Key Components to a Quality PWB Fabrication Drawing

Reading time ( words)

Over the past 13 years, I can safely say I've seen quite a lot; maybe I haven’t seen them all, but I've seen a lot of them…fab drawings, that is. I've seen the good, the bad, and (unfortunately, too many) uglies in terms of what gets produced by engineering departments. Good fab drawings make life easy for everyone involved when producing rigid, rigid-flex, or flex circuits including, but not limited to: Purchasing, the quoting process, process engineering, and the CAM engineer.  

Uglies usually come out when fab drawings are handed down from one predecessor to another and no one has time to scrap and rebuild. However, time spent creating or rebuilding a quality fab drawing will save everyone more time and money than you thought possible. Remember, your fab drawing will likely be printed out and “travel” with your product from the CAM room to final inspection and packaging, being referenced nearly every step of the way--it is typically the leading document for guidance to a proper build for a PWB fabricator.

In this article, I would like to give a fabricator’s perspective on what details make for a quality fab drawing beyond giving a few dimensions with which to work. Some engineers might say they are obvious, but you would be surprised as to how often much-needed details are left out of many fab drawings received. My company has had engineers forget finished copper thickness, surface finish, overall thickness, soldermask color, silk screen color, and the like.

When items such as specification requirements, materials, tolerances, final finish, dimensions, hole sizes, hole schedules, impedance requirements, overall thickness, etc. are left for fabricator option, the door is left wide open for failure. Remember, these are custom parts, not off-the-shelf items like a box of cookies at the grocery store. Do not leave the recipe up for interpretation to the chef. 

When you want steak with mashed potatoes and steamed vegetables you have to state that. Order it how you want it cooked; otherwise the chef might bring you chicken and rice because all he thought was that you were hungry. To make your suppliers successful you must set them up for success at the beginning of the process.

Keep in mind fab drawings should be the ruling document for specifications with only the PO or a pre-agreed upon deviation or global spec super-seeding it. Even when the PO is the presiding document, details can get lost in transition which emphasises the need for an accurate fab drawing. When there are questions, they must be mitigated, which takes time. 

This is your time; the clock on delivery stops during the time it takes to resolve conflicts or engineering questions which often ends up pushing delivery back by days or even weeks. Engineers should not push the responsibility on the fabricator to discover mistakes rather than have a design team output an error-free fab drawing.

When you’re dealing with U.S.- or Asian-based factories, they will often times build strictly to the Gerber file unless otherwise noted to build off of the fab drawing. My company enforces strict rules that CAM engineers must do a thorough comparison of the fab drawing and Gerber file and this is where they catch a few discrepancies.

Following these general guidelines should significantly reduce those e-mails and/or conversations from purchasing asking you to answer CAM questions from an engineer at the factory level. A brief description of items that should be on successful fabrication drawing:

General Specs 1. Customer-supplied or IPC build, class, and qualification requirements to the latest Revision for the general specifications will suffice (i.e., IPC-600 or 6012 and Class References (I, II, III).2. Mechanical dimension specifications (inch or mm including a datum and all critical locations with tolerances including items such as counterbores, counter-sinks, mill-down, etc.).3. Tolerance (warp and twist, trace/space specifics).4. Drill chart (with sizes, plating info, tolerances, and quantities).5. Array specification if an array drawing is not included (ask CM/EMS company for help).

Fabrication 1. Any specific IPC fabrication requirements.2. Stack up requirements (prepreg thickness, etc, as needed).3. Finished thickness and tolerance.4. Any additional items such as thieving, removal of non-functional pads, tear-drops, etc.5. Impedance requirements with values, layers, type of impedance, and traces specified.

Material 1. Proper IPC specification or vendor-specified materials.2. Proper UL flame rating if required, default is 94V-0.3. General material type with equivalent options.4. Minimum Tg rating, if required.5. Minimum Td rating, if required.

At this point, it is your discretion to note something about IPC-4101. If you simply state that the material must meet a specific slash sheet of IPC-4101, all other requirements above are not needed. For instance, if you say: Material must meet IPC-4101/21, you do not need to specify material type, Tg, Td, etc. IPC-4101/21 specifies: NEMA FR-4, Tg 110°C minimum, as well as a bunch of other requirements like peel strength, moisture absorption, etc. Most material data sheets will state what slash numbers they conform to. For instance, the Isola 370HR data sheet says it conforms to IPC-4101, 21, 24, 26, 98, 99, 101, and 126.  6. Finished copper weights    a. Inner layer    b. Outer layer

A brief note about plating thicknesses, specifically old, obsolete requirements like “0.001 minimum plating in holes.” These requirements cause confusion and are often very hard to achieve. Imagine a PCB with 1 ounce of finished copper on the outer layers: You start with 1/2 ounce then plate up to 1. You are not going to add anywhere near 0.001” of copper in the holes. IPC-6012 requirements are for 0.0008” average and 0.0007” minimum (Class 2) and 0.001” average and 0.0008” minimum (Class 3). So by specifying 0.001” copper in the hole wall, you are not only specifying something that is difficult to achieve, but something that exceeds the requirement for Class 3 boards! 7. Markings on PCB    a. Manufacturer's UL logo    b. Date code placement/format    c. Serial number requirements as needed    d. RoHS markings    e. Color     f. Locations for items not in the data files

8. Finish    a. Surface Finish (specify type and thickness)    b. Soldermask type/color    c. Legend type (where applicable)/color.

9. Test Requirements    a. 100% net list     b. Voltage    c. Specification     d. Any additional requirements (Hi-Pot, dielectric withstanding voltage, etc.).

10. Packaging Requirements      a. Package labeling          i. PO number          ii. PN and revision          iii. Date code      b. Special QTYs per package      c. Any additional items (vacuum seal, ESD, desiccant, humidity indicator strips, etc.).


  • Get a part numbering system (see the don’ts below).
  • Update your material call-outs (no matter how well your old drawings held up back in the day, people don’t use some of those old material call-outs anymore).
  • Update your specifications. Do not ask the fabricator to build to an obsolete spec. For example, do not reference the obsolete Mil-P-13949 material spec when the current IPC-4101 spec is the correct reference.


  • Don’t name your products with the product name. Create a PN system that can easily roll with the changes if they product keeps going.
  • Please don’t mix document revs! In other words, don’t have your fab drawing as Rev B and your Gerbers as Rev A. Do you have any idea how confusing it gets when your fabricator has a purchase order with a Rev B and you’re Gerber files are still Rev A, but the only change was to an engineering note on the fab drawing?
  • Do not rev your boards based on a date! God made letters and numbers for that.

Of course, not even the perfect fab drawing will eliminate all questions. However, you will drastically reduce your future time and efforts if you make sure to detail the items referenced above--you'll also keep tighter control on the quality of your product. James Brown is co-owner and vice president of sales and marketing for PCB Solutions, LLC, a provider of high-quality PCB manufacturing and competitive solutions for the industry. Brown, with the company since its inception in 2002, specializes in customer relationships and developing customer service procedures that enhance customers' experience while focusing on growing organic business. His company has established domestic and offshore relationships with several high-quality fabricators to support prototyping, high-volume production, and basic to complex multilayer PCBs.


Copyright © 2017 I-Connect007. All rights reserved.