Sample fabrication drawing notes.

In this post I shall provide a listing of sample fabrication drawing notes that may be used on any fabrication drawing for a pcb. Fabrication drawing notes typically specify materials and finished requirements in a text outline form. Critical requirements shall be specified in the note structure.

Notes:

  1. Fabricate PCB in accordance with IPC-6012, Class 2; per IPC-6011.

  2. Materials:

    1. Laminate and Prepreg (B-stage) to be in accordance with IPC-4101/21.

    2. Copper foil to be in accordance with IPC-MF-150. Unless otherwise specified, all copper weight for inner signal layers and inner plane layers to be 35um (1 oz.). For outer layers 53um (1.5 oz). Copper weight is to be considered “finished”.

  3. All holes shall be located within 0.2 (0.008”) Diameter of True Position. Layer to layer registration shall be within 0.125 (0.005”).

  4. Finish:

    1. All exposed conductive pattern areas not covered with solder mask or other plating shall be Hot Air Solder Leveled using eutectic Tin Lead Solder (Sn63/Pb37 ), per ANSI/J-STD-006 (HASL).

    2. Apply liquid photo imageable solder mask (color green) per IPC-SM-840, class H, to both sides of the board over bare copper. Via holes covered with solder mask do not need to be plugged. Only solder mask images that are the same size as the component pads may be enlarged, and shall not be enlarged beyond 0.08 (0.003”) per side or 0.15 (0.006”) overall. All other solder mask images shall not be enlarged.

    3. Silkscreen shall be white, permanent, organic, non-conductive ink. There shall be no silkscreen on any solderable component pad.

  5. Marking:

    1. Board part number and revision letter is rendered in etch on the bottom side of the board. Revision letter should be identical to this drawing.

    2. UL logo, manufacturer’s identification and date code letter shall be rendered in etch on the bottom side of the board approximately where shown.

  6. Test requirements:

    1. 100% net list electrical verification using customer supplied IPC-D-356 net list for opens and shorts.

  7. The supplier may add thieving to compensate for low copper density areas on this design. Thieving shall not be added to within 3.8mm (0.150”) minimum distance to any existing feature. There shall be no exposed thieving in any areas free of solder mask.

  8. Plate Edge Connector 0.8um (0.00003”) minimum gold thickness over 2.5um (0.0001”) minimum low stress nickel.

The sample above is acceptable for double sided pcbs and up to most six layer pcbs. Now we shall discuss variations of the notes for different types of designs. These variations shall take into account higher layer counts, industry sectors, RoHS and Lead Free assembly compliant materials.

Lets start with note 1: Fabricate PCB in accordance with IPC-6012, Class 2; per IPC-6011. This note is acceptable for commercial applications where equipment performance is desired. For medical, aerospace or military applications we should specify Class 3. Class 3 implies that the device must work on demand without exception. This generally implies a life or death situation. Failure is not acceptable. Reliability is critical. This also results in a higher cost to manufacture the pcb. Acceptance criteria is more difficult to comply which has an effect on manufacturing yields. The amount of testing and inspections performed increases. Extra material and labor costs are increased by the manufacturer.

For reference, the IPC is an industry trade organization. One of its many functions is to create relevant standards for use by the industry. IPC-6012 is one of the main specifications that they publish. Future posts on this blog shall explain referenced specifications in greater detail. Their home page is www.ipc.org

Note 2.1: Laminate and Prepreg (B-stage) to be in accordance with IPC-4101/21. The /21 refers to standard FR4 with a Tg range between 110°C and 150°C. Each slash number refers to a different data sheet within the IPC-4101 specification. Consideration should be given for the following designs…

  • Pcbs of 8 layers or higher the /21 should be changed to /24. The /24 refers to standard FR4 with a Tg range between 150°C and 200°C.

  • Pcbs that need to be Lead Free Assemby compliant the /21 should be changed to one of the following /99, /101, /121, /124, /126 or /129. Materials qualified to one of these slash sheets have been determined by the IPC to be lead free assembly compliant. These are typically phenolic or modified epoxy systems that have high Td values. One of the most popular lead free compliant laminate systems is 370HR manufatured by Isola. Their home page is www.isola-group.com This material has been qualified to the /99, /101 and /126 data sheets.

Note 2.2: The copper weights specified above can be modified as follows…

  • Large current carring devices and specify 70um (2 oz.) copper. As the copper increases the spacing between conductors must also increase.

  • Impedance controlled designs may require the inner layer signal copper to be dropped to 18um (0.5 oz) copper.

Note 4.1: All exposed conductive pattern areas not covered with solder mask or other plating shall be Hot Air Solder Leveled using eutectic Tin Lead Solder (SN63/PB37 ), per ANSI/J-STD-006 (HASL). The decision to select another final finish is typically done for two reasons. The first is the desire to get a flatter solderable surface. The second is to comply with RoHS which restrics the use of Lead in the finished product. Other finishes may be specified in the notes as follows…

  • Shall be coated with Organic Solder Preservative (OSP).

  • Shall be plated with Electroless Nickel Immersion Gold (ENIG) per IPC-4552. Some customers like to specify various thickness ranges that deviate from the specification. DON’T! Just reference the IPC-4552 specification and everything shall work out. I shall elaborate more about ENIG in future posts.

  • Shall be plated with Immersion Silver (IAg) per IPC-4553.

  • Shall be plated with Immersion Tin (ISn) per IPC-4554.

  • Lead Free hot air solder leveling is relatively new. There are currently a dozen different flavors of alternatives available with vastly different soldering characteristics. Great consideration should be given before selecting one of the leveling finishes. Common alternative lead free solders are SAC305 and SN100.

Note 4.2: Via holes covered with solder mask do not need to be plugged. This can be removed and a separate note adding via plugging may be added. There are different types of via plugging techniques employed yielding different results. The least amount of ink in the hole forming the plug can be as low as 25% filled and is refered to as capping. Complete hole filling between 85% to 100% filled is refered to as plugging.

When impedance controlled designs are required a special note should be added. The note should identify the specific line widths on specific layers as being controlled at a specific impedance range. For example…

All .005” lines on layers 1, 4, 5 and 6 shall be controlled impedance to 50 +/- 10% ohms.

It is important to identify impedance lines on the fabrication drawing. The pcb manufacturer shall verify that the design and the materials used shall meet the finished requirements. It is also a common practice to add specialty coupons to the process panel that shall allow the pcb manufacturer to verify the impedance using a Time Delayed Reflectometer (TDR) impedance tester.

Any critical charateristic important to the finished pcb may be specified in the note structure. The important thing to remember is to be direct and keep it simple. When in doubt, ask your pcb manufacturer to help formulate a note. Feel free to ask in this blog.

Tags: , , , ,

2 Responses to “Sample fabrication drawing notes.”

  1. Zubair Says:

    Can you suggest a sample fab note for Flex and Rigid Flex design

  2. David Duross Says:

    Flex and Rigid-flex use many of the same manufacturing operations as rigid printed circuit boards.

    The acceptance and performance specification changes from IPC-6012 to IPC-6013. Use type 1 for single layer flex, type 2 for double sided flex, type 3 for multilayer flex and type 4 for double sided / multilayer rigid-flex. Class 2 for commercial applications or class 3 for military, medical or aero-space applications.

    The material specification for the rigid portion of the rigid flex could be IPC-4101/24. Flexible clad material could be IPC-4202/11. The cover coat could be IPC-4203/1.

    EPEC Engineered Technologies has a brief and straight forward four page document. Page one describes the different flex types. Page four has a good example of the note structure for a flex or rigid-flex pcb. You can find it here.

    Another subtle difference applies to the solder mask. Solder mask used on traditional rigid board technology does not bend and flex. Over the flexible portion of the flex circuit an adhesive Kapton cover coat is applied. As an alternative to an adhesive Kapton cover coat you could specify a flexible solder mask.

    Another option to consider is ecco-bonding the flex to rigid interface of a rigid-flex pcb. The rigid portion at the interface has fracturing and exposed glass weave. Ecco-bond is a black epoxy material applied at the interface to cover up and encapsulate any potential non-conformance. Its also very expensive.

Leave a Reply