Friday, December 6, 2013

How to Import Graphics and RF Geometries Using DXF Files

How to Import Graphics and RF Geometries Using DXF Files



Often PCB designers need to bring in a company logo from a graphic design team, or an RF component designed in a 3D field simulation program. In both of these cases the associated 2D design tools can export the data in a universal "DXF" format. However, if the graphic was created in a vector image design tool it may often come in as an outline only, so you will need to use a few tricks to refill the geometry accurately in to the correct solid shapes. In this video, Applications Engineer Max Clemons shows the best approach for not only importing these design graphics but also performing the necessary "refilling" of the designed shape, and finishes off with a neat trick to be able to easily move and resize the various related geometries.


Thursday, December 5, 2013

Announcement: Altium Designer 14.1, Vault updates and TC2

Announcement: Altium Designer 14.1, Vault updates and TC2


Altium Designer 14.1, Vault, TC2, Private License Server, Altium Vault Server

On behalf of the Altium Development team, I’m excited to announce the release of Altium Designer 14.1, along with updates to the Altium Vault Server, Private License Server, and our newest product, Team Configuration Center (TC2).

Altium Designer 14.1

With this update we have paid particular attention to stability and performance issues. See the What’s New and Release Notes for a complete listing of all the fixes and enhancements.

To download this update you can use the new update system:

- Make sure you are signed-in and have chosen a license with valid subscription

- Goto DXP » Extensions and Updates, you should see the Update is available download link on the Updates page.

There are also updates to the Mixed Simulation and SIMetrix/SIMPLIS extensions.

Note: If you are using a Private Server license or Standalone license and you have renewed your Subscription since activation, you will be required to reactivate your license to obtain this and future updates.

If you are wanting to install a new build containing this update, the new Installer can be downloaded from the Download page in AltiumLive. A new Offline Installer is also available, please contact your local Altium office or Value Added Reseller.

Introducing Team Configuration Center (TC2)

By automatically configuring Altium Designer to use an organisation’s approved set of tool configurations and preferences, document templates and output job settings, design teams can save set-up time, avoid design rework and eliminate fabrication issues caused by generating incorrect or poorly formatted outputs.

TC2 centralizes and deploys Altium Designer settings and preferences, and ensures the entire design team are all working from a company-standard set of document templates and output job formats.


Tuesday, November 26, 2013

How to use Schematic CAD Drawings for Cable Assemblies: Part 1

Most electronic engineers work on products that require Printed Circuit Board designs to be interconnected by cable assemblies. As you might have already noticed, some dedicated tools that primarily focus on designing cable assemblies, while powerful, are quite expensive and beyond the scope of just creating a simple cable design. Most of the industries they are focusing on are automotive, HVAC, and aerospace firms. So you inquire yourself, what is the best alternative? The answer is simply in front of you, utilize your ECAD tool to create the cable assembly!

When working in Altium Designer, I acknowledge all I can do within the tool; I can create my schematic layouts and PCB layouts, I can manage libraries in many ways, and I can control document sources through Version Control. But there are often other questions that come to mind:

  • What if I wanted to create a design that will determine what the connections are going to be like through a cable?
  • How can I trace where signals are going, through a designed cable, in an automated way - and how can the design software help?
  • How can I quickly and effectively generate a detailed cable assembly drawing for the shop floor?

The answer is, use the Altium Designer schematic editor! You can generate very detailed cable drawings with the assistance of importing DXF/DWG files. For example, you can import mechanical drawings of connector heads or crimps that are will be needed for assembly. This way, the assembler can have the life-like drawing to refer to while building the cable. Below is a sample of such a cable drawing:

Figure 1. Example Cable Assembly Drawing.

As an example here (see Figure 1), we have a scaled length mechanical cable drawing, with two 1:1 sized connectors, one at each end. Below the mechanical drawing is the schematic representation of it using schematic symbols for the connectors, joined with wires. Within this schematic symbol diagram, you can see that net labels are linked to each connection. The bubbles with arrows (leader notes) represent a line item that you can refer to within the Bill of Materials. Once you have written your assembly notes, you can then send the ready drawing to the assembly house that makes your cables.

Through my own real-world experience, and in collaboration with other work friends, we came up with a robust and powerful methodology for cable design in Altium Designer schematics that takes care of these needs. So, throughout this blog series, I want to share with you:

  • How to generate the library parts as the building blocks of the cable assembly.
  • How to use the library parts to generate a complete and well drawn cable assembly.
  • How to prep and finalize the cable drawing to create your labels and generate outputs to hand-off to the manufacturer.

The first step is how can I get my parts placed as shown in the diagram? The simple answer is to create a multi-part library. What the library will encompass is the cables, connector heads, crimps, and any other mechanical drawing along with the schematic symbol. This will be further discussed in my next installment (part 2) of the Cable Assembly Blog Series.


Thursday, November 7, 2013

Announcement: New Libraries for AMS, ISSI SRAM & STM32

New Libraries

The Altium Content Team is pleased to announce the release of several new board-level libraries for vendors including AMS, ISSI and STMicroelectronics. From AMS it’s a mixed selection of parts covering the lion’s share of their catalog, ISSI is all about SRAM, and we’ve finally updated the STM32 families including the addition of STM32 F3.

We’ve also just shared our first batch of components developed directly as customer requests! These cover several different manufacturer parts and were created in response to feedback received via the content request form. This is the first of 3 releases that should see us deliver 99% of the individual components that have been requested so far.

More than 10,000 new components have been released! Here’s the breakdown of what’s included:

Audio (40) Data Converters (76) Interfaces (28) Light Sensors (112)

Lighting Management (91) Magnetic Position Sensors (45) Piezo Motor Drivers (3)

Power Converters (1) Power Management (260) RF Products (18)

STM32 F3 (37) STM32 F4 (135) STM32 F0 (53) STM32 F1 (244)

STM32 F2 (94) STM32 L1 (113) STM32W (20)


Synchronous SRAM Pipeline (875) Synchronous SRAM Flow-Through (689)

Synchronous SRAM No-Wait (ZBT) (1246) Synchronous SRAM Automotive (614)

Asynchronous SRAM 5V High-Speed (100) Asynchronous SRAM 5V Low Power (42)

Asynchronous SRAM Automotive (248) Asynchronous SRAM High Speed Low Power (414)

Asynchronous SRAM Lower Power (204) CellularRAM/Pseudo SRAM (34)


Content Requests

The first release of requested content includes more than 600 components covering dozens of individual requests. Highlights include:

Please note these requested components are only available in the Altium Content Vault.

If the parts you requested aren’t among these, the second round of requests will be released early next week, with a third catch up release the week after. Beyond this we hope to keep the turnaround times short (depending on demand). Please also note this is still only a trial, so we won’t be able to guarantee delivery within a certain timeframe.

As usual, all new parts mentioned above are available from the Altium Content Vault and (excluding content requests) as Design Content libraries available here. You can also place components directly from within Altium Designer using the Vault Explorer – where you will also find live supplier links and pricing information from suppliers such as Digi-Key, Farnell/Newark, Mouser and others – connect to the Altium Content Vault to explore further.


Wednesday, October 30, 2013

Creating an Embedded Side-View LED

Practical steps for creating embedded components with side-emitting LEDs


The Bluetooth Sentinel design, included with Altium Designer 14’s installation, gives a good introduction to some of the new rigid-flex tools available. I was asked to modifying this design to incorporate a different style of flexible region, but the repurposed board was left without room to place LEDs around its perimeter. Finding a way to add the LEDs back in posed an interesting challenge, and gave the perfect opportunity to try out some of the new tools.

One of the cool new features added for AD14 is the ability to embed components within the board. This can be done for a number of reasons, including cutting down on space in very dense designs, and shortening return lengths in high speed applications. For the modified Bluetooth Sentinel design, an alternative was needed for the LEDs, and embedding Side-View LEDs maintained the original functionality of the design, without having to modify it too much.



A thin package like the 48-213 SMD LED to the left was ideal for embedding, but really, the choice was only limited by the amount of vertical space available in the board. Creating this footprint was fairly straightforward, with only a couple minor additions to take advantage of the new features.

1. Footprint information and package dimensions were both available in the datasheet. When creating a footprint, one of the fastest ways to achieve a good end result is to set an appropriate Reference Point and Grid spacing. From there, it’s simply a matter of placing Pads, 3D Bodies, and any additional Mechanical information required.

2. Extruded bodies worked fine for most parts of the LED, the lens object being the lone exception. While the extruded bodies are surprisingly robust, and work well for polygonal shapes, the arced corners of the lens were more feasible to create externally and bring in as a STEP model.

3. Preparing a component to be embedded starts from the footprint itself. A Cavity - simply a Solid Region configured as shown - must be placed in the Library. Its height, as defined from the Properties, should be just large enough to allow for the component body. The LED package was 0.3mm, so the Cavity was created with a height of 0.35mm. This, of course, will ultimately depend on your specific Layer Stack and overall design intent.

4. It’s important to note that Cavities can be placed within any footprint, whether or not it will ever be embedded. When the component is placed on an inner layer, the Cavity will carve out a section of the core material, but on an outer layer, it won’t affect the design in any way. Placing one of the newly-created LEDs on an inner layer showed how cool this looks in action.

5. Technically, a Cavity alters the Layer Stack in that particular area, and it’s crucial that this information is conveyed through fabrication notes. The Layer Stack Diagram that can be automatically generated and placed already takes this into account. In this design, there was no question where the Cavities were added, or what layers from the stackup were included in those areas.

6. Assembly must also be considered, since embedded components are placed before those on the outside of the board. It’s a good idea to create a separate pick and place report, as well as an extra assembly drawing printout, for any inner layers embedded with components.

I’ve included the footprint and completed design for reference, but this is certainly not the limit of how embedded components can be used. Just an interesting way to solve this problem!


Wednesday, October 23, 2013

Development of a Methodology to Determine Risk of Counterfeit Use, Part 1

Development of a Methodology to Determine Risk of Counterfeit Use, Part 1

Counterfeit components have become a multi-million dollar, yet undesirable, part of the electronics industry. The profitability of the counterfeit industry rests in large part on its ability to recognize supply constraints and quickly respond, effectively taking advantage of a complex and vulnerable supply chain. Factors such as product obsolescence, long life cycles, economic downturn and recovery, local disruptions in manufacturing due to natural disasters, and lack of proper IP legislation all represent opportunities for the counterfeit component industry to flourish. Electronic counterfeits affect every segment of the market, including consumer goods, networking and communications, medical, automotive, and aerospace and defense. In manufacturing, the use of undetected counterfeits can lead to increased scrap rates, early field failures, and increased rework rates; while this presents a major problem impacting profitability, the use of counterfeit components in high reliability applications can have far more serious consequences with severe or lethal outcomes.

The independent distributor level has typically been seen as the weak link in the supply chain where counterfeits are most likely to be introduced. With the emergence of new legislation and through the efforts of different industry entities, new standards and guidelines are now available for suppliers to establish and maintain product traceability and to establish receiving inspection and detection protocols. There is no substitute for a healthy supply chain, and distributors play an essential role in the dynamics of the system. At the same time, there is an increased awareness of the need for proper management of electronic waste. Regardless of the nature of the counterfeits, whether cloned, skimmed, or re-branded, counterfeits are dangerous and too expensive to be ignored.

The work presented here by the iNEMI Counterfeit Components Project takes a comprehensive view of the problem by surveying the possible points of entry in the supply chain and assessing the impact of counterfeit components on the industry at various points of use. We then propose a risk assessment calculator that can be used to quantify the risks of procuring counterfeit parts. This calculator is aimed at all segments of the supply chain and will be of interest to component manufacturers, product designers, distributors, loss estimators, industry groups and end users.

Read the full article here.


Tuesday, October 22, 2013

Announcement: Techdocs - a new era for Altium’s technical documentation

In conjunction with the release of Altium Designer 14, Altium is pleased to herald the arrival of a new home for its technical documentation

This represents a significant milestone for Altium and kicks off the start of a campaign to ultimately get our documentation 'house' in order - and then some! It reflects our strong commitment to a singular overriding quest, and that is to provide high-quality, highly-relevant and accessible documentation to assist our customers optimize their use of our design solutions.

As a humble, and battle-hardened author of many of Altium's technical documents over the years, I feel empowered by the possibilities that this new documentation platform promises. Not only for myself and my fellow authors but, more importantly, what it can deliver for you as our readers.

So join me as I take you through what can only be regarded as the beginning of a new era for Altium's technical documentation. Through this blog I hope to explain what it is about this new site and direction that has us excited, and along the way I'll provide you with a little insider's insight as to where we are, and where we are headed.

Not a 'Wiki'

Before you roll your eyes and run for the hills, I can't stress this point enough. I know how the very name 'Wiki' has drawn exasperated gasps of frustration from our readership over the years. Imagine my reaction when I left the office at 11pm one day producing PDF-based documentation, and the next day the Wiki was the 'new world'!

A Wiki, by definition, is the culmination of efforts across a many and varied base of contributors, about a neverending variety of topics. Altium's documentation on the other hand, is a finite set of topics that, if we're being realistic, can, and should, be written and delivered by members of the Altium Team. It is an unrealistic expectation to place that burden on our users.

With that, albeit late realization clearly in mind, the paradigm for documentation became one of delivering a premium content-managed system, rather than a documentation space driven by the Altium user community.

And we already had the platform to do this in place, having relaunched the Altium website earlier, and built on the open-source Drupal Content Management System.

Unified Delivery of Documentation

In the past, a barrier to getting documentation has been, well, 'getting at' that documentation. This was hampered by the silo'd approach to the documentation, with some Wiki articles here, some PDFs there, and some older-style WinHelp and HTML Help files thrown in to confuse the mix. Our divergent documentation completely flew in the face of our unified design software!

The techdocs site provides a single, cohesive environment from which to source all of the documentation - from the highest-level conceptual document regarding some new-release feature, to the lowest-level resource document explaining what a dialog control does, or how a command is used.

What's more, by utilising the Drupal platform, we have been able to fully integrate the documentation with the AltiumLive community. As a general reader, there is no signing in required. But as a contributor, this means you no longer have to juggle a separate login. Simply sign-in once to AltiumLive with your usual credentials.

The First Step...

Having started with the company back in the days of 99 SE, I still have recollection of the size of the documentation available back then. A mere drop in what was to become a veritable ocean of words! Quite a double-edged sword in reality - the more that is written, the more that has to be maintained. And we were under no illusion as to the gargantuan task that lay before us.

But every journey starts with that first step. And I can proudly attest to the determination and rejuvenated outlook the merry band of authors have brought to the task. Concentrating primarily on resource reference material for the core technologies - namely in the Schematic and PCB arenas - I can share the following statistics of just what has been addressed in this initial site launch:

·         394 dialogs.

·         1541 commands

·         52 preferences pages

·         57 objects

·         13 panels

·         28 design rules

Not to mention a variety of 'hot-off-the-press' articles detailing the many new features available in the Altium Designer 14 release!

Browser-based Dialog Help

Yes you read that correctly! We've steered the documentation away from reliance on out-dated help methodologies and technologies, favoring delivery of all documentation through the single, cohesive Techdocs site. In terms of dialog-level help, no longer do you need to click, click, and click again to see help for options in a piecemeal fashion. Now, simply press F1 with the dialog open and get a page of information on that dialog in its entirety – being able to see, at-a-glance, what each option and control does. Presenting information for a dialog on a browser page delivers numerous benefits, above and beyond that of its previous WinHelp-based incarnation, including:

  • Ability to elaborate on the detail of a control, with additional note, information and tip highlight boxes.
  • Ability to keep the information visible while clicking elsewhere in the dialog.

·         Ability to add cross-linking to other pertinent areas within not only the technical documentation, but the wider AltiumLive community.

  • Ability to maintain the documentation for a dialog in a far more streamlined and expedited manner – making updates without having to compile installable files.

This initial release sees a myriad of resources supported by this reinvigorated approach to F1 help functionality in Altium Designer. And while you will undoubtedly run into resources that don't pop a specific page, rest assured coverage will continue to grow!

Ease of Browsing

While accessing the resource material directly from the software is one means of entry, it is by no means the only method. For those who like to browse through the documentation using a nav tree and search facility, we have you covered.

For a start, you will notice that content has been separated into specific and specialized content areas. This practical grouping of pages offers a more logical browsing experience and facilitates quickly finding the information you need.

And the platform's native search facility also benefits from this partitioned approach, allowing you to either pinpoint documentation from across all spaces, or only that residing in the space at hand.

The Road Ahead

On any journey, it is difficult to know how long each stage of that journey will take, what obstacles may lay on the path, or indeed what might be encountered around the next corner. But armed with a fresh and powerful content management platform, dedicated support from developers who are Drupal Masters, and a growing team of documentation authors, we have already started to formulate a decisive plan of attack, in a campaign that will realistically span a number of releases to the software. The following are just some highlights of forthcoming attractions to whet your appetite (in no particular order, of course).

Offline Documentation

By using an open-source platform for our technical documentation, we are well placed to deploy localized documentation repositories without the burden of paying licensing fees for each deployed instance. In essence, it will provide you with the option of having offline documentation that doesn't require an internet connection. And with the ability to reconnect to the techdocs 'mother ship', in order to synchronize your offline repository with the AltiumLive-based 'master'.Content Quality

While this initial release has addressed a sizeable portion of the resource reference material, it is just the tip of the proverbial iceberg. A large part of this will be to address the higher-level content in the Altium Designer space of the site. This features some 700+ pages of material which, in some cases, has exceeded its useful shelf life!

Getting this updated at the same time as providing additional new feature content is paramount and will go a long way to earning back some credibility with you, our users.

Reference Material

Having delivered an impressive array of resource material in this initial launch, we will of course be carrying that momentum forward. Addressing the remainder of resources for the core technologies, followed by the servers related to ancillary technologies thereafter. And let's not forget the plethora of detailed references in need of an overhaul too!

Advanced Semantic Search

While the documentation can be searched, the current search is, at the end of the day, very basic in its nature. To bring credible results to our users, we need to take this basic search and turbo-charge it. To use tagging and indexing to empower the search facility, allowing advanced searching not just of the technical documents themselves, but of all other services within the AltiumLive community, and the wider Altium website as a whole.

Productivity Boosters

By introducing features such as annotation and sharing, you will be able to create your ideal documentation 'set' and share it among your team. Just think of the ability to mark a page of the documentation with some well-honed personal remarks, and then share those with others - clip notes on a whole new level!

Language Support

Many people have asked me over the years why support for different languages has never appeared to 'take off'. And this is a very good question. Various spaces for a range of different languages have been available, but their content has never really mimicked that of the English content space. But again, that has more to do with the authoring tool available than the dedication of the authors in those spaces. But now, with Drupal as our platform, we have the ability to re-energize this whole area.

For us, supporting multiple languages across our technical documentation is an important part of our global operational reach, and one which we very much intend to deliver upon moving forward.


Monday, October 21, 2013

Announcement: Altium Designer 14

Announcement: Altium Designer 14


This latest release is definitely one of the biggest PCB releases that we’ve made for a very long time and it’s very gratifying to deliver such concrete evidence of our renewed focus on our core technologies and customer value. With a number of the added features coming directly from customer requests, it affirms our ongoing intentions to support you with the technologies you need today and into the future.

The key highlights of this release include:

·  Support for Flex and Rigid-Flex Design

·  Enhanced Layer Stack Management

·  Support for Embedded Components

·  Differential Pair Routing Improvements

·  Via Stitching within a User-Defined Area

·  AutoCAD Importer/Exporter Enhancements

·  CadSoft EAGLE Importer

·  Ibis Model Implementation Editor

·  Preferences-based Control over Vendor Tool Usage

·  Supplier Support for TME

·  Support for Xilinx Vivado Toolchain

·  New Installation System

·  Browser-based F1 Resource Documentation

See the What's New documentation area and our website for more information about the specifics of the release.

Accessing Altium Designer 14

All customers with valid Altium Designer subscription will be receiving an email shortly, but if you can’t wait for that and want to install now;

1. Goto AltiumLive to download the new installer

2. Download, Install and Run Altium Designer 14

3. Locate and use your existing Altium Designer license.

Note: If you are using a Private Server license or Standalone license and you have renewed your Subscription since activation, you will need to reactivate your license to use Altium Designer 14.

Friday, October 18, 2013

Altium Designer 14 - Coming Soon

Hi All

I'm excited to share with you the imminent release of Altium Designer 14. We have updated our website today in preparation for this event.  We are in the final stages of the release process and you will be notified when the software is available for download.

Thursday, October 17, 2013

Announcement: New Xilinx Series-7 & Linear Technology Board-Level Components

The Altium Content Team has released new updates to the Vault and Content Store.

We're happy to announce the addition of Xilinx Series-7 FPGA board-level libraries including Artix-7, Kintex-7 and Virtex-7 - all available now. Also released are board-level components for Zynq-7000 devices. To view the latest from Xilinx in the Content Store click here.

In Linear Technology, Comparators join Op Amps with 630 new library parts added to the collection - covering all high speed and micropower comparators from Linear. Linear Technology Comparators

Thursday, October 3, 2013

Altium Designer 14


We’re working hard on our upcoming major product releases. Why not join us each day to see what new and exciting things we’re working to bring to the help you create your next generation electronic design.

23 September 2013

Ruminating Rigid Flex - Part 4

In this blog post, I want to show a handful of important rules to follow when routing copper for flex and rigid-flex circuits, that not only increase the fabrication yield but also the reliability and lifespan of the flex circuit.

Read more

18 September 2013

Ruminating Rigid Flex - Part 3

In this blog, I discuss a few of the documentation requirements needed to get a flex or rigid-flex circuit board fabricated. Along with that, there are a few flex-circuit related issues to watch out for.

Read more


16 August 2013

Ruminating Rigid Flex - Part 2

How are flex, and rigid flex PCBs manufactured? In this blog I discuss how the materials are combined, laminated and cut out to create the final product.

Read more

31 July 2013

Ruminating Rigid Flex - Part 1

More and more designers are facing the need to reduce size and cost of the products they design, while increasing density and simplifying assembly.

Read more

More news


Define New Layer Stacks

Video (01:28:00)

Eagle Importer

Video (01:34:00)

Easier Neck Down

Video (00:00:38)

Consistent Pair Impedance

Video (00:00:46)


Monday, September 23, 2013

Ruminating Rigid Flex - Part 4


It’s easy to look at the problems of layer stack design, parts placement, and cutouts and think we’ve got the issues down. But remember in my first blog in this series how flex circuits have some gnarly material quirks. Quirks ranging from relatively high z-axis expansion coefficients of adhesives, to the lower adhesion of copper to PI substrate and coverlay, to copper’s work hardening and fatigue. These can be compensated for largely by following some Dos and Don’ts.

Do Keep Flex Flexible

This may seem obvious, but it’s worth saying. Decide just how much flex is needed up front. What I mean is; if your flex-circuit sections are only going to be folded during assembly and then left in a fixed position - such as in a handheld ultrasound device - then you are a lot freer in the number of layers, the type of copper (RA or ED) and so on you can use. On the other hand, if your flex-circuit sections are going to be continually moving, bending or rolling, then you should reduce the number of layers for each sub-stack of flex, and choose adhesiveless substrates.

Then, you can use the equations found in IPC-2223B (Eq. 1 for single-sided, Eq. 2 for double, etc.) to determine what is your minimum allowable bending radius for the flex section, based on your allowed deformation of copper and the characteristics of the other materials.

This example equation is for single-sided flex. You need to choose EB based on the target application, with 16% for single-crease installation of RA copper, 10% “flex-to-install” and 0.3% for “dynamic” flex designs (Source: IPC-2223B, 2008 Here, dynamic means continuous flex and roll during use of the product, such as a TFT panel connection on a mobile DVD player.

Don’t Bend at Corners

It is generally best to keep copper traces at right-angles to a flex-circuit bend. However there are some design situations where it’s unavoidable. In those cases keep the track work as gently curving as possible, and as the mechanical product design dictates, you could use conical radius bends.

Figure 1: Preferred bend locations.

Do Use Curved Traces

Also referring to figure 1 above, it’s best to avoid abrupt hard right-angle trackwork, and even better than using 45° hard corners, route the tracks with arc corner modes. This reduces stresses in the copper during bending.

Don’t Abruptly Change Widths

Whenever you have a track entering a pad, particularly when there is an aligned row of them as in a flex-circuit terminator (shown below), this will form a weak spot where the copper will be fatigued over time. Unless there is going to be stiffener applied or a one-time crease, it’s advisable to taper down from the pads (hint: teardrop the pads and vias in the flex circuit!)

Figure 2: Trace width change and pad entries can cause weak spots.

Do use Hatched Polygons

Sometimes it’s necessary to carry a power or ground plane on a flex circuit. Using solid copper pours is okay, as long as you don’t mind significantly reduced flexibility, and possible buckling of the copper under tight-radius bends. Generally it’s best to use hatched polygons to retain a high level of flexibility.

While thinking about this one, it also occurred to me that a normal hatched polygon still has heavily biased copper stresses in 0°, 90°, and 45° angle directions, due to alignment of hatch traces and ‘X’es. A more statistically optimal hatch pattern would be hexagonal. This could be done using a negative plane layer and an array of hexagonal anti-pads, but I found it fast enough to build the hatch below with cut-and-past.

Figure 3: Using hexagonal hatched polygons can spread the tension biases evenly among three angles.

Do Add Support for Pads

Copper on a flex circuit is more likely to detach from a polyimide substrate, due to the repeated stresses involved in bending as well as the lower adhesion (relative to FR-4). It is especially important therefore to provide support for exposed copper. Vias are inherently supported because the through-hole plating offers a suitable mechanical anchor from one flex layer to another. For this reason (as well as z-axis expansion) many fabricators will recommend additional through-hole plating of up to 1.5 mils for rigid-flex and flex circuits. Surface mount pads and non-plated-through pads are referred to as unsupported, and need additional measures to prevent detachment.

Figure 4: Supporting through-hole pads in flex with plating, anchoring stubs, and reduced coverlay access openings.

Referring to figure 4, the second option is good for adhesive coverlay and the third for adhesiveless. Coverlays attached with adhesive will exhibit “squeeze out” of the adhesive, so the pad land and the access opening must be large enough to allow for this while providing a good solder fillet.

SMT component pads are among the most vulnerable, especially as the flex circuit may bend under the component’s rigid pin and solder fillet. Figures 5 and 6 show how using the coverlay “mask” openings to anchor pads one 2 sides will solve the problem. To do this while still allowing the right amount of solder the pads have to be somewhat larger than typical rigid-board footprints would have. This is compared in figure 6, with the bottom SMD footprint used for flex mounted components. This obviously reduces the density of flex circuit component mounting, but by nature flex circuits cannot be very dense compared with rigid.

Figure 5: Coverlay openings for an SOW package showing anchoring at each end of each pad.

Figure 6: Adjusting the pad sizes and “mask” opening for coverlay. The top land pattern is for a nominal 0603 size chip component, whereas the bottom is modified for coverlay anchoring.

Double-Sided Flex

For dynamic double-sided flex circuits, try to avoid laying traces over each other on the same direction (figure 7). Rather stagger them so the tensions are more evenly distributed between copper layers (figure 8).

Figure 7: Adjacent-layer copper traces are not recommended.

Figure 8: Staggered adjacent-layer traces are preferred.

This is by no means a complete set, but You should now have a few good tips on how to design flex circuits to give the best yield and highest reliability for the product - but be aware of the tradeoffs between cost, performance and reliability.

In my next blog, I’ll be wanting to whet your rigid-flex appetites, by considering a few example applications of this technology, and hopefully some novel ideas will arise as a result.


Wednesday, September 18, 2013

Ruminating Rigid Flex - Part 3

Fab documentation for flex circuits and rigid-flex boards.

In the last blog on rigid-flex PCBs, I talked about the fabrication processes typically used by board houses. It's important to understand the steps required to build up a rigid-flex or flex circuit PCB because it has a big effect on how you need to design the board. And it also affects what needs to be included in your fabrication data set to send the design to successful fabrication. If you haven't read parts 1 and 2 of this blog, go read them here and here before continuing on.


Let's talk about documentation then. This is essentially where we tell the fabricator what we want, and it's probably the most likely part of the process where errors or misunderstandings can make costly delays happen. Fortunately there are standards we can reference to make sure we are communicating clearly to the fabricator, in particular IPC-2223B (which I am referencing in writing this).

It could boil down to a few golden rules:

  • Make sure your fabricator is capable of building your rigid-flex design.
  • Make sure they collaborate with you on designing your layer stack to fit their particular processes.

·         Use IPC-2223 as your point of reference for design, making sure the fabricator uses the same & related IPC standards - so they are using the same terminology as you.

  • Involve them as early as possible in the process.

Output Data Set

In interviewing a handful of rigid-flex capable board houses locally, we found that many designers still present gerber files to the board house. However ODB++ v7.0 or later is preferred, since it has specific layer types added to the job matrix that enable clear flex-circuit documentation for GenFlex® and similar CAM tools. A subset of the data included is shown in table 1.

Table 1: Subset of Layer Types in ODB++ (v7.0 and later) used for GenFlex

(Source: ODB++ v7.0 Specification)

Layer Type

Base Type




Clearances of a coverlay layer



Clearances of a covercoat layer



Pattern for die-punching of the flex circuit



Shapes and locations of stiffeners to be adhered

Bend Area


Labelling of areas that will be bent while in use



Pressure Sensitive Adhesive shapes and locations



An area definition (Rigid, Flex, or arbitrary)

Exposed Area


An exposed area of an inner layer and its associated coverlay (could also be used for embedded components)

Signal Flex


A signal layer for a flex circuit

Power Ground Flex


A power of ground layer for a flex circuit

Mixed Flex


Mixed layer for a flex circuit

Plating mask


A mask for defining which areas within a layer should be masked off from plating process

Immersion Mask


A mask for defining which areas within a layer should be masked off for immersion gold

There are some issues we face if using gerber for the output data set, or earlier versions of ODB++. Namely, the fabricator will need separate route tool paths and die cut patterns for each rigid and flex circuit section in the layer stack. Effectively, mechanical layer films would need to be produced to show where voids need to be in the rigid areas, and more to show where coverlay or covercoat will be on the exposed flex circuit areas. The coverlay or covercoat also has to be considered a mask for component pads for those components that may be mounted on flex circuit areas.

In addition, careful attention needs to be paid to layer pairs for drilling and through-hole plating, because blind vias from a rigid surface layer down to an opposing flex-circuit layer will have to be back-drilled and add significant cost and lower yield to the fab process.

As a designer, the question is really then, how can I define these areas, layers and stacks?

Define the stack by area using a table

The most important documentation you can provide your fabricator is arguably the layer stack design. Along with this, if you're doing rigid-flex, you have to provide different stacks for different areas, and somehow mark those very clearly. A simple way to do this is make a copy of your board outline on a mechanical layer, and lay down a layer stack table or diagram with a pattern-fill legend for the regions containing the different layer stacks. An example of this is shown in figure 1.

Figure 1: An example of a stack diagram showing fill patterns for rigid and flex circuit areas.

In this example, I used the matching fill patterns for different stack areas to indicate which stackup layers are included in the Flexible part or the Rigid part. You can see here the layer item I named "Dielectric 1" is actually an FR-4 core, which could alternatively be considered a stiffener.

This poses a new problem, in that you also have to define in 2D space where bends and folds can be, and where you will allow components and other critical objects to cross the boundaries of rigid and flexible sections. I will discuss this a little more later on.

Conveying the PCB design intent

We all know a picture is worth a thousand words. If you can generate a 3D image showing flexible and rigid areas this will help the fabricator understand your intent more clearly. Many people do this currently with the MCAD software, after having imported the STEP model from the PCB design. Figure 2 is an example of this concept.

Figure 2: Bending up the mechanical model to show design intent.

This of course can have the added benefit of detecting flex to flex and flex to rigid interferences ahead of epic failure.

Parts Placement

You can see also from the image above, that rigid-flex designs imply that components might exist in layers other than top and bottom. This is a bit tricky in the PCB design software, because normally components must exist on top or bottom. So we need some ability to place components on inner layers.

Interestingly, Altium Designer has always supported pad objects on any layer, so this is not impossible. There's also an implication that silkscreen could exist on flex layers as well. This is not a problem, since coverlay material can adhere well to the silkscreen ink. The trick is more to make sure there's adequate contrast for the color of ink chosen against the coverlay material. Also, resolution is affected since the ink has to traverse a small gap beyond the screen to land on the flex circuit coverlay. Again, this is something that needs to be discussed with the fabricator to determine what's possible and economical.

Side note: If you're going to the effort of drawing the regions of the PCB which are exposed flex layers, and placing components on those regions, this also makes a reasonable method for placing embedded components into cutout regions of the board. You need to generate a set of very clear documents that show where the cutouts are and in which sections of the layer stack they apply. This is going to be limited depending on the fabricators methods - either back-drilling or multiple laminated stack-ups can be used. So communicating your intent and minimizing the number of separate cutout stack sections is important. It's best to completely avoid having intersecting cutouts from opposite sides of the board.

Side-note: Defining Flex Cutout

Notice in figure 1 how there are no hard corners, but rather there's a minimum radius to each angle? IPC recommends greater radii than 1.5mm (about 60 mils), to reduce the risk of tearing of the flex circuit at corners. The same goes for slots and slits in the flex - make sure there's a designed-in relief hole at each end of diameter 3mm (⅛") or more. Another example of this is shown below.

Figure 3: Slots, slits and inside corners should have tear-relief holes or tangent curves with minimum 1.5mm radius.

In order to produce reliable rigid-flex based products, there are many considerations relating the fabrication and the end-use of the flex circuit, to the design of the copper pattern. In the next blog I want to discuss several of these do's and don'ts. Look out for it!