Printer Friendly

Working with fabricators: tricks of the trade: designers, don't overlook these simple steps for preparing the design the right way.

As with Web design in the past several years and desktop publishing before that, circuit board design has evolved from the responsibility of a few technical elites to part of the day-to-day job of engineers in all industries. To a large extent, that shift has been made possible by advances in software that make it simpler and faster to create designs. However, many engineers new to PCB design may not be aware of some of the tricks of the trade that can mean the difference between success and failure once their design reaches the manufacturer.

1. What you see isn't always what you get. Don't assume that what you see in your design software is what the manufacturer will see. There are sometimes wide variations between what the design software shows and the output in the Gerber files. It's wise to use a third-party review to check your design.

2. Fab notes: they're notes, not a novel, When providing fab notes, limit the number of notes per board to as few as possible, and avoid the temptation to cut and paste notes from a previous design. While it saves time, you may end up including notes that aren't applicable to your design, increasing the chances that notes specific to your design may get lost in the shuffle.

Take advantage of the existing industry standards. A good example of this is IPC-6012, which addresses almost all requirements pertinent to the performance and appearance of most commercial rigid boards.

It's much simpler, and infinitely more useful to the manufacturer, to simply refer to the IPC specification to which you want the board built. Instead of detailed descriptions, which are open to interpretation by the manufacturer, specify "Build to IPC-6012, Class 2." (A complete listing of the specs can be found at ipc.org.)

3. Design rule checks. Getting an objective, third-party check of your design, either from a fellow engineer or from a service provider, is critical before submitting a design to a manufacturer. First, this ensures that the manufacturer will not make changes to your design in order to properly produce the board--changes which could affect the way the board will work. Second, it helps guarantee that the board won't get held up in production and delay the project.

4. Dollars and sense. Calculate the cost of your board as you design it. This may allow you to change the number of boards you've created or the design of the board to reduce the production cost. It's a good exercise that could not only save your company money, but it may spark innovative thinking and help you develop a better, less costly method of producing something. Some fabricators have online pricing matrices that calculate the costs of the board as you put it together.

5. Can you reach me now? Provide an after-hours contact number and/or email address where you can be reached. Some fabricators have technical support around the clock during the week to ensure your delivery. Know your fabricator's availability. If there is an issue on a time-critical order, you will want your fabricator to be there to help resolve it.

6. Check the checklist. Pilots don't take off, or even get into an airplane, without reviewing a checklist to make certain they are prepared for flight. Most PCB orders get put on hold because of a clerical error by the designer, so it behooves the designer to create a final submission checklist (which may include many of the above items) to review before sending a design file to a manufacturer.

Here's a list of items that typically prevent PCB orders from moving smoothly through the production process; incorporate them into a pre-order checklist:

1. Missing aperture list. An aperture list does not need to he sent with RS-274X format files. If RS-274D format is sent, the aperture list will be used in combination with the Gerber files to create the artwork. The Gerber files specify what to do, and where. The aperture list specifies which tool to use. Therefore, you need only output one comprehensive aperture list for all layers, rather than a separate aperture list for each layer.

2. Missing Excellon drill file. The manufacturer uses the Excellon drill file to determine what size holes to drill and where. Plated and non-plated holes should be included in one drill file, with plated and non-plated holes having different tool numbers. Nearly all layout packages will output an Excellon drill file, so producing one with your order shouldn't be an issue. If it is, most manufacturers can create one from the fabrication drawing.

3. Missing tool list. Manufacturers use the tool list in combination with the Excellon drill file to create the drill, which specifies where to place the holes. Your tool list specifies what tool to use. The tool list should be embedded in the Excellon drill file or sent as a separate text file. Using a tool list provided on a fabrication drawing is not preferable, as it eliminates many automatic verifications and makes data entry errors far more likely. If your layout software outputs an Excellon drill file, it will also output a tool list.

4. Insufficient annular ring. Annular ring is the donut ("annulus") created when your drill pierces a copper layer. It is defined as the radius of this donut. For example, a 0.030" pad with a 0.020" hole would have a 0.005" annular ring. This is required to allow for complete plating on vias, as well as solderability on component holes. All layout packages provide this as a DfM check. Setting sufficient annular ring in your layout software is the preferred method, as copper spacing will be maintained.

5. Copper trace width/spacing. Copper spacing is the minimum air gap between any two adjacent copper features. Trace width is the minimum width of a copper feature, usually traces. All layout packages provide this as a DfM check. Setting sufficient trace width/spacing in your layout software is the preferred method. Trace width and spacing push and pull against one another, so changing a problem area may require rerouting traces, adding vias, or moving components.

6. Insufficient inner clearances. Inner clearance is the minimum distance from the edge of a hole to any adjacent, unconnected, innerlayer copper. Sufficient inner clearances help ensure that your drill does not cause shorts to the inner copper layers. This is important for both plated and non-plated holes, as non-plated holes may either cut into an adjacent trace or cause shorts during assembly. Fabricators can resolve most inner clearance issues if negative image inners are provided, but it is preferable to not modify these. Setting these clearances in your layout software is the preferred method, as this will maintain the intended connectivity. While most layout packages provide this as a DfM check, not all do. Those that do not can usually be manipulated to check for this violation by setting spacing and annular ring higher. A rule of thumb: Spacing + annular ring = inner clearance. Another trick that can help resolve problem areas is to move the affected traces to outer copper layers, where this is not an issue.

7. Board outline. A surprising number of PCBs are submitted without data telling the fabricator where to cut out the board. Faxed or hard copy drawings should be avoided. The best format is the same as for your artwork: Gerber. This permits the fabricator to easily compare your board outline to your artwork to identify potential problems.

Take your time and remember the carpenter's rule: Measure twice, cut once.
TABLE 1. A Short Guide to Fab Notes for Commercial PCBs

SUGGESTED TEXT COMMENTS

Boards shall conform Save time. This simple statement addresses
to IPC-6012, class 2 almost all requirements pertinent to the
 performance and appearance of most commercial
 rigid circuit boards. Be aware that class 3 can
 add significant premiums to the bare-board
 cost.

Material: FR-4 Specify min. Tg only if the application
 dictates this as a requirement.

Finished thickness: 0.062" is by far the most common finished
0.062" +/-10% thickness specified. Other common thicknesses
 are 0.020", 0.031", 0.040", 0.093" and 0.125".
 Standard tolerances are +/-10%.

Min. finished copper Unless ordering a controlled-impedance PCB,
on the surface: 1 oz. count on only specifying the min. copper
 weight; the max. will vary based on copper
 distribution and other fabrication issues.

Min. plated copper on This is a typical specification for a 1 oz.
the hole wall: 0.001" finished copper PCB. Fabricators start with 0.5
 oz. foil for the base copper and plate 0.001"
 on top of that. The result will be slightly
 over 1 oz. on the surface and 0.001" on hole
 walls.

Soldermask: Green is most common; black, blue and clear are
color--green, sides 2 usually also available. There may be a premium
 for colors other than green.

Legend: color--white, White is most common; yellow, black and red are
sides 2 also usually available. There may be a premium
 for colors other than white.

Place fabricator logo Add this note only if necessary. If the design
and date codes in the is an RF application, where the additional text
area specified (usually in copper, unless specified otherwise)
 will affect functionality, or there are other
 reasons that would dictate that these markings
 should be in a particular area, this should be
 specified. Provide an area clearly labeled in
 the fabrication print for these markings
 (designate an area approx. 0.300" x 0.300").

Layer stack-up Usually applies only to multilayer designs;
 however, if the contents of your files are not
 evident from the file names it is a good idea
 to specify the layers referring to the file
 names.


TONY BREGLIO is FreeDFM.com manager at Advanced Circuits (4pcb.com). He can be reached at 800-289-1724 ext. 337; tony@4pcb.com. Jim Hellmer is engineering support manager at Advance Circuits. He can be reached at 800-289-1724 ext. 338; jim@4pcb.com.
COPYRIGHT 2004 UP Media Group, Inc.
No portion of this article can be reproduced without the express written permission from the copyright holder.
Copyright 2004, Gale Group. All rights reserved. Gale Group is a Thomson Corporation Company.

Article Details
Printer friendly Cite/link Email Feedback
Title Annotation:Design Checklists
Author:Hellmer, Jim
Publication:Printed Circuit Design & Manufacture
Date:Mar 1, 2004
Words:1664
Previous Article:Design at the speed of 6 Gb/s: loss tangent and skin effect can degrade rise and fall times, blow noise and timing budgets, or worse. Good analysis...
Next Article:Cost modeling or price comparing? Complex tools aren't needed if what you want is to compare prices.


Related Articles
Analyze it! Designers and fabs look for different things, so both bear the burden of validation. (CAM Works).
Pride and respect: could the secret to improved performance be in how we treat each other? (ROI).
Who's afraid of the big, bad CEM?: lay out or miss out? Don't be bullied into revealing your costs of goods.
The crucial pre-construction phase.
What designers should know about LDI: not just a tool for fine lines, laser direct imaging eliminates phototools and tightens design tolerances....
Embedded passives material standard readied.
Built for speed: think cost is king? When it comes to quickturn work, designers value reliability and relationships over the almighty dollar.
Who is minding the technology store? If OEMs eschew technology development and others lack resources to fill the void, maybe serious industry...
Are you proactive or reactive?
Technical conference.

Terms of use | Privacy policy | Copyright © 2021 Farlex, Inc. | Feedback | For webmasters |