Section 14 – PCB Design: Silkscreen Marking

This is the fourteenth section in the back-to-school series for PCB Designers and those who may want to know more about it. 

Contents

Silkscreen Marking

A good silkscreen can really make or break the final product. On the assembly side, the rotation and location are added to the reference designator to inform the placement. From a traceability angle, the part number, revision are a start. The location for other identity labels like serial numbers and the bar codes are defined in the silkscreen with an outline The labels are subsequently referenced on the assembly drawing and/or bill of materials.

All of this usually goes on the primary side of the PCB along with your company logo and a description of the board function. Connectors and test points may have a secondary call-out of the net names in addition to the reference designator.

Larger components may have a system that shows the assembly and test group the pin designations beyond just pin-one. A BGA may have numbers and letters around the outside to indicate rows and columns. A quad-flat-pack or connector may have a little tick mark for every tenth row.

Safety information warns of high voltage or ESD sensitivity. The Reduction of Hazardous Substances (RoHS) compliance indicator looks like a little garbage can. If necessary the Underwriters Laboratories  UL seal of approval will make the main side of the board complete.

Vendor identifying information and safety ratings on board

Figure 1. Image Credit: Author - The vendor is responsible for certain information including the flammability rating and traceability.

Marking the Secondary Side - With or Without a Silkscreen

The secondary side is where we can expect to put the bare board part number and revision. If there are no components down there, the part number can be etched into a metal shape as a negative image or added as text if it is not a PCB with copper pour on the outer layers. The vendor adds their logo, date code and country of origin. This is usually applied in some way on the secondary side but can be inked onto the primary side.

The Quality Assurance people who inspect and/or test the board have a stamp they use when they “buy off” the board. They will put it anywhere unless you give them a special box for their stamps. Whatever is agreed to should be covered in a note on the fabrication drawing.

Board and card pairing in overall circuit with clarifying labels for tracking)

Figure 2. Image Credit: Author - A motherboard/daughter-card pairing with the typical stick-on labels for tracking purposes.

I try to do an adequate job on the silkscreen but I have to hand the crown over to one of my followers who added polygons around the functional circuits on the board with a label for each one. It was amazingly clean. I wish I could remember his name or at least have a screen-shot of the board.

There are not a lot of boards that I can recall where there was that much extra space but it does happen. The roomy boards like the one I’m using as illustrations in this chapter are typically internal-use test fixtures. There is usually an abundance of extra marking on boards used to bring-up and test integrated circuits in post silicon validation.

Proper Marking of the PCB

When you don’t have enough room for all of the above, there is a hierarchy of things that can be left off. Before you make the decision to start removing any marking, you should get buy-in from the stakeholders in assembly and test. It is generally agreed that the first thing you can remove is the component outline and all of that extra text and tick marks that describe the pin numbers beyond pin-one.

“When the rush-schedule is over, the shortcuts taken remain.”

As an aside, using a line between the pads of a passive component smaller than an 0603 package is not a great idea. The line will have at least some height which could act as a fulcrum to start the tombstoning process during reflow. Going down to 0201 size and smaller components, it would most likely work best without an attempt to draw an outline around the individual parts. You’re using those components because board real estate is at a premium.


After removing the component outlines, the next thing to sacrifice is the reference designators on those same components. The exception is for test points and connectors which should always have a reference designator on the board. If you can find a remote location where the marking for a dense field of parts can be offset, that can be a fall-back plan. If I was taking that approach, it would be done late in the design cycle. Otherwise, I would advocate for arranging the text earlier to help with placement review.

Circuit board marked with text for corresponding pin and components

Figure 3. Image Credit: Author -  Quick and dirty marking scheme.

In Figure 3, the important items within the shield have remote labels. The touch-points are labeled with reference designators and functional descriptions. Many components are not marked at all. When the rush-schedule is over, the shortcuts taken remain. Count on the last minute of the schedule to be hijacked by something out of the blue. Strive to do your part a full day before the last minute.

Polarity marks are a safety and sanity thing so they should stay no matter what. The IPC suggests a dash that protrudes from the component outline rather than a dot. The dash takes up less space but is part of a line which helps it adhere to the board. The same kind of tape test used to check solder mask adhesion is used on the silkscreen.

Buttons with descriptions on them on a circuit board

Figure 4. Image Credit: Author - Buttons deserve a description as well as connectors, LED’s and, of course, test points.

If you helpfully added the text “3.3V”, I’d put my inspector hat on and get out my adhesive tape then rub it into that period really well so I could rip it off and reject your board. Call it “3V3” and we can all go home happy. It will help the text stay put if it has a stroke width of at least 127 microns. Even better would be 178 micron stroke width.

That thick manufacturable line width could make the tiniest text look blurry. Things like the top of the R fill in but the overall shape of the character is defined well enough. The assembly, test, inspection and field service people can usually make it out under good lighting and magnification. And again, just like solder mask, we can sharpen the linework using laser jet technology. Putting decent marking on the PCB is your way of letting all of those people know that you care about them. You ought to since they’re depending on you.

Related Documents:

  • IPC-4781 - Qualification and Performance Specification of Permanent, Semi-Permanent and Temporary Legend and/or Marking Inks
  • IPC-TM-650 Test Method 2.4.1, Adhesion, Tape Testing, defines the procedure for using pressure sensitive tape to determine the adhesion quality of platings, marking inks or paints, and other materials used in conjunction with printed boards.

Next - Section 15 Creating a Document Package

About the Author

John Burkhert

John Burkhert Jr is a career PCB Designer experienced in Military, Telecom, Consumer Hardware and lately, the Automotive industry. Originally, an RF specialist -- compelled to flip the bit now and then to fill the need for high-speed digital design. John enjoys playing bass and racing bikes when he's not writing about or performing PCB layout. You can find John on LinkedIn.

Follow on Linkedin More Content by John Burkhert
Previous Section
Section 13 – PCB Design: Solder Mask
Section 13 – PCB Design: Solder Mask

Learn about solder mask, solder mask silvers, vias, and more

Next Section
Section 15 – PCB Design: Creating a Document Package
Section 15 – PCB Design: Creating a Document Package

Learn about documentation, assembly drawings, projecting views, and more