Have you ever gone to a buffet hungry and looking forward to digging in? You grab the plate and start down the food line, picking things as you go. Halfway through, your plate is stacked up with food, looking very similar to the Leaning Tower of Pisa. Then you get to the good stuff at the end of the buffet, but there’s no room on your plate. At this point, you probably felt much like that with the first part of looking at our footprint, but rest assured, although your plate is already full, the good stuff is still waiting for us.
I hope you’re not full, because I’ve saved the best for our second offering.
All PCB designs have two primary functions. The first is to allow components of all different sizes and shapes with their endless functions to connect to the PCB surface. The second is to connect those components with traces and vias. Last month, the first half of the buffet accomplished the first function with a discussion of copper pads, the solder paste applied to those pads, and the solder mask that sets up some boundaries and protection.
The second half of the buffet is where the good stuff is.
First, every component should have a legend, also known as a silkscreen (Figure 1), the top layer of the PCB design that holds the information for the components, which includes the reference designator and orientation or polarity markers. There’s also vital information such as board identification or details needed at specific points for tests or troubleshooting. As smaller designs are much more common, the purpose of the silkscreen has changed. Putting the components and information on some designs has become a real challenge.
Figure 1: Component silkscreen (legend).
As someone who started as an electronics technician, the silkscreen was vital for troubleshooting because the technician would find the defective component, replace it, and put the board back in service. Now the entire board is swapped out partially because of how cheap PCBs are. The primary function of the silkscreen is used during the assembly inspection process. Of course, visual inspection is accomplished automatically, and the silkscreen identifiers determine if it is correct.
Time for a heart-to-heart with your fabricator.
What drives your choice of text size depends on the method your fabricator intends to use. There are three basic methods of applying silkscreen:
- The manual screen method with line widths greater than seven mils (0.007"). A stencil is used to apply the ink, cured in an oven.
- The next method is liquid photoimaging (LPI), which can be down to the line width of four mils (0.004") using liquid photoimageable resist and exposed to UV light to cure. This is the most common method.
- The final and most expensive method is direct legend printing (DLP), which uses an inkjet printer with acrylic ink that uses the CAD data and is then cured using UV light as it is printed.
Basic Rules for Silkscreen
Identify the critical components' orientation
Integrated circuits identify Pin-1 because the component can easily rotate. Therefore, a Pin-1 marker is a must. It will save you time, money, and from calls from your assembler. When necessary, identify polarity markers on such components as capacitors and diodes.
Keep your clearance
As we all have experienced in the past two years, a phrase in everyone's lexicon is social distancing. The same is valid with your PCB and your silkscreen. So keep the distance; do not overrun the silkscreen depending on the method of applying it; all you may get back are large ink spots and "blobs" (an engineering technical term) on your PCB.
Do not apply silkscreen to copper
Assure that you do not place the silkscreen on the bare copper surfaces, although this should be a design rule in your ECAD software. Usually this is a check done by the fabrication house, but it is just good practice not to tempt fate. If it does slip through, it results in lousy solder joints.
The next item in our buffet (I didn’t forgt about that) is the assembly information (Figure 2). That provides the needed details for your assembly drawing and the mechanical verification, i.e., does your PCB fit in the enclosure with no interference, which might be important down the road?
Place the assembly information on an assigned mechanical layer.
Rant: Many times during the PCB process, either on purpose or by accident, the correct information given to the fabricator is lacking. The fabrication and assembly drawing is your instructional document to create your design. We provide the bare minimum. I have never experienced the situation of a fab or assembly house complaining they got too much information. The opposite is true, though.
On the assigned mechanical layer, you will have your component's 3D model (Figure 3). So, where do they come from? Well, your first source is the component manufacturer. Many component manufacturers are finally coming up to speed (not a moment too late) to provide the 3D models. Other sources include 3D Content Central and Grab CAD. These are phenomenal resources for a wide variety of component models.
That brings up a fascinating subject; even for the most commonly used components, there are varying heights for each of the components. For example, take a 0402 size chip resistor; according to Octopart.com, there are 32,312 results with 25 different heights that range from 250 µm to 12.7 mm. So, which 3D model do you use?
Before I answer that, keep in mind that to stay aligned with the IPC standards (Figure 4), there are three variations of the land patterns for each component.
- Density Level A: Maximum land/lead to hole relationship
- Density Level B: Nominal land/lead to hole relationship
- Density Level C: Least land/lead to hole relationship
The primary use of density is to accommodate a level of manufacturing producibility. Therefore, Level A (maximum) is the most design for manufacturing (DFM) friendly vs. Level C (least), which would be the densest and most challenging to manufacture.
Figure 4: Component density level.
Which height should we use with these three variations of the 0402 footprints? We cannot have all the different variations resulting in 75 different available footprints. Nope. Often, the heights are divided into three groups, and only the tallest for that group is used. For our 0402, the first group is from 250 µm to 360 µm, the second group is from 370 µm to 450 µm, and the final group is from 457.2 µm to 12.7 mm. So the three models used are 360 µm, 450 µm, and 12.7 mm.—the worst-case scenario, we would say, for each density condition. Each one handles the group of heights.
The final item in your footprint is the placement courtyard, which, as the name implies, is used for placing the component on the PCB. Since you use a standard grid size for the footprint, you can use that information to calculate the total area on the PCB, called the “density feasibility study.” According to IPC, the ratio between the component area and your PCB total area should not exceed 65%. I would refer you to one of my previous columns titled “Density Feasability Putting 10 Lbs in a 5-Lb Bag.”
Figure 5: Component footprint placement courtyard and size.
Putting It All Together
We have all the needed items to carry out our PCB design in the footprint. Components get mounted using the copper pads, solder paste, and mask; the assembly information is used for the Assy DWG with the 3D model verifying no interference or mechanical issues with the enclosure. The placement courtyard is available for placement on the PCB. If you run the density feasibility, you can verify that you aren't trying to push 10 pounds of stuff into a five-pound bag.
John Watson, CID, is a customer success manager at Altium.
Download The Printed Circuit Designer’s Guide to… Design for Manufacturing by David Marrakchi. You can also view other titles in our full I-007eBooks library.