression, the value 0.0100 would be 00 + 01000, written as "000100", but with leading zero suppression the same value is written as "100". With trailing zero suppression the same value 0.0100 would be written as "0001".
How To Describe Data FormatsGerber data and other XY languages use a standard method for describing the data format. Two examples include: "2,3 leading inch" or "3,3 trailing metric". The first number specifies the whole digits used. The second parameter states the precision. "Leading" and "trailing" pertain to the zero suppression. And the last part of the description indicates the units. Refer to the above sections if these concepts seem unclear.
Typical
Documentation PackageA typical package must include the following information:
Image DataGerber (RS-274D or RS-274X) files must be provided for all image layers (i.e. all circuit layers, solder mask(s) and legend(s)):
Note: RS-274X format (Gerber data containing imbedded aperture
information) is the preferred file format, but it is susceptible
to errors typically associated with custom shape definitions. It
is advisable, that prior to sending us any quick turn work that
you send us sample data so that any bugs can be identified and worked
out ahead of time.
Note: Aperture lists must be entered into our CAM software in order to correctly view your Gerber data. Aperture lists, when entered by hand, are susceptible to human error. A more desirable method is to use software to convert the supplied aperture table. Circuit Graphics has software to convert aperture lists output from the most commonly used CAD packages to a format recognizable by our CAM software. For this conversion process to work, you must tell us what your CAD package is and ensure that you do not edit the aperture file in any way. We have conversion programs for the following CAD systems:
Drill Data Most CAD packages offer a utility which will output a drill file in Excellon drill format (an industry standard). We require the ASCII version of this file, as opposed to EIA or Binary. Along with the drill file we require a report file which provides the finished hole size and total hole count for each tool change. Any non-plate through holes (NPTH) should also be clearly identified. The report file may be supplied as a separate ASCII text file or may be included as part of your Read_me.txt file.
Fabrication
DrawingThis drawing may be supplied in either Gerber, HPGL, DXF or hard copy form. This drawing will be used as a reference during the manufacturing process and should provide the dimensions for the board profile as well as the size and location of any internal routs. Drill hole locations along with a hole chart should also be included. Ensure that any non-plate through holes (NPTH) are clearly identified. It is good practice to reference the perimeter of the board to a feature such as a tooling or board mounting hole.
Preparing
The OrderGetting your digital data to us is only half the battle. We need some additional information about your data formats, PCB specifications and order requirements. The following information must be supplied with each order. We suggest that you use your favorite text editor to prepare a "template" similar to the following one, which you can modify slightly for each order. Include this file with your data files, giving it a creative filename such as READ_ME.TXT to attract our attention. Please supply this file in ASCII text format to ensure that we can read it.
Sample Order96/09/20 10:56 AM To: Enigma Interconnect Inc From: Name Company Address Phone: ____________ Fax: _______________ PO Contact: ____ Technical Contact: _______ PCB Name/Part No.: ________ PCB Rev. ____ P.O. Number: _____ New Design: ___ Previously Mfg.: ______ Required Delivery Quantity 30 Hours (hot rush) _______ 3 Days _________________ 5 Days _________________ 10 Days ________________ Standard _______________ The Following Files Accompany This Job: (note: file names are samples only)
General Specifications The information provided below is used for quotation purposes and should be as accurate as possible.
Sample Drill Report File
Checking
Your DataBefore sending any data, we advise that you check the files by viewing them using some form of Gerber view software. For your convenience we provide a Shareware version of Graphicode's "GC PREVUE" in the Software Tools section of our website. If you have used GC PREVUE to check your files and are satisfied that they loaded correctly and look right, you may then save the files as a ".PWK" or ".CWK" file (see GC PREVUE manual "Save All Work"). You can then send the ".PWK" or ".CWK" file instead of your Gerber files and NC Drill file (if loaded). We still however, require you to send your Drill Drawing, Fabrication Drawing and Read_me files.
Data TransmissionOnce your data is assembled, you may send the digital portion to us on disk or by sending the files as an "attachment" to an e-mail via the Internet. We are capable of receiving data using the following:
Internete-mail: sales@enigmacorp.com World Wide Web: www.enigmacorp.com For convenience and economy of time, we recommend that you place all of your data files, FOR EACH INDIVIDUAL JOB, into a single archived file before transmitting. Shareware versions of PK Software's PKZIP and PKARC are available in the Software Tools section of our website.
Manufacturing
ConsiderationsAll boards are manufactured to IPC Class 2 specifications unless otherwise specified at time of quotation.
LaminateDouble & Single Sided
Circuit
Layer FeaturesConductor Width/Clearance
Inner Layer Clearances: 0.015" isolation clearance should be maintained between inner layer features and finished hole size. Annular Ring Requirements Ipc-D-300g 3.1.3.1 The minimum annular ring is the distance from the edge of a functional land to:
Land Size Determination Ipc-D-300g 3.1.3.2 The minimum size of a land surrounding a hole in a printed board shall be determined by considering the following.
Minimum Land = a + 2b + 2c (if required) + d All lands and annular rings shall be maximized wherever feasible, consistent with good design practice and electrical clearance requirements.
Finished Hole Size Smallest finished hole size (plated) is 0.010". Board Edges IPC-D-300G 3.2.1 One board edge should be located from a datum, and where applicable other edges should be dimensioned from the same datum. Where board outer edges have a relationship to each other they shall be dimensioned using a single dimension to maintain that relationship. Board Edge Tolerances Ipc-D-300g Table 4
Plated/Unplated
Holes
RoutingThe following router bit sizes are stock:
Tooling HolesAll boards/pallet require min. 3 non-symmetrically placed tooling holes. If not provided for in the design, Circuit Graphics will add holes as required.
Solder Mask Feature Clearance Solder mask clearances should be 0.005" minimum. i.e. A 0.050" circuit layer feature would have a 0.060" solder mask feature. Solder Dam Solder dams between SMT pads must be a minimum width of 0.005" .
Component
LegendFeature Width Line widths should not be thinner than 0.008" with text heights not less than 0.060". Feature Clearance 0.008" clearance should be left between legend features and the edges of SMT pads or holes for through mounted components.
ScoringFeature Clearance Circuit features should be kept a minimum of 0.025" away from scored edge. Available Cutters Standard Blade: 30 Available Blade: 60
Gold FingersFeature Clearance 0.030" minimum clearance must be maintained between edge of gold finger and plated through holes. |
||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||
