Fabrication notes are one of the most cryptic and confusing parts of the PCB design process. In fact, many experienced designers are not completely sure about how or what to specify. Fabrication notes are made even more difficult to create because of fabricator inconsistencies and a lack of guidelines. Very little information seems to be available on the subject. However, before a designer can direct a manufacturer on how to proceed, he/she must ask a few questions and understand the manufacturing process.
These notes aren't made to restrict the fabricator, but to provide consistency and serve as a starting point for when it becomes necessary to tighten values. Taking the time to research and understand the processes, tolerances and reasoning saves the designer precious time down the road.
Documenting fabricators standards
A "starter list" of manufacturing specifications is shown in Figure 1. (An editable version of Figure 1 is available online at the author's Web site.) A list of manufacturers and some of their capabilities also is available at www.ipc.org.
Understanding the manufacturing process
The fabrication notes should follow the manufacturing process so the manufacturer may use it as a checklist for project completion. First, it is necessary to understand the process. Note: Most of the values are for "conventional" values. Contact your fabricator for their capabilities and tolerances.
Selecting the material - From the fabrication notes, the manufacturer determines how to manufacture the board. This information should be clear and detailed.
Specify the quality and the reliability of the board. (These specifications are primarily used with IPC standards) For example: The board shall be Class II, (quality) Type III (multi-layer).
Specify the core material type - quality and tolerance. (Check with IPC 4101 for materials.) The thickness tolerance for this material should be no more than +/-.002". The core material is a fiberglass dielectric* that is copper clad (see Figure 2). It is important not to specify the copper or the dielectric thickness at this point. A design may be composed of several combinations of core material separated by pre-impregnated fiberglass, as shown in Figure 3. *Dielectric is material that is placed between conductors that act as an insulator.
Specify the pre-preg material type, quality and tolerance. (Check with IPC 4101 for materials.) The tolerance for this material should be no more than +/-.001". "Pre-preg" is a fiberglass type material that is pre-impregnated with an adhesive used to adhere the core material and to provide an insulator between the copper layers. Pre-preg comes in sheets with a thickness of .002" each. The pre-preg (see Figure 4) is stacked to create the desired thickness; therefore the material tolerance is additive.
Do NOT hold the manufacturer to the core/pre-preg thickness tolerance unless the thickness is critical in cases such as controlled impedance boards. Core/pre-preg tolerance should be specified with the stack-up when the layer thickness is specified. (Available core/pre-preg materials will be discussed in a future article: "The Board Stack-up.") For example: Core material shall be Type GF glass cloth base, laminated, copper-clad material per IPC-4101. Pre-preg material shall be of GF type material per IPC-4101 (or other high quality materials).
The layer stack-up (see Figure 4) should clearly define each layer as to the type (core/pre-preg/Copper), thickness in inch/mm but not ounces (copper is .0014" per oz.), and show the overall board thickness including tolerance (+/-.010% conventional standard).
Unless layer thickness is critical, specify the dielectric tolerance +/-.005". This allows the manufacturer to choose from several different combinations of materials. This gives them a better selection of materials in an industry where fiberglass is becoming scarce and manufacturers are reducing the amount of different stocked materials. Do not include the mask and silkscreen in the overall thickness unless they are critical to the design. (Board stack-up and materials will be covered in a future article.) For example: Material stack-up, copper and dielectric thickness are shown in Figure X . Copper thickness tolerance shall be +/-.001". Dielectric material thickness between layers shall be +/-.005".
Imaging - The information from the Gerber files is photo transmitted onto an etch-resist film that is placed on copper clad material (see Figure 5).
At this point, the CAD/CAM operator will place some manufacturer information on the board. If necessary, specify locations and type for all manufacturing markings such as date code, manufacturer ID, etc.
The view of the data delivered to the manufacturer and how the image is to be transferred to the material (directly or indirectly). For example: All manufacturers' marking shall be located on the bottom side of board. Image Layer data is viewed from the topside through the board. Image must be transferred to a stable material or directly to the copper material.
Etching - The process where a chemical is applied and the copper, in unprotected areas are removed, leaving the intended circuit (see Figure 6).
Define trace width and the tolerance (.002" is normal & .001" is tight). Do not attempt to build in thickness for etch-back (see Figure 7). This is the manufacturer's job. A design that has oversized traces, to account for etch-back, will be limited to that technology because different manufacturers have different etch-back allowances. For example: Min trace width is .006" (+/-.001). Min conductor spacing is .006" (+/-.001"). Manufacturer shall adjust for manufacturing process and document all changes.
Pressing (multi-layers only) - This is the process where several copper-clad layers are aligned, adhesive insulate material is placed between the layers, and the stack of material is pressed under high pressure and heat, forming a solid board (see Figure 8).
Define the layer-to-layer registration. (in reference to layer 1). This provides a constant for all other layers to reference to (see Figure 9). For example: Layer-to-layer registration must be no more than .003" from layer 1.
During the pressing cycle, the material may expand. The outline may be routed correctly but the board can still be out of scale. Define the overall board scale tolerance. For example: "Board scale is not to exceed .001" per inch, .005" overall."
Look for Part 2 of "The Fabrication Drawing" in next month's issue.
Chris Robertson [www.robertsondne.com] is a senior designer with a major aerospace systems corporation. Send your comments and suggestions to email@example.com.
© 2001 CMP Media LLC.
7/1/01, Issue # 1807, page 40.
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.