This article provides you with important information about how we interpret and process your project data for the Amazing Assembly of your PCB.
Please read it carefully before submitting your assembly order and check if your design goes in line with the rules stated below.
A conventional PCB contains many different components, which can be divided into two groups - components with and without polarity. The main difference when it comes to the assembly of a PCB: Non-polarized components (as most of the resistors and capacitors) can be soldered in either direction and still work the same, whereas polarized components (diodes, LEDs, electrolytic capacitors, ICs, …) can only be connected in one specific direction. Incorrectly soldered components will not only work as desired but can also get damaged and cause severe malfunctions of the whole board. That is why we must ensure that the final placement of a component is carried out exactly as intended.
In theory, the silkscreen provides the assembler with all necessary information to identify the position and orientation of each component of the board. However, the reality is different: Due to missing standardizations and the immense variety of CAD applications, component types, and footprints, the silkscreen is not a secure source of information. For example: Depending on the used application, the anode (+) of a capacitor can be marked with line or dot, but in the footprint of another application the same markers refer to the cathode (−) - even if it is the same component. Despite these inconsistencies, a few PCBs do not include a silkscreen layer at all.
A better (yet not perfect) way to get more robust information about the component’s orientation is to evaluate the uploaded project file, because most of the applications show a high consistency in using standardized pad names in their standard footprints.
Using KiCad as an example (see figure below): In most of the diode footprints pad “1” represents the side of the cathode and pad “2” the side of the anode. For polarized capacitors, this correlation is flipped – pad “2” marks the position of the cathode, pad “1” the anode. KiCad thereby follows the guidelines of the IPC-7351B, which defines (among others) the orientation and pin naming in CAD applications for common electronic components.
If you are not interested in the Amazing Assembly, you can skip the check-up completely and proceed with your order as usual - it is not necessary when just ordering pcb, stencil or parts!
After uploading your project file, you should see the gray polarity arrows / indicators in the Board Inspector. In case you have any polarized components on your board, the arrow marks:
the position of the cathode / negative pole for two-pin components
the position of the first pin (PIN “1”) for multiple-pin components (number of pins > 2)
Please control each component and the assigned orientation and/ or polarity! By submitting your order, you confirm the correctness of the assigned orientations!
If a component is marked with an arrow, but does not have any polarity (i.e., a regular capacitor), you can ignore the assignment as it is not relevant for the functionality of this component.
If the assignment of a component is missing or false, please check the corresponding footprint in your CAD application. Do the pad names / pad numbers and their assignment match with the relevant polarity rule (see table below) for your application? If not, try another footprint or modify it by renaming the pads according to the naming rules. Also make sure that the reference name(s) for diodes and capacitors correspond to the table.
Table: Correlation between pad name/pad numbering and polarity for supported CAD applications
|Two-pin||Multi-pin (no. of pins > 2)|
|Reference||"C#" (i.e. C5)||"D#" (i.e. D10)||(i.e. U1, R4 ...)|
|Positive pole (+)||Negative pole (−)||Anode (+)||Cathode (−)||First pin|
|KiCad, Altium||1||2||2||1||1, A1|
|EAGLE, Fusion||+||−, 2||A||C, 1||1, A1|