Xpedition Enterprise Blog

Learn about the industry's most innovative PCB design flow, providing integration from system design definition to manufacturing execution.

We'll keep you updated on the latest design trends, and other interesting tech tidbits in the industry.

21 July, 2014

This is the third post in this series. View the first and second one.

In this series we have talked about the placement challenges that occur when we, as PCB designers, do not get complete information from the engineers. Without enough information, we can’t move forward independently.VernBlog_Placement3_ImageOption

So, how do we correct the issue? Training. But, in order to create a “rock star” design team, training must be a two way street.

First, the engineers must have confidence in you as a PCB designer. To build that confidence, they might need to work closely with you for a while as they train you in the method by which they like to see specific circuits and components placed. Engineers like to be very exact with their circuits, and two different ones may place the same circuit slightly different based on their application. As a PCB designer, you must take note during this training as your training of the engineer comes next.

As you start to gain the trust of your engineer, show them what you require as a layout designer for a high quality design that is completed in an efficient manner for a faster turnaround time.

We need to teach the engineers to provide complete information for their design, and not just notes and statistics – but true design layout intent from their perspective.

One method of providing intent is constraints, but often getting the engineer to add constraints to their schematic requires them to learn a complicated constraint system (and most will not even try).

But, we want placement intent. As demonstrated in the previous posts, the engineer can now provide some of that intent directly from the schematic. This includes placement information such as circuit grouping and even circuit group locations or rooms.  Groups can be passed to the PCB designer and layout directly, adjusted by the layout designer, and then passed back for review when needed. Then these groups can be used to rapidly floor plan a layout placement and easily reviewed prior to starting the finer and more intricate circuit placement.

Imagine that your engineer has created a FPGA design with a 2000+ pin device and hundreds of decoupling devices. What if the engineer grouped the decoupling devices hierarchically based on the functional banks of the FPGA? Would that provide intent? Of course it would, and it would be much better than a sheet in the schematic with thousands of decoupling devices to try and figure out.

What about re-use circuits or channels that are duplicated from the current or previous design? Pre-grouping these circuits will allow the layout tools to use copy circuit technology better to quickly place these groups.

With a bit of increased how-to knowledge, engineers can provide better information based on their intent, and it can easily be done right in their own schematics.

We will all make better design teams by sharing information in both directions. Take a look at this video on some other capabilities that can be passed from the schematic. But, if you have to do it old school, I have also provided a link to a design guidelines document [HERE] that I have used for many years. You are welcome to use it to help train your engineers. With the right information from your engineers, you are further empowered to design the best possible layout.

23 June, 2014

This is the third post in this routing series. View the first and second post.

Board fabricators will tell everyone that spacing is king. If the traces can be spread apart and centered between via and/or pin pads, then it will result in higher yields during the fabrication process. Fewer shorts will be created and less work will be required to remove them.

In Expedition PCB and Xpedition PCB Layout, we have a “Spread” routine in the “Auto Route” dialog that will automatically spread the traces apart and center them between pads. Based on my discussions with many AEs and customers, I suspect that many have tried to simply run it from the “Auto Route” dialog and found that it did not work as expected.

In fact, the expectation was that it would only spread the traces. Centering them turns out to be an unexpected yet wonderful bonus. The reason why it doesn’t work as expected is due to the fact that it requires some very specific setup. First, a text side-file is required that has the appropriate spacing values per layer; and second, a check-box in the “Auto Route” dialog needs to be set.  Let’s begin with the text side-file.

SpreadTo.txt

This file needs to be created and placed in the “Config” directory for the design you are working on.

ConfigDirectory

The contents of this text file include the units, the layer and the corresponding spread clearance for that layer.

SpreadTo

Units are “th.” By default, the units are the design units; so in most cases, this line is not even needed.

Then list the layers to be spread and the trace-to-trace clearance desired. Here, on both layers 3 and 4, the trace-to-trace spread clearance is 12th.

Auto Route Dialog

autoroute

To enable “Spread” to work, the ‘Allow “Cleanup” if not routed 100%’ check-box needs to be checked. This is because when “Spread” is included with a number of other routing passes, it (along with other cleanup routines) should usually not be run unless the design is routed completely. If you are just using “Spread,” this check-box must be checked.

Run the “Spread” pass with a 1-3 effort.  It will spread the traces as much as possible up to the spread clearance specified in the “SpreadTo.txt” file.

Example

Routing before “Spread”

RoutingBeforeSpread

After “Spread”

RoutingAfterSpread

Note that the differential pairs are not spread apart, but they are also spread away from other nets.

Caveat:  “Spread” does not push traces over via or pin pads. Because of this, you may want to move some traces around (as I did in this example) before running “Spread.”  This will maximize the effect of spreading and prevent extra jogs in traces that are trapped between vias in open space.

Centering Traces

If the spread value is large enough, then it will also center traces between vias and pin pads. What is considered large enough? For example, if a trace will be centered between via pads with a trace-to-via clearance value of 8th, then any spread value equal to or larger than 8th will center the traces. You don’t have to get the value exact; in fact, usually it will be larger due to the desire to spread the traces themselves significantly – so that will work just fine!

Example

Before “Spread”

The white arrows point to some places where the clearance is at minimum spacing and it would be good to center or move the traces away from the pads.

CenteringBeforeSpread

After “Spread”

The traces are centered where necessary and move away as appropriate.  Note that it will center just one trace or even two if needed.

CenteringAfterSpread

Conclusion

In the previous discussion, it was all about a method for centering traces.  Here we provide another method for spreading traces that also centers traces.  Which method do you like better?

16 June, 2014

This is the second post in this series. View the first one here.

A placement challenge that I had to endure reminds me of the Rolling Stones song, ‘Get Off of My Cloud.’ I imagine that many of you still endure a similar challenge today…

I was placing a design that I knew was going to take weeks to complete, after reviewing the schematic, I contacted the engineer with a list of concerns. I asked for some written instructions and a possible floor plan based on the mechanical chassis requirements. Here is what I received back: “I will come and sit with you during placement so we can get it right.” Ugh! These are the words no PCB designer wants to hear. They are the death knell to productivity. But I had no choice.

And so, for the next three weeks, I sat in a small office with another design colleague and this engineer who, by the way, was a guy who ate way too much garlic and was always sweating. It was a living hell!

Why can’t engineers write good instructions for placing a PCB? Why must they thrust themselves into the design, when they have signal integrity stuff to worry about? In the past, without creating a document in a word processor, there was no real way to specify design intent through the EDA tools. Plus, as the capabilities of adding constraints to a design have become available, they have stuck to their old ways.

Leaning over a PCB designers shoulder ties us up in addition to engineering resources, and requires so much more time than providing good instructions – or any instructions!

We need a tool that allows the engineer to easily add constraints, and even design placement intent, such that the PCB designer will understand component grouping and critical placement locations…without the need to have the engineer babysit the design. That time has come! Xpedition xPCB layout now has the ability, through component explorer, to aid in planning and placement from the onset of the schematic design through to completion of the PCB design.

Take a look at the link below on component planning and placement with component explorer. In our next discussion we will talk about how to tell your engineer, “Don’t hang around ’cause two’s a crowd, on my cloud baby!”

11 April, 2014

This is the second post in this routing series. View the introduction post here.

To increase fabrication yield, it is important to center the traces between the fanout vias inside the BGA area. Large BGAs are usually 1mm pitch and medium sized ones are 0.8mm. Then we go down to 0.65, 0.5, 0.45 and 0.4. Is anybody designing with even finer pitch BGAs?

In any case, it is important to center the traces between the ball pads and/or the fanout vias. If the routing is on the outer layers, then it is important that the traces do not get exposed with the soldermask openings. Of course, if the BGA pads are soldermask defined, then the problem of exposure is eliminated; however, this method is not always used.

On inner layers, any increase in the via-to-trace spacing will help to prevent shorts during the fabrication process. When fabricating boards, “Spacing is King.” You may also want to force the traces to be centered so they will not cross anti-pads on the plane adjacent to the signal routing.

Difficulties include various pin pitches, and we also have to deal with differential pairs along with the single-ended routing. As the pin pitches vary, rule areas can accommodate finer trace widths and spacing, and if set just right, it can automatically force either the differential pairs or individual traces to be centered. The problem is with “either.” If both differential pairs and individual traces need to be centered, a single spacing value will not force all the traces to be centered.

There is a method in existing Expedition PCB and Xpedition Layout that can be used to accommodate the centering of both single ended nets and differential pairs.

Solution: DRC Visualization and Repair

The step-by-step instructions are as follows:

1. Differential Pairs:  In the Constraint Manager, increase the trace-to-via (or if on the mount layer,  trace-to-pad) clearance to a value so that the differential signal will be centered. You can do this in the default rules, and if you are using rule areas around the BGA, you can do this for each of the rule areas.  I trust you can do the math.

2.Turn on visibility of all routing layers. Run the DRC Visualization routine.

DRCV

3. There is no need to look at all the violations – there will be many. After the DRC completes, select the traces you want to have centered, and click the right mouse button.

This menu will appear:

Menu

4. Choose “Repair Selected” and all the DRC violations that can be repaired will be repaired by pushing the traces away from the pads and vias.

5. Set your Gloss to “Local Gloss,” frame-select the traces that you just repaired, and then choose “Gloss.” This will remove any small segments that might have been created.

6. Do this method for all the BGAs that have differential pairs running through them.

7. Set the trace-to-via and trace-to-pad clearances back to the original values. You can also accomplish this by exporting the original constraints and then importing them back into the design.

8. Single-Ended-Nets:  After the differential pairs have been centered, go through the same cycle with single-ended-nets. The differential pairs will not be affected by this operation for single-ended nets.

9. Once the rules are reset to the original rules, do a full DRC to ensure that no other problems may exist or have been created during this centering process.

At this point, the vast majority of the traces will be centered as desired. It may read like a lot of steps, however, it is certainly much more effective than centering the traces manually.

Here is a video that illustrates centering of differential pairs.

Are there other methods that you would like to offer?

2 April, 2014

PlacementChallenges#1Long before video games, children had simpler means of entertainment. Boys had their army men and marbles. Girls had their coloring books and paper dolls. As a young boy, I used to watch my sister carefully cut out dolls and clothes to glue on them, and thought yuck!

15 years later I found myself doing the same thing…well kind of. If you have been in the PCB design industry for as long as I have, you likely remember the days when we placed boards by cutting out shapes for components to be placed on the boards and called them “Paper Dolls.” Back then, placement was not complex. We tried as best we could to get parts close to each other, but boards were nowhere near as dense as they are today. It was easier to get close when it came to placement; there weren’t many restrictions as long as you stay on that 100 Mil grid.

Today everything has changed. I am so glad to have CAD tools, because I do not think I could make a paper doll of a 01005 capacitor, considering they are about the size of a grain of sand. And, I can now place several parts in that 100 Mil, not just one. PCB designs today have much different placement challenges: density, thermal, mechanical, and more!

As a designer, it used to be that placement was easy and routing was tough, but that has changed. Advanced routers help shorten design schedules, but achieving the same for placement is much more difficult. Dense boards with thousands of components can take weeks to just get placed.

So, how do we solve this as designers? Placement strategy is a huge part of the success of a design. What new strategies can we invoke to place a board with the efficiency and quality we need in our product?

In this series, I will discuss some of the current challenges that face us during the placement phase of a design, plus how we can remove these challenges with sound placement strategies.

In the rest of this series, I will also cover some technology that’s included in the latest Xpedition release. In the meantime, take a look at this webinar which shows the new planning and placement technology available in this release.

What placement challenges are you facing on a daily basis?

26 March, 2014

You’ve likely heard that there has been a new release of the product formerly known as Expedition Enterprise, called Xpedition. So, what’s this release all about? How does the new functionality compare to the tools you use today and what’s in it for you?

I’m Vern Wnek, Technical Marketing Engineer for the Xpedition software group. But, before I lose you with that let me explain my background and why the discussions you and I will have through this blog are relevant. I’m a PCB designer by trade and have been in the industry for over 35 years. After designing boards, working in board houses, assembly houses and test facilities, I have landed where I’m at now. I’ve worked for service bureaus and large companies from military to commercial.

I’ve encountered the challenges and seen the industry evolve to better address them. I’m going to discuss efficiency in tools, processes, and technology trends. But most of all, I care about your challenges.

What are your challenges? What’s your take on the paradigm shifts of the industry and have any of them changed the way you look at PCB design?

Expedition has been the source of my livelihood since the days of Veribest. I have seen new versions come and go and tested a number of PCB design tools. Mentor Graphics is the best of the best and I’m not just saying that because I work here. I’m looking for you to challenge me. Prove me wrong. Show me what we’re missing. Let’s discover all that makes up Xpedition and how it’s relevant to you.

Here’s a glimpse of what’s to come:Xpedition Layout
•    Placement challenges and new strategies
•    New auto-assisted routing paradigms
•    3D integrated layout
•    System and multi-board design
•    PCB layout designer resource challenges
•    Industry trends in design technology and manufacturing of PCBs

Through our discussions on this blog, I think you’ll see that Xpedition VX is SO much more than just a rebranded name on a slightly new version of the Expedition Enterprise product. This latest release really has earned a new name and I’m looking forward to showing you why.

21 March, 2014

This is the first of a series of blog topics related to routing PCBs

My name is Charles Pfeil and my role at Mentor Graphics is one in which I always have a primary focus on routing technology and methods – although I do get involved in numerous other projects. I began in this industry working my summers in high school inspecting Ruby-Lithe designs for scratches and repairing them. Sounds rather antiquated? Indeed, this began in 1966 (some would say “way back” in 1966). I went to college to study architecture but soon realized that my passion for PCB design was so strong that I should pursue that instead.

After years of working as a job-shopper designing boards, I opened my own design service bureau, Sunshine Design. We started out with manual design and tape-ups. I still have some of those Mylar sheets with black tape-ups if anyone knows of a museum that might be interested them…I suddenly feel very old. In 1978, we made the change from manual design to CAD after getting two Racal-Redac Minis. During this transition, we lost all our customers who weren’t interested in CAD data. Fortunately, we were able to hook up with some customers who also used the Racal-Redac systems. At that point, CAD routing technology, both manual and automatic, became of great interest to me.

Since then I have worked at Racal-Redac, ASI, Cadence, Intergraph, VeriBest and Mentor Graphics. This industry has been very good to me and my career. I am grateful for all the wonderful people that I have met and worked with over these years.

CharlesIntroBlogPhoto

My goal for this blog is to provide meaningful discussion of routing problems and their solutions. Over the years the routing task has become much more complicated, not only due to evolving component and fabrication technology, but also the need to fulfill high-speed requirements and manage the signal integrity concerns. I look forward to hearing your ideas and methods and hope that the discussions we have will help better equip us to solve the routing challenges that we face.
Here are some topics I look forward to discussing with you:

  • Length of time needed to manually route a design
  • Difficulty of phase match tuning
  • The dense, tangled netlines between BGAs are hard to route
  • The need to center traces between vias in BGA fanout array
  • Fanout pattern complications and the difficulty of adding them

What challenges are you encountering? Are there any topics you would like me to add to my list?

19 November, 2013

Both veterans and newcomers to PCB systems design may appreciate this video on our website that showcases the evolution of PCB design over the past decades and the role that Mentor Graphics has played in this journey. While visiting our website, you may notice something else—we have introduced Xpedition, the new identity for our flagship PCB design flow.

Why have we introduced this new identity?

The technology in our upcoming release is groundbreaking and serves as a foundation for the next generation of proven, innovative thinking. It is so substantial that we believe it deserves a unique identity platform. But there is more to it than that.

Xpedition Identity

Xpedition represents the value and importance of the overall PCB design-to-manufacturing flow. For development organizations to be successful, they need to exploit every opportunity to drive greater productivity in their design flow while continuing to adjust for increasing complexity. This means they must reduce and eliminate process bottlenecks by deploying effective strategies for system definition, virtual prototyping, routing productivity, new product introduction, IP management, and design concurrency.

Proven Innovation

Since the 2005 release of Expedition Enterprise, Mentor Graphics has had a strong track record of delivering innovation tools including XtremePCB, CES, DxDesigner, and the world’s most productive PCB layout environment. This has made us the global leader, by far, in PCB systems design solutions. Xpedition builds on this legacy to deliver next-generation leadership technologies for modern PCB development teams.
Thank you to our customers for partnering with us in this ongoing journey. To those not yet familiar with us – we look forward to showcasing technologies that are, “jaw dropping…a huge leap in thinking and power,” as one Beta customer remarked.