PCB Business Card Ruler With QR and NFC

That all changed when I discovered the "elegant PCB artwork ruler" and "RF & MW Elegant PCB ruler" designed by Makis Katsouris. I originally found them through ebay, but Makis' website, SV1AFN.com, details all aspects of the rulers along with some really top notch RF projects.

Taking inspiration from these elegant rulers along with the Sparkfun, Adafruit, Digi-Key and Nvidia rulers, I decided to morph a PCB ruler into a business card. I wanted to focus my business card design on footprints, common measurements and useful reference materials to help folks who are interested in making their own PCBs. Of course, I could fill the card with references to all the types of op-amp configurations, diode types, and trace current capacity calculations, but I wanted to make something that would put a physical size to common part package sizes instead. This way, the designer would have something tangible in front of them to gauge the actual size of a package on a board and give them a better idea of how much clearance a package would need in relation to other components on a PCB.

Tools:

• Soldering iron (at least 40w)
• Tiny conical tip (Weller ETH & TETS are a good example)
• Decent pair of tweezers
• Android phone with NFC capabilities
• Magnifying optic
• Side cutters

Materials:

• Tiny diameter solder (0.025 or smaller recommended)
• Solder Wick
• Solder Tip Tinner (optional)
• Isopropyl alcohol (any variety will do)
• Q-tip / Paper towel
• PCB Business card

Components:

• (1) NFC chip (TSSOP-8 package)
• (1) Green SMD LED 800mcd z-bend [optional]
• (1) Resistor 47ohm 0603 [optional]
• (1) Capacitor 220nf 0603 [optional]

Sometimes the best way to start a project is to check if someone else already did the same thing. Sure, I knew that it was unlikely that I would find a business card design to my exact tastes, but I wanted to at least check if something came close. Looking at other designs on the web gave me further motivation and validation that this was indeed a great idea.

I settled on this very useful and succinct business card made by Brian D. Carlton to use as a template. After all, I'm a KiCAD user and even if I decided to start over, the Edgecut dimensions should be the right size :D. I really liked the simplicity of Brian's heavily layout-based business card, so I took the same principle and applied it to my card. Cheers Brian on the great business card!

One of the first changes I made to the card was add more components. I really liked where Brian's business card was going but there was too much empty space for my tastes and I could use that space to fit in more footprints. I decided to keep a good chunk of the IC packages and transistors, but I expanded on the passive footprints, diodes and SOT packages. Here's an early iteration of my board. It's not pretty, but it's getting somewhere.

My goal was to squeeze the most out of a compact layout. I added a simple font size scale and trace width scale. I added common test pad sizes as a reference to test jig design or bed of nails testing. I added some fiducials for good practice and attached a 2.4ghz antenna, which is now even more common from the IOT craze. I didn't want to leave out common footprints from older equipment, so the TO-5 CAN10, DIP and crystal packages were added. I decided not to include hole sizing because wire strippers with included AWG sizes are pretty commonplace. Also, additional drilling adds to manufacturing time, and through-hole plating varies by pcb vendor, so it's best to skip it completely.

One of the biggest departures of my design is the included rulers. I designed each of the three rulers as a custom array of lines so I could mix 1/16 and 1/32 of an inch on one ruler, tenth of an inch and 5 hundredth (50 thousandths) on another and millimeters and half millimeters on another ruler. None of these types of rulers are available with the included kicad footprint library rulers. I didn't even know the KiCad library contained ruler footprints until I checked out Jan Böhmer's PCB ruler. A ruler is the last thing you'd expect in a footprint library!

The QR code was created by a qr code generator website and then converted over to a kicad mod file using the "Bitmap to Component Converter" built into Kicad. Make sure you use a high resolution image when using this tool and adjust the "Black / White threshold" slider to fine tune the "Black&white" picture preview. This picture preview is exactly how the kicad_mod file will look. I previously used the super useful Wayne & Layne img2mod Image Converter for Kicad web tool. This is a great little tool for converting images to kicad_mod files, but the one downside is that is creates huge kicad_mod files which bogs down Kicad. This is largely because it integrates the area of an image with tiny unconnected polygons instead of just creating large contiguous polygons like "Bitmap to Component Converter."

One thing to note, inverted QR codes are not always read by every barcode scanner application. I have found that lightening QR is one of the few barcode scanning apps on the android app store that works well with the inverted PCB bar code. It is a bit spammy with ads, which I'm not a fan of, but I have not found an opensource alternative yet. Apple devices with a qr code scanner built in seem to pick it up just fine.

A big time sink with projects like this is ironically, layout. But not in terms of connecting everything together. Anyone can throw a footprint somewhere on a copper layer, but if you are trying to make a legible reference card, equivalent spacing becomes paramount. Ideally, you don't want some footprint references to be harder to read than others and you certainly don't want silkscreen overlap, causing the user to think two references are one! Footprint overlap is also a big no-no.

The concept of scale is also extremely important. Sure, that trace width gauge looks great from being zoomed in at 1000x, but when rendered to actual size, it's far too small and no one can read it! These are the main issues when making a tiny reference card. I found that the included 3D viewer in KiCAD is pretty fantastic for getting a decently accurate representation of the board. The 3D viewer enables you to scale the pcb small enough to exactly match the size of a business card by enabling orthogonal projection. This is the render on my 30in 2560x1600 lcd and the actual business card side by side. Nearly spot on. Using the 3d renderer, an optic and a caliper (for referencing font size on other rulers), I was able to create a pretty legible PCB business card without needing to send away for boards multiple times. A true life-saver.

I really like the use of soldermask pullback to highlight titles on the Digi-Key 12in rulers which gives that nice contrast-y two-tone color scheme, so I adopted it on my design. Also, a big shout out to Digi-Key for creating a dedicated Digi-Key kicad library with footprints, part numbers and links to part datasheets and Digi-Key part pages. This is extremely helpful.

Traditionally, footprints are designed to aid in the bonding of components to the traces on a circuit board. You line up the component to the footprint on the board, add solder and bam you're good to go. A footprint file consists of copper landing pads, specified soldermask pull back around the pads and a courtyard to prevent a copper pour in a specific area. The copper pads are connected to a series of copper layer nets which connects different leads of a component to different parts of a circuit. The soldermask is the negative of the copper footprints and serves as a basic insulator while preventing unwanted solder bridging. If you are making something non-critical like a ruler or business card it's not that important if a the footprints are floating and are not part of a copper layer net, as the PCB will never be used as an actual circuit.

The same way footprint files can be used for standard components, footprint files can be used to create PCB artwork. With the combination of copper pull back zones, soldermask pull back zones and traditional silkscreen, a layout designer can really get creative, such as this astro themed front solder mask. If you want to get crafty with PCB making, combining the soldermask pullback technique with fancy copper pad coatings such as ENIG (electro nickel immersion gold), will really make your designs pop and push your pcb from just-any-old-pcb to artwork.

Using soldermask pull back techniques, a myriad of common component footprints, custom rulers and useful size gauges, I created my first successful revision of a PCB business card. Even though my fingers were quite numb from constantly using [ctrl]+[m], I somehow managed to fit in four variations of each chip package on a single side. I spent a while moving components about trying to find a good middle ground for the density of components. This revision offered the best balance of usability and legibility.

The original file made by Brian was composed in Kicad ~2 so the footprints look different than the most current Kicad Library. One really great little surprise with Kicad 5.0 was the additional 49 pin 0.4mm pitch BGA package footprint. Now my 49 pin ICs range from 0.8mm, 0.65mm and 0.4mm pin pitches!

To get started with this project and Kicad, it is best to get familiar with the five programs that makeup kicad: EEschema (schematic layout editor), symbol editor, PCBnew (layout editor), footprint editor and gerber viewer. PCBnew is where you will spend most of your time. The biggest time saver with using any software is watching demo videos and of course learning the shortcuts. Here's a list of the most invaluable KiCad shortcuts needed for this project:

Within PCBnew:

• B = fill
• Ctrl B = remove fill
• Ctrl M = move exactly
• Alt + 3 = show 3d render
• Tilda = highlight net --> makes everything darker. Hit again to remove
• Ctrl + Shift + M = measure
• View > Flip board view (no hotkey yet)
• Help > List hotkeys
• PgUp = Switch to top component layer (F.Cu)
• PgDn = Switch to back copper layer (B.Cu)

Within 3D Viewer:

• Z = Show board on side one
• Shift Z = Flip board
• Tab = Rotate

A good portion of this project involves the tedious use of the measure,
move tool, and switching layer tool, but your biggest friend is the included PCBnew footprint libraries. There are hundreds of SMT and through hole footprints available, from connectors to terminal blocks to even old school can oscillators. You can even view the footprint and 3d model of the footprint side by side before placement! How convenient is that!

Once you are satisfied with your Kicad project, go ahead and begin the export process. Go to File > Plot. Select gerbers in the top right under "plot format." Set the gerber output directory to a new folder. Select yes to "do you want to use a path relative to..." so the path works for other people who may want to download / modify your project if you chose to share your project.

Settings:

• uncheck "plot footprint values"
• check "plot footprint references"
• check "exclude pcb edge layer from other layers"
• check "exclude pads from silkscreen"
• uncheck "subtract soldermask from silkscreen"
• check "use protel filename extensions"Included Layers:
  • f.cu
  • b.cu
  • f.silks
  • b.silks
  • f.mask
  • b.mask
  • edge.cuts

Generate Drill Files

Drill files are used as coordinates for drilling and jig borer machines to make incisions into your PCB. Select "Generate Drill Files..." on the plot window. This will bring up another menu.

Settings:

• check PTH and NPTH in single file
• Drill map file format: PostScript
• Drill units: inches
• zeros format: decimal format

2 More Images

It's sound practice to double check everything before shipping out for production. A good place to start is from the outputs: the gerbers and drill files. Unzip the gerbers and drill file and open them with different gerber viewers. I used both the built-in KiCad "Gerber Viewer" along with the excellent GerbV gerber program. Simply load the gerbers into the programs and inspect. I like to load the drill file and edge cuts first, then add all the rest but order doesn't really matter.

Start by inspecting each layer one-by-one. Disable all the imported layers and enable the edge cuts, drill file and front soldermask. look to see how the drill holes and soldermask keepout line up. Do they look centered? if not, something is clearly wrong in your pcbnew project file and you'll need to go back and correct it. if all looks good, disable the front mask and toggle on the back mask. Do the drill holes line up? Toggle off the mask and toggle between the f.cu and b.cu layers, checking to see if drill holes and pads line up. The idea is to take advantage of contrast to point out any errors that you might have missed when creating the board as a stack inside pcbnew.

Another nifty trick is to compare all layers using file > print and print preview. Select the color option. This will create a multi-page preview of each layer printed one after another. This provides a nice contrast of layer vs white background to help you spot any errors or mistakes that you may have overlooked.

When I'm confident my gerbers resemble what I want, I like to "sit on it" and wait for a good solid 20-30min before sending them out. This way I have adequate time to mull over and accept the completed nature of my design in my head. I literally save everything, close down all my pcb software and do something completely different. Sometimes this belief that you are done clears up head space and reminds you of another idea you had for a minor revision or allows you to think of a completely new design. This is how my backlit salvagedcircuitry logo came to fruition. I was originally perfectly content with back illuminating the open source hardware gear logo. I sat on it for a bit, came back and added it to the second revision.

If you're submitting a ~40+ board order, it's a good idea to flag the PCB manufacturer to send an image of what the board looks like on their end. It seems that a lot of board houses use their own proprietary gerber tool or some mashup of a currently available gerber tool.

I had an issue with the included JLC online gerber viewer. It showed some circular traces intersecting themselves in random places throughout the board. That did not show up in either of my gerber programs. It would have been catastrophic if I received 150 boards with semicircular ruler traces. Try explaining curved ruler traces to someone!

With the gerber and drill files all zipped up, and the gerber files checked for consistency, you are now ready to ship out your boards to final production! Now comes the decision on board production costs. How much are you willing to pay? Where do you want your boards made? There are a myriad of PCB vendors available. A majority of the low cost vendors are located around shenzhen and various chinese providences, but there are also several great vendors in the USA and Germany that can output very high quality boards. Since these business cards are by no means complex or in need to critical tolerances, I chose to manufacture the boards at two inexpensive PCB vendors in China.

This image represents the user interface used by a majority of the inexpensive chinese board manufacturers. Almost all of these board houses suspiciously use the same near-identical interface for calculating cost per feature, which is rather strange.

Here's a breakdown of what all these features mean for someone just jumping into PCB design:

• MATERIAL: You want to choose Normal FR-4. FR4 is a Fiberglass based insulator pcb and is the most commonly used PCb material. Aluminum board is aluminum backed PCB which is useful for custom high-power led boards that will dissipate a lot of heat and need good thermal conductivity. Rogers board is an overarching term used for boards with a different insulating material than fiberglass. Usually a teflon based or other high tolerance material that is very useful for Radio Frequency applications. Rigid flex board is for flexible Pcbs commonly found in high density digital designs.
• FR4-TG: This is the thermal properties of the PCB selection. TG 130-140 is fine, you will not need to reflow this board as it is unpopulated.
• THICKNESS: Normal PCBs are usually 1.6mm thick. For business cards, you want something thin. The best business cards are usually 20+ point thickness, which is 20 thousandths of an inch thick. This is about 0.5mm thick. Most board houses have a sub 1mm thickness available. 0.6mm-0.8mm is a good trade off, and a lot of board houses won't charge extra for 0.8 or 0.6mm. 0.4mm is more expensive so avoid that.
• MIN TRACK SPACING: This is the minimum distance between traces on a board. Stick to 6mil track spacing at the minimum. Business cards need to be as inexpensive as possible, and this is not where you want to spend extra.
• MIN HOLE SIZE: stick with 0.3mm as smaller holes add cost.
• SOLDERMASK: This is the coating that fills in the space between copper traces and prevents shorting. This is the "color" of your board. Choose anything that is not matte. Matte colors are usually more expensive and I don't believe they turn out that amazing. Most pcbs produced have a glossy finish and having a matte one may look odd and not be as durable to repeated handling. Most importantly PAY ATTENTION TO YOUR BUILD TIME ESTIMATE! Some soldermask colors are only run on a few days of the week, so your build time will go up by a day or 2 while the boards are on hold.
• SILKSCREEN: This is the color of the text on the board.
• GOLD FINGERS: This is a process where the exposed pins on a board are hard plated with gold. This is expensive and only needed for RF designs and boards that will be repeatedly removed/inserted like board-edge PCIe computer cards.
• SURFACE FINISH: This is the type of finish that will be applied on top of the exposed copper pads. HASL is the traditional cheap Hot Air Solder Leveling plating that applies on top of a pad. Leaded is cheapest, lead free is a bit more, Gold is even more and the other options are astronomical. OSP sounds like one to avoid. Immersion gold, or Electro-less nickel immersion gold is what you want for business cards. This is where you need to break the piggy bank. Gold plating will make any PCB project look fabulous. Gold plating is used on a lot of fancier pcbs not because of how it looks or pad quality, but because how flat gold lays on a pad. It allows for superior part leveling and solder wicking/adhesion.
• VIA PROCESS: Tenting vias is perfectly fine.
• FINISHING COPPER: 1oz is plenty for a board that will never be used. When doing PCb runs for actual boards, check the copper allotment from your vendors. Sometimes cheap board houses do not actually give you a 2oz copper board when you pay for it and give you something slightly more than 1oz, which is frustrating.

I originally tried out the "single pieces" production option to get an idea for how my boards would look by the default method. They came out far better than I expected. I thought I would be getting smudged, uneven silkscreen, terribly mis-aligned soldermask, and have a crap finish. To my surprise, the boards came out quite good.

I spent $118 on 30 express production, express shipped business cards. I used Pcbway as the vendor for the blue business cards and they still managed to ship me my business cards in time (ahead of schedule) even though they were enduring an unexpected monsoon. That is frankly unbelievable. I still don't know how they did it.

The cards were unbelievably good. Look at how well the ruler marks line up. They are near identical to the Adafruit rulers. This photo doesn't do the rulers justice, as the lens used has a bit of barrel distortion. A truly rectilinear and well-corrected macro lens is needed to show how well they match up. They are spot on. I was completely blown away by the results and seriously wondered why more folks don't make PCB business cards. PCBs almost never come out this well on the first run.

At ~$3.93/card, it's understandable why this is not very commonplace. Business cards are usually made in advance by a corporate marketing department so I can't imagine they would bug an engineer to make promotional business cards for the entire company.

Besides this, traditional paper business cards are about 4-30 cents per card depending on quantity and quality. If I was not in a rush to get the PCB business cards before the 2018 OSHWA conference, I would have paid close to $2/card through PCBway, or half my original order. Regardless, this is still quite an expenditure for business cards.

My PCB layout business cards served me well and were a good conversation starter at conferences and events. As I came across more and more business card designs, especially those integrated NFC based business cards, I knew I was in for a redesign.

Loann Boudin's excellent PCB business card with NFC really pushed me toward Revision II as I was unaware of any single package NFC chips that could handle phone to coil handshakes, without the need of jtag reprogramming. I was blown away by how simple and quick it was to implement the tiny NFC chip in my design, program it with an andorid NFC app, and have the card up and running. I thought the off-the-shelf NFC tags were the only economical option. Special thanks to Eric Kuzmenko for sending me the instructables link and Loann for the excellent writeup.

This is my latest and greatest business card. It implements QR, NFC, the same three rulers, but a whole lot more packages - all while maintaining a legible silkscreen. I also added in even smaller packages, such as the 0.4mm pitch dsbga footprints as well as more footprint variations. It's powered by a tiny NXP NFC chip with power harvesting capabilities. The small tssop-8 package is still big enough to hand solder, which is a major plus. This chip handles all the NFC handshakes and can harvest enough power from a phone to power the chip, transmit a web address and blink an LED. The NXP chip even comes in a XQFN-8 package measuring 1.6x1.6x0.5mm high. Crazy! If I ever decided to switch over to a stencil and paste assembly process, that's my primary choice.

The NFC coil design implemented was based off the suggested ISO/IEC 14443-1 criteria for NFC coils. The major benefit of using a specific "class" coil is that the example coils are thoroughly tested and characterized, so you know they will work flawlessly within an NFC design. Here are some very inclusive antenna design guidelines found in application notes from three major semiconductor manufacturers. These have more information about the 6 coil classes (class 1-6) and the appropriate antenna sizing calculations.

• AN11276 from NXP
• SLOA217 from Texas Instruments
• AN2972 from ST Micro

Of the 6 defined coil classes, I selected a "class 4 coil" measuring 27x50mm, as it actually fit within my board space of 89x51mm. Unfortunately, the class 4 coil was a bit too rectangular for my layout design, so I modified it to be more square to fit in better with my business card. I compensated by adding another turn to the coil as well. Conveniently, the NXP Guide to designing antennas for the NTAG I2C plus includes the design files for class 4 and class 6 coils, so I didn't have to manually create a footprint in kicad. The coil design files turned out to be eagle .brd files, but the awesome Kicad developers included a kicad-to-eagle converter in Kicad 5.0+, so crisis averted. Thanks KiCad devs!

One unforseen problem I had with the coil is the curved corners. At this point in time, Kicad 5.0+ can not make or edit curved copper traces fluidly. To draw a curved line, you need to integrate dozens of points along a line into a curve-like shape, very similar in principle to how a gerber file read-out would look: a series of X,Y coordinates. Because I did not want to painfully redraw these curves manually, I added a square coil on the inside layer to avoid making a curved corner. I plan to update this design when curved trace capability is added to Kicad. If one is very invested in kicad of skilled in python, I believe it is possible to implement a curve drawing function using the python plugin module for kicad. I opted not to do this because it is a very minute issue that would have minimal impact on the coil, considering how many pads on the flip side are causing interference.

Here is the circuit diagram of my business card. It is incredibly simple and is based off the guidelines specified by NXP. I went with 0603 components so I can still easily hand solder them in place. A 220nF capacitor was chosen as NXP recommends a minimum of 200nf across VCC and GND. This value was doubled to 440nF to allow for the use of a higher current consumption LED. A green led was chosen because the forward voltage across a green led is ~2.1v. A 47ohm resistor in series with the LED was used. The resistance value was calculated based on R = (Vcc-Vled)/ Iled where Vcc is the supply voltage (tied to the Vout energy harvesting of the chip), Vled is the operating voltage of the led, and Iled is the current through the LED.

You may have noticed a change in style with this card. That curved contrast-y bit is a copper pour keepout region, around the NFC coil. In order to preserve the permittivity of that portion of the card, the internal copper layers had to be pulled back to reduce interference between the coil and neighboring copper structures. This ensures a magnetic flux between the coil in the phone and the coil in the business card.

Of course, there are still a bunch of smaller copper pads on the back, partially mitigating this design practice. Because this business card will be handed out with or without components soldered in place, leaving almost 1/3 of a card side blank was not an option. I chose a happy middle ground where a small amount of components were placed over the back side of the coil. It's not ideal, but all this card has to do it transmit a website and make an led blink. An imperfect antenna should work just fine.

Lastly, I added in a backlit salvagedcircuitry logo to add that extra bit of flare to the card. I always liked the look of backlit illuminated PCBs, even going back to the days of simple double layered 80386 motherboards. There is just something about the way fiberglass prepreg layers evenly diffuse light and make the pcb act as a single color diffuser.

My latest business card was designed in KiCad 5.0. The design files are free to download. If you haven't checked out KiCad, now's the time! Check out the amazing work of the KiCad devs on their ever-growing changelog. If you are having trouble using KiCad, comment on the KiCad Forum or try watching some recent online tutorials.

Kicad Files

Duplicate Kicad Files on GitHub

Special thanks to Brian D. Carlton for creating an awesome KiCad business card template. This project is an extension of Brian's original project and is appropriately licensed under a Creative Commons Attribution-NonCommercial-ShareAlike 4.0 International License.

Please note, when having PCB business cards made, use ENIG or PBfree coatings. Do not hand out HASL lead solder based business cards to people. Lead is not safe if ingested. Don't be that guy.

• Originally, in Kicad 4.06, I could not figure out how to duplicate a copper layer onto a soldermask layer. For the Kicad logo, I wanted the "Ki" text to be in the soldermask color, but the square logo outline to be exposed. The "Cad" portion be in the native soldermask color and outlined with soldermask pullback. My solution was to superimpose available kicad logo footprints that had portions of soldermask pullback on top of other variations that didn't have soldermask pull back. The correct solution was to simply open up the kicad footprint file, click a part of the logo and select which layer that geometry should be on. My results somehow came out great, but my original approach was completely absurd.
• Early on, While experimenting with custom kicad footprints, I spent a lot of time making designs in CAD or Inkscape, saving as a bitmap, then importing with the bitmap-to-component converter. I could have just exported my design to dxf and imported directly into a new footprint in Kicad instead.
• I should have spent far less time with Inkscape and just went straight to Illustrator. I would often fire up my CAD package to draw a vector shape, export it, then convert it into a bitmap just so I could avoid using Inkscape. This was before dxf import in Kicad 5.0. Inkscape is a great open source program, but it needs some serious UI/UX work to make it more user friendly.
• I Should have switched to Kicad 5.0 earlier. I waited about a month to switch and honestly, I could have been far more productive that month with 5.0.
• I did not notice the ST Micro eDesign Antenna simulator on their website when designing the NFC coil for my second PCB business card revision. The NFC coil I implemented on my first production run would have been a lot closer to NFC specification (2.35uH or 2.75uH).
• One of the challenges faced with this design was under estimating the amount of light fall off from two layers of soldermask. I originally implemented a 400mcd reverse mount led to illuminate my logo on the top side. This was a far cry from the light output actually needed. I soldered in a high powered led and a tiny ml-421 lithium battery as a quick fix.

• A redesign of the coil closer to 2.75uh or 2.35uh as well as a reshuffling of components on the back side of the coil should improve coil performance and allow for greater harvesting capabilities of the NFC chip. I may remove a layer of soldermask underneath the LED to improve performance as well.
• Optimize the NFC coil with a Vector Network Analyzer. This way I can appropriately measure the impact of the interfering nearby copper pads on the opposing size and maximize the coil performance.
• Leave alternative traces to an SMT coil cell battery footprint in case new coil still can't harness enough power to run a high power LED. May have to remove one side of the soldermask regardless, but that might make the card look a bit hazy around the LED footprint.
• Differential pairs and trace matching in the copper layer connected to a mid-sized FPGA footprint would look pretty sweet. Personal contact information on the silk screen would hover over a dense and busy design, but the soldermask would cover it for a very subdued effect. This image was borrowed from Tesla500.