Get Rid of Your Fab Drawing: IPC-2581 Already Has the Data

IPC-2581 can streamline PCB handoffs by keeping manufacturing requirements connected to intelligent design data.

A surprisingly large number of technical queries (TQs) generated by a manufacturing partner after PCB design handoff have nothing to do with the design itself. They concern the documentation accompanying the design.

In fact, some manufacturers report that documentation-related issues can account for as much as 50% of the TQs generated after handoff.

Consider how much engineering effort goes into verifying a PCB design: running design rule checks, checking signal integrity, reviewing the stackup, verifying impedance requirements and confirming the design is ready for manufacturing. Then additional metadata and manufacturing instructions are manually entered as text in a fabrication drawing, disconnected from the design objects to which they refer. Every additional representation of the same information creates another opportunity for inconsistency.

Traditional PCB manufacturing handoff packages require designers to create fabrication and assembly drawings. Although greater automation is available for generating these drawings today, they remain another representation of information that often already exists elsewhere in the design. Whenever the same information exists in two or three places, there is a possibility those sources will disagree. That is where many unnecessary TQs begin.

A dimension on the fabrication drawing may not match the actual board outline. The documented stackup may differ from the stackup data. A note may specify one copper weight while another document specifies something else. The number of holes listed in the documentation may not agree with the manufacturing data. The manufacturer then has to determine which information is correct.

Interestingly, when manufacturers find discrepancies between fabrication documentation and Gerber data, one response they sometimes receive from the design organization is, “Use the Gerber data.” In other words, ignore the documentation because the graphical manufacturing data is the master.

That raises a basic question: In the age of AI, why are we still spending engineering time creating documentation that may ultimately be ignored? Why not provide intelligent manufacturing data containing the information the manufacturing partner needs and eliminate as much duplicate documentation as possible? That is one of the less-discussed, but very practical, benefits of IPC-2581.

Where the discrepancies begin. A typical fabrication drawing contains a significant amount of information beyond the graphical representation of the PCB, including dimensions, tolerances, stackup references, material requirements, plating requirements, impedance information, fabrication instructions, test requirements and other manufacturing notes. All this information must remain synchronized with the actual design.

Manufacturers report discrepancies involving dimensions or tolerances that do not match the board outline, incorrect hole or via counts, differences between the documented and actual stackup, conflicting impedance or loss requirements, netlist differences, conflicting material or plating requirements, and fabrication notes that reference obsolete or incorrect documents.

In a traditional manufacturing package, drawings contain instructions while Gerber, drill, netlist and other files contain different portions of the manufacturing data. When these representations disagree, the manufacturer has little choice but to generate a TQ.

Someone at the design organization must then research the question, determine which information is correct, respond to the manufacturer and, in some cases, issue updated documentation. Multiply that process across several questions, boards and manufacturing partners, and a seemingly minor documentation problem can consume a significant amount of engineering time. More importantly, every TQ can delay manufacturing.

Netlist limitations. Netlist information in traditional manufacturing packages is commonly transferred using IPC-D-356 or IPC-D-356A. These formats have limitations and do not adequately represent certain aspects of design intent, including intentional shorts and intentional opens.

As a result, some manufacturers report that designer-supplied netlists cannot always be used in production exactly as received. Additional interpretation or processing may be required. Again, the design itself is not necessarily wrong. The manufacturing package simply does not completely communicate design intent.

Using IPC-2581 to reduce documentation. IPC-2581 has been in production use across the industry for approximately a decade. One capability introduced into the standard several revisions ago permits specifications and notes to be associated directly with the design and individual design objects. IPC-2581 provides this capability through the SPEC element.

A SPEC element may not sound particularly exciting, but it can eliminate a surprising amount of traditional documentation. Instead of placing manufacturing instructions only on a separate fabrication drawing, that information can become part of the intelligent PCB design data.

Companies using IPC-2581 can therefore reduce – and in some cases eliminate – traditional fabrication and assembly notes when transferring PCB data to manufacturing partners.

The SPEC element. An IPC-2581 SPEC element is created by the PCB design tool based on information entered during design. When the IPC-2581 file is generated, the information is included directly in the data file. Technically, SPEC is an XML element within the IPC-2581 file transferred to the manufacturing partner.

The important point, however, is not the XML structure. It is the manufacturing information the element can communicate.

A SPEC can be associated with the PCB itself or with specific objects within the design. Board-level fabrication information, for example, can identify the applicable IPC class, board type, material, copper weight, surface finish, plating requirements, panelization, panel orientation, markings and test requirements. These are the same types of instructions traditionally placed on a fabrication drawing. With IPC-2581, they can travel with the intelligent design data.

Making fabrication notes part of the design. Defining fabrication requirements through SPEC elements makes those requirements part of the design and includes them in the IPC-2581 manufacturing data. An IPC-2581 viewing or manufacturing tool can read the information directly from the file.

This eliminates the need to locate the correct drawing revision and manually correlate a note on that drawing with information contained in several other files. The information instead travels with the design, reducing one of the most common problems associated with document-based handoffs: ensuring everyone is working from the correct revision.

Associating specifications with design objects. SPEC information becomes even more useful when associated with individual design objects.

Consider the plating requirements for a connector. Instead of placing a generic note on the fabrication drawing and requiring the manufacturer to determine which feature it applies to, the specification can be associated directly with the appropriate object.

The same concept applies to controlled-impedance traces. Manufacturers need more than a general note stating that certain traces require impedance control. They need to know which traces require impedance control and the applicable requirements.

Associating SPEC information with the relevant design objects provides a more precise representation of design intent than a note placed separately on a drawing.

Including assembly instructions. The same approach applies to assembly requirements. Suppose a component requires a heat sink installed using a specific process. The assembly instructions may require application of a particular thermal epoxy before heat sink installation.

Rather than placing those instructions in an assembly drawing or separate manufacturing document, they can be associated with the appropriate component. The instruction and the object to which it applies then travel together as part of the intelligent manufacturing data.

Reducing references to separate documents. Fabrication notes frequently direct manufacturers to separate documents for information already available within the PCB design data. A typical note might instruct the manufacturer to refer to a stackup document for board thickness and impedance requirements. That approach introduces another document that must be included in the manufacturing package, located by the manufacturer, maintained at the correct revision and checked against the rest of the manufacturing data.

IPC-2581 can communicate stackup information as intelligent data. Creating a separate document simply to direct the manufacturer to information that can already reside in the manufacturing data adds another potential source of inconsistency. Reducing the number of separate representations of the same information reduces the opportunity for conflicts among those sources.

Communicating intentional shorts and opens. The same principle can be applied to electrical intent. For intentionally shorted or intentionally open nets, a SPEC element can be associated with the appropriate nets to communicate that condition to the manufacturing partner. Instead of discovering what appears to be an inconsistency and generating a TQ, the manufacturer receives information explaining the condition with the design. An intelligent manufacturing handoff should communicate more than the geometry that exists. It should also communicate the designer’s intent.

Reusing manufacturing specifications. Entering manufacturing specifications individually for every PCB could become time-consuming, but many requirements repeat across designs. Engineering organizations already maintain libraries for components, footprints, design rules and other reusable design information. The same approach can be applied to commonly used manufacturing specifications.

PCB design tools can store these specifications for reuse according to the requirements of a particular design. An organization might maintain approved specifications for different IPC classes, fabrication technologies, copper weights, surface finishes, materials, via structures, test requirements and assembly processes. Instead of recreating fabrication notes for every PCB, the designer can begin with an approved set of specifications and modify only the requirements unique to that design.

Standardized templates can also improve consistency among design teams and PCB projects, reducing variability before the manufacturing package is generated.

From drawings to intelligent data. The objective is not simply to eliminate a drawing. It is to eliminate duplicate, manually maintained representations of information when that information can instead be communicated as intelligent data.

Traditional PCB handoff practices developed when drawings were one of the primary means of communicating manufacturing intent. Modern PCB design systems contain considerably more information about the design, including board geometry, stackup, nets, vias, components, materials and constraints. IPC-2581 SPEC elements extend that information to manufacturing requirements that historically resided only in drawings.

A fabrication drawing may still be appropriate for certain company-specific or manufacturing requirements, and eliminating drawings entirely may not be practical for every organization or PCB. But drawings should not be generated simply because that has historically been the handoff process. The better question is what information the manufacturing partner actually requires and whether IPC-2581 can communicate it directly. In many cases, it can.

Fewer documents, fewer TQs. The primary benefit of incorporating fabrication and assembly information into IPC-2581 is not simply the time saved by eliminating a drawing. More important is reducing the number of independent sources of manufacturing information that must remain synchronized throughout the life of the design.

With IPC-2581, manufacturing notes and specifications can become part of the intelligent design data rather than being manually duplicated across separate documents. Specifications can be associated with the PCB or directly with the objects to which they apply. Stackup information can travel as stackup data, impedance requirements can be associated with the relevant design information, and intentional shorts and opens can be identified before they generate questions during manufacturing.

The result is fewer opportunities for conflicts among drawings, stackup documents, netlists and manufacturing files. It can also reduce documentation-related TQs, simplify revision control and limit the engineering time spent resolving avoidable questions after design release.

Reusable libraries and templates add another benefit by providing a consistent set of approved fabrication, assembly and test requirements across multiple designs.

IPC-2581 is sometimes described simply as a replacement for Gerber or other PCB manufacturing data exchange formats. That description understates its potential. The larger benefit is the transition from a collection of drawings and loosely connected files to an intelligent manufacturing handoff capable of communicating both the PCB design and its intent.

Before generating the fabrication drawing for the next PCB, consider how much of the information on that drawing already exists – or could exist – within the IPC-2581 data. The drawing may contain far less unique information than it appears.End of article content

Hemant Shah is an EDA veteran and chair of the IPC-2581 Consortium (ipc2581.com). Shah led the effort to create an industry-wide consortium of design and supply chain companies to get IPC-2581 – the standard for transferring PCB design data to manufacturing – adopted.

He spent 20 years at Cadence as product manager for various PCB design products. Shah also led the industry adoption of the IBIS-AMI algorithmic modeling standard. Prior to joining Cadence, Shah worked at Xynetix and Intergraph. He is passionate about developing and marketing leading-edge software products for PCB design.