Assembly Polarity Rules

About this article

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 (βˆ’) - 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 β€œ1” represents the side of the cathode and pad β€œ2” the side of the anode. For polarized capacitors, this correlation is flipped – pad β€œ2” marks the position of the cathode, pad β€œ1” 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.

Check the assigned polarity of your 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 β€œ1”) 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

Β  Two-pin Β  Β  Multi-pin (no. of pins > 2)
Component Capacitors Β  Diodes Β  All
Reference "C#" (i.e. C5) Β  "D#" (i.e. D10) Β  (i.e. U1, R4 ...)
Β  Positive pole (+) Negative pole (βˆ’) Anode (+) Cathode (βˆ’) First pin
KiCad, Altium 1 2 2 1 1, A1
EAGLE, Fusion + βˆ’, 2 A C, 1 1, A1
Target3001! 1 2 1 2 1, A1

Hello I have a question about the placement of components. We are using EAGLE for our designs.

In the first image below, the polarized capacitor C51 has pin 1 as anode in the designs, only this resulted in that this component was placed backwards during assembly.

After contacting the Aisler support, it was suggested to switch the pins on these components. In the second image, the pin allocation of component C51 are switched and on the assembly page, the arrow now indicate pin 2 anode.

For me it seems that the assembly program indicates pin 2 for all (non-/polarized) capacitors and pin 1 for all other components?

Hi @Peter2 !

Welcome to the community!

To clarify our methodology again using EAGLE as an example:

We use the names of the pins to determine the polarity of a component.

  • For capacitors (e.g. C1) with two pads (and here it is irrelevant whether it is a capacitor with polarity) we interpret the pin with the name β€œ2” or β€œ-” as the negative pole

  • For diodes (e.g. D1) with two pads, we interpret the pin with the name β€œ1” or β€œC” as the cathode

  • For all other components with at least 3 pads, we mark pin 1 (pin with the name β€œ1” or β€œA1”) in the assembly view

It is important that the polarity displayed matches the actual polarity of the component as this configuration is taken into account (if necessary) during the final assembly.

As you have shown, you can change the polarity (and thus the final orientation of a component) by changing/switching the names of the pins. This is then interpreted according to our rules.

If I understand correctly, capacitors were soldered incorrectly in your assembly project. If the polarity of the assembled components does not match the polarity displayed in the project view, there may have been an error during assembly process itself. To find out exactly what went wrong with your project, a colleague will contact you directly.

Best Regards,