All designers have been in the situation where they complete a PCB design-barely by the scheduled due date-in order to get the design into the PCB manufacturer, and the issues and questions start streaming back from their CAM department. These issues lead to schedule delays and wasted time by the designer and manufacturing engineering people that could be better spent on meeting the next projects deadline. This article helps the PCB designers understand why this happens and how it can be eliminated by using The Continuous Design Improvement Model.
When a new design comes into a PCB manufacturer, the first step their CAM department takes is performing a design rule check (DRC). This is where the CAM operator compares the customer's design to their manufacturing capabilities and design for manufacturing guidelines. A report is generated that lists the items on the board that are beyond their manufacturers capabilities, and that also lists any issues where the design can be modified to improve yield and throughput and lower the cost to manufacture and assemble the board. If the designer were to use and not violate the same guidelines to design the board as the manufacturer used during the DRC check, this would eliminate three painful steps during the design and manufacturing process. Figure 1 illustrates the current and the desired process between the PCB designer and the manufacturer. As you can see, many non-value-added steps can be eliminated by understanding the process and using The Continuous Design Improvement Model shown in Figure 2.
The Continuous Design Improvement Model can be used to help the PCB designer, manufacturer and assembler understand each other's needs and requirements. The designer usually wants to push the limits of the manufacturer's capabilities and the manufacturer prefers a design that is "in the heart of its capabilities" so that the board will be easy to manufacture. The three basic steps (see Figure 2)-which are collaborations between the designer of the system(s) and the manufacturers that build them-are listed and detailed in the text that follows:
1. Set the design rules and data format used when designing the board.
2. Review existing designs for manufacturability.
3. Have a post-manufacturing meeting where you discuss what you have "learned by doing."
Step One - Design specification collaboration
The three players (designer, fabricator and assembler) will review the existing design specification or write a new one to be used when designing boards. Each player will bring to the table their critical items that need to be considered when designing and manufacturing. This spec will be used entering the design rules into the design workstation to generate the design through the PCB manufacturing and inspection through the assemblers manufacturing and inspection. As shown in Figure 2, any violations will result in issues for the PCB manufacturer and assembler. The items that will be included are:
Data Format - The optimal software format for an easy transition from design to manufacturing is ODB++. There are several reasons for this:
The data reads directly into the CAM system without effort. The data doesn't have to be manipulated in order for the CAM system to read the files.
The ERF file is provided with the data set. The ERF is the designer's design rules that can be used for manufacturing analysis.
The job matrix sets up a "stack-up set" so the data is in order as the board is being build. This allows the analysis to take place without renaming the layers and moving them into order.
The layers are pre-aligned; there isn't any extra data on the layers that needs to be removed or that potentially could cause issues.
The data set provides the components and their placement.
Data Package Requirements - The manufacturers will provide the designer(s) with a checklist that describes the items needed to produce the systems. The list will include:
One-up fabrication drawing. This data file will include the hole chart, tolerances, lay-up, notes on the materials and surface finish requirements.
Array drawings. If the boards are to be provided in multiple-up arrays, an additional fabrication drawing is necessary that includes the breakaways, all additional dimensions and tolerances.
Image data for all layers, including solder mask and legend. All layers are to be provided in separate files and are to be labeled for the manufacturer to easily interpret which layer they are.
Size does matter and smaller is better. The data file should be optimized to reduce the size of the file. This makes the file transfer from the designer to the manufacturer easier and the smaller file takes up less storage space on the server.
Manufacturer's Design Rules - These rules are the basic process and tooling guidelines used in producing and assembling boards. Usually the manufacturers can provide the design rules in a "seminar" to the design and manufacturing engineers. This seminar gives the designers an opportunity to understand why the requirements are necessary and it also builds the relationship between the designers and the manufacturers.
Array design specifications. V-scoring, breakaway, price tradeoffs for the number or X-outs allowed on the boards.
HDI and BGA routing optimization. With the tighter BGA package requirements, PCB manufacturers are meeting designers' routing needs by offering HDI capabilities. The manufacturers can (at a minimum) give designers the design rules for these designs. What we have been finding is that this is not enough. Most designers do not truly understand how to optimally design HDI product. Some manufacturers are offering design help to actually convert existing designs to HDI. They can, in some cases, reduce the layer count from 24 to 16 layers.
Fiducial location and size. Isolated fuducials with diameters below .050" should have a copper box surrounding it that is covered by soldermask. This will reduce the occurrence of being etched off.
Thieving and copper balancing. Areas with isolated traces or low copper density on a board cause manufacturability problems in copper plating and etching and lamination. With the addition of non-connected copper in the low density areas, this eliminates the manufacturability issues and gives the designer a more robust product.
Copper features distance from edge of board.
Tear dropping. This refers to an addition of copper at the transition of the trace to pad. It allows additional surface area for the drill to hit in case of misregistration. The designer may want to write in the specification that it is okay to add tear drops to existing designs without signoff.
Removal of non functional pads.
Place the complex circuitry on the inner layers of the board. Imaging and etching of inner layers is a much simpler process than outer layer.
Test pad versus test via pad size. This allows the manufacturers of the solder stencil to turn on and off the pads they do not want to coat with solder paste.
Controlled impedance stack-up call-out. On the fabrication drawing, many designers will specify the dielectric thicknesses between the layers. Different material types have different dielectric constants (DK). Usually, if a manufacturer used the designer's lay-up, it would not meet the specified controlled impedance. The designer's best bet is to state the desired impedance for the layers and the overall thickness, and the board manufacturer will use their lay-ups to hit the specifications.
Manufacturers Capabilities - The list that follows contains some of the specification highlights that need to be included in the design specification. The capabilities should be provided by the manufacturers with the technical roadmap to illustrate the direction the manufacturers are heading.
Line width and spacing
Hole sizes and manufacturing methods (mechanical, laser, plasma, etc,)
Legend size and width
Solder mask clearance
Hole size tolerance and plating thickness
Part size minimum for fabrication and testing
A PCB design specification that can be used as a reference when setting up the design guides for system design. If the specification is followed, there will a dramatically reduced amount of issues coming back from the PCB CAM group, and in turn eliminate the need for additional process steps.
Step Two - Design for manufacturability analysis
The three players analyze the PCB and assembly designs for issues with producing the board and assembling and testing it. They come to a meeting with the list of issues and improvement ideas and "negotiate" through their lists. The negotiation is between the designer pushing the limits of the system design and the manufacturers pushing back because of yield, throughput, and cost issues. The communication sounds a lot like this:
Designer: "Can we bring the spacing between the trace and the pad down to 3 mils?"
PCB fabricator: "We can if we don't need to lay down solder mask between the two."
Assembler: "You can't cover my test pad with solder mask!"
1. Revised system design that includes the negotiated design features
2. List of updates for the PCB & PCBA Design Spec
Step Three - Post manufacturing meeting
The first run of any new product has items that cannot be calculated or figured in on the CAD station. This is why we like to call this the "Learn by doing" step. After producing the first few lots of a new product, the manufacturers collect quality data and observations made while manufacturing the system. Then the three sit down again and discuss potential ways to improve the manufacturability and reliability of the product. A few of the potential improvement items are:
Controlled impedance stack-ups. After the board is produced to the designed stack-up, it can be micro-sectioned for thickness and TDR-tested for the actual electrical properties of the board. The engineer can compare the desired readings to the actual and review with the group and make modifications to the lay-up or line widths, as necessary.
The PCB manufacturer and assembler will bring in data showing the features of the board that were difficult to produce or caused a high yield loss. For example, there could be a low copper density area on the board that was found after lamination and which caused wrinkles in the foil. The PCB manufacturer will recommend filling this area with copper thieving that will even out the distribution and reduce the occurrence of wrinkling.
The assembler may see that there were issues with solder shorts between pads on the board and recommend modifying the solder mask coverage to dam the area and prevent the shorting.
1. Quality data from the manufacturers on the specific parts performance during manufacturing.
2. An updated design that is ready for production.
By now you can see the definite benefits of working both up- and downstream on new projects. In the long run, new products will get to market quicker and the process will build the relationships between the designer, fabricator and assembler.
David Barry is vice president of engineering at ATOMIC29. He has over 17 years of technology experience, with a background in system analysis and engineering. Most recently, he served as director of operations for Publicard Corp., where he designed a network deployment software system for duplicating hard disk drives. He previously worked for Tyco Corp. and Formosa Plastics.
© 2001 CMP Media LLC.
7/1/01, Issue # 1807, page 14.
Reproduction and distribution of material appearing in PCD and on the www.pcdmag.com Web site is forbidden without written permission from the editor.
Contact information for Reprints.
NOTE: The articles presented here contain only the text originally published in Printed Circuit Design magazine. Any accompanying graphics and illustrations have not been recreated here. You may view the article in its entirety in each printed issue of PCD.