Printed circuit board quality is strongly influenced by the design. At this stage the designer determines the production process and quality issues. Many small mistakes may be eliminated by introducing changes to the design. Hints applying to printed circuit board design are presented below.
Printed circuit board’s designer should not only take into consideration electrical quality but also production capacity of supplier. There are certain rules which should be followed in order to prepare a good project to be produced in our plant. Such rules can be found on our website; these are, inter alia:
- minimum distance between conductive parts,
- minimum path width,
- minimum holess diameters and rings sizes,
- minimum mask exposure,
- number of layers etc.
Every project has to be analyzed according to above rules. Fortunately, every deviation from these principles is easy to spot, since most modern systems for PCB design are equipped with checking and correction functions.
Due to the incorrect design, production problems may occur. It is worth to notice that such problems do not have to result from failing of complying with the rules mentioned above. These problems can also decrease PCB quality.
Copper surface and paths
One of the most common problem is incorrect copper distribution on outer layers. Efficiency of electrochemical processes of applying copper on PCB surface and into the holes is connected very strongly with the proper copper distribution on the PCB surface.
Printed circuit board surface with small number of elements (single insulated paths, holes) characterize with higher copper than other areas of the PCB with large number of elements or areas of copper.
Such solution results in the problem with maintaining holes diameter tolerance and correct soldermask applied on the edges of excessively thick paths in the areas with low number of elements. In order to improve copper distribution, additional copper surface is advised to be added in the area with small number of elements. Such non-functional copper area does not have any electrical function, but helps to obtain correct copper distribution in the electrochemical metallization process.
Figure 1. Not recommended solution, such situation should be avoided. Next: recommended solution – insulated paths and holes are protected with additional copper fill.
Another issue is the over-running minimum-width paths. Single insulated paths with the minimum allowable width cause digestive problems of printed circuit boards. Such paths are easy to be etched and exposed to mechanical damages and openings. It is recommended to reduce the length of paths with minimum width during the designing process. It means we run a 4-mil path in the heavily packed areas, but as soon as the density decreases, we increase the track width by 2-3 mills. An example is shown on Figure 2.
Figure 2. Figure 2. Not recommended, two bottom paths are exposed to etching and mechanical damage. Next: Recommended solution – paths with minimum width were expanded so both etching and mechanical damage are limited.
Teardrops next to pads
Quality issues of printed circuit boards are caused by the lack of ‘tear’ next to small pads (rings) very often. It happens that drilled hole is tangent to the edge of the pad. Such solution is allowed only if a hole is not tangent to the edge of the pad in the area of path and pad connection.
At this point the risk of gaping increases significantly. In order to protect against such problems, a special “tear” is added to the pad. It should overlap the path by not less than 5 mils. This rule is particularly important for small hole diameter (0,3 mm and lower) with minimum acceptable rings, where the probability of the defect of non-centric hole rises due to the insufficient rigidity of the drill.
Figure 3. Standard pad and the one with teardrop added.
Another reason for quality issues is free space between pads and paths (width of less than the acceptable minimum, e.g. 4 mils). After the exposure and development, the 4-mil (or less) photopolymer strip has limited adhesion. It often happens to detach and stick to the other area of the PCB. It results in shorts and opens depending on technology. This problem is presented on Figure 4. Figure 5 presents recommended solution.
Figure 4. Space between the bottom pad and path is too small.
Figure 5. Correct solution – correct distance between pad and path.
Another cause of errors are areas covered with soldermask of width < 3 mils. Such places also have reduced adhesion and tendency to flake (the same goes to photopolymer). It is noticeable especially on gold plated PCBs (damaging effects to the soldermask).
Such surface should be extended or removed from the project. Small residues of copper on the board also have a big impact in this case. PCB’s designer should pay particular attention not to leave unnecessary remnants of copper.
Copper remnants have very poor adhesion to the laminate and may cause short circuit when applying the mask. This problem is presented on figure 6. Also the large difference between the top and bottom surface of copper result in low quality of the PCB.
Such difference causes tension. This types of PCBs have a tendency to bend in heat treatment. It applies especially to the PCBs thinner than 1,5mm. In such cases it is advised to use additional copper fulfillment on the side with lower surface or copper grid on the side with higher copper surface.
Such solution relieves the tension and there are no PCBs’ deformations. Figure 7 presents copper grid instead of masses with the whole copper surface. While creating such grid, it is good to remember that the side of the empty square should be minimum 8 mils and the thickness of copper line no less than 10 mils. The last issue is creating the large surface without copper on the inner layers of PCBs.
Figure 6. Accidental part of copper.
<img alt="Using of the grid instead of mass with the full cooper surface." height="183" web="" uploads="" images="" 1638547e4f08bd3a979ea9c3ef390a82.jpg"="" style="display: block; margin-left: auto; margin-right: auto;" title="Rys. 7. " width="284">
Figure 7. Using of the grid instead of mass with the full cooper surface.
Figure 8. Not recommended solution – black area on the PCB is the low pressure area. Next to it, recommended solution – empty area has been filled with copper.
During the pressing process, such places create so called areas of low pressure. Such areas require large amount of resin to fill it utterly. If there is not enough resin, empty vesicles are formed (that resembles of delamination process). The solution is to add in non-functional copper surface (which is presented on figure 8). Compliance with this rule is particularly important for the projects with copper thickness ≥70μm.
Efficient use of laminate
PCB’s designers have also an impact on the final price of the circuit as far as the use of laminate is concerned. Solutions used by them may have great impact on the efficiency of the laminate use. Since PCBs are not produced as single pieces but in a production format (e.g. 460×610mm). PCBs producers advice clients to contact them to discuss the optimum panel size resulting in high efficiency of material usage.
It happens very often that adding one single PCB to the panel or removing it greatly reduces the wastage of laminate.
Issues presented above result from the mechanical and physiochemical feature of material and process used for PCBs production. The PCBs designed following the above rules will be a lot easier to produce, which means that we can produce it faster, better, cheaper and also avoiding the risks connected with the quality problems.