Contact our corporate or local offices directly.
An exciting evolution in the design and development of electronic products is the ability to print the electronic circuit directly onto a substrate, such as a plastic molding that becomes a part of the product.
This surface-oriented implementation technique is referred to as Printed Electronics. While the term Printed Electronics is not a precise description of the technology, as printing is not the only technique used to create it, the term has broad industry acceptance and will be used on this page.
There are a number of approaches being developed to create printed electronics, including: 3D printing with conductive inks; stamping techniques that can create conductors as well as simple circuit elements, such as transistors; and laser deposition techniques that can build up conduction paths at very small scales, with ultra-high precision.
Printed electronics will become a pivotal technology, allowing the integration of electronics into new markets. Printed electronics allow an intimate connection between the circuit and the product. From a flexible sensor that attaches directly to the body, through to a multi-sensor, finger tip-shaped molding that allows a robotic hand to hold a soft plastic cup as liquid is poured into it, printed electronics will allow innovative new solutions to be developed across many market segments.
In terms of what the technology delivers, the game remains the same - electronic components are connected together via conductive pathways, forming an electronic circuit that performs a useful function. What differs is the approach used to build up the circuit.
The layer-oriented fabrication technology used to make a traditional PCB is a reductive process. Each conductive layer starts as a continuous sheet of conductive material, such as copper, which is then etched away, leaving only the copper that forms the required conductive pathways. It is also a multi-staged process, as the individual conductive layers are sandwiched together with alternating layers of insulation, and various drilling and post-plating processes applied.
Printed electronics is an additive process, the signal pathways are printed directly onto a substrate. If a subsequent signal pathway needs to cross an existing pathway, a small patch of insulation is printed directly in the required location. Acting like a tiny bridge, it allows the new signal pathway to be printed across the existing pathway, without connecting to it. As an example, if the design is using the DuPont InMold technology, the circuit is first printed onto a flat plastic substrate, which is then thermoformed and injection molded into the final product shape.
Using printed electronics, the humble rigid fiberglass printed circuit board substrate is no longer required. Instead the circuit is formed directly as a part of the product, the conductors ultimately following the shape and contours of the product's surface. As there is less material used and less waste, printed electronics will ultimately become a more cost effective approach than a traditional PCB, in many situations.
Apart from the substrate that the design is printed on, there are no physical layers in a printed electronics product - conductive pathways are printed directly onto the substrate. Where the design requires pathways to cross over each other a small patch of dielectric material is printed in that location, sufficiently expanded beyond the crossover to achieve the required level of isolation between the different signals.
The outputs required to drive the printing process are generated using a standard output format, such as Gerber.
The outputs will include a file for:
So how are these multiple printing passes defined in the PCB editor? In printed electronics, each printing pass requires an output file, so rather than thinking of it as a series of copper layers separated by dielectric layers, think of it as a set of printing passes, with each pass either being a conductive layer of ink, or a non-conductive layer of ink.
To create a printed electronics design, first create a new PCB using File » New » PCB from the main menus.
Configuring a new board as a printed electronics design is done in the Layer Stack Manager. Choose Design » Layer Stack Manager from the main menus to access the Layer Stack Manager. Use the drop-down then select Printed Electronics or select Tools » Features » Printed Electronics from the main menus.
When the Printed Electronics feature is enabled, the dielectric layer between the two copper layers disappears. Why? Because printed electronics require an output file for every layer, so dielectric layers are not used as they are not used to generate output files.
Instead, non-conductive layers are added. Dielectric shapes, referred to as patches, can be manually or automatically defined on these layers where ever signal paths need to cross each other on the conductive layers.
Right-click on a layer to insert a layer above or below, move a layer up or down, or delete a layer. Printed electronics do not use the Bottom Solder or Bottom Overlay; these have been removed.
Once the layers have been added, set the properties of the material for each layer.
The material used in both traditional PCB design and printed electronic design are selected in the Layer Stack Manager's Material Library.
When the Layer Stack Manager is open, use the Tools » Material Library command to open the Altium Material Library dialog.
The software needs to place a via to maintain the connectivity of the net during routing, and also to manage the connectivity when the routing is modified by pushing or dragging. Vias are not needed for layer-to-layer connectivity, the software assumes that overlapping tracks on different layers, are connected.
The route thickness can be built up if required, for example to implement a structure such as a printed antenna. This is achieved by placing multiple routes on top of one another, on different conductive layers.
Once the nets have been routed, the next step is to create the dielectric patches needed to separate any different-net cross overs.
Online DRC is not supported when the layer stack is configured as Printed Electronics because of the different logic used to define violation conditions; such as nets crossing on different layers being flagged as a short circuit. Once the routing is complete and the isolation patches have been defined, click the Run Design Rule Check button in the Design Rule Checker dialog (Tools » Design Rule Check) to perform a batch DRC.
Notes about net connectivity and Design Rule Checks:
In a Printed Electronics design, when different nets cross over on different layers, they are flagged as a short circuit. These cross-overs are isolated by placing a dielectric patch on a non-conductive layer.
Net to net clearances are tested on all layers, not just the same layer.
Layer transitions do not require a via, the net analyzer will recognize that the net is not broken.
Contact our corporate or local offices directly.