Posts Tagged ‘PCB’
You are a backplane designer and have been assigned to engineer a new high-speed, multi-gigabit serial link architecture from several line cards to multiple fabric switch cards across a backplane. These links must operate at 6GB/s day one and be 10GB/s (IEEE 802.3KR) ready for product evolution. The schedule is tight, and you need to come up with a backplane architecture to allow the rest of the program to progress on schedule.
You come up with a concept you think will work, but the backplane is thick with over 30 layers. There are some long traces over 30 inches and some short traces of less than 2 inches between card slots. There is strong pressure to reuse the same connector you used in your last design, but your gut tells you its design may not be good enough for this higher speed application.
Finally, you are worried about the size and design of the differential via footprint used for the backplane connectors because you know they can be devastating to the quality of the received signal. You want to maximize the routing channel through the connector field, which requires you to shrink the anti-pad dimensions, so the tracks will be covered by the reference planes, but you can’t easily quantify the consequences on the via of doing so.
You have done all you can think of, based on experience, to make the vias as transparent as possible without simulating. Removal of non-functional pads on the inner layers, and planning to back-drill the connector via stubs will help, but is it enough? You know in the back of your mind the best way to answer these questions, and to help you sleep at night, is to put in the numbers.
So you decide to model and simulate the channel. But to do so, you need accurate models of the vias to plug into your favorite circuit simulator. But how do you get these? You have heard it all before; “for high-speed, the best way to model a via is with a 3D electro-magnetic field solver”. Although this might be true, what if you don’t have access to such a tool, because the cost is more than your company wants to spend, or because you don’t have the expertise nor the time to learn how to build a model you can trust to make a timely decision?
On top of that, 3D field solvers typically produce S-parameter behavioral models. Since they represent only one sample of a given construction, it is impossible to perform what-if, worst case, min/max analysis with a single behavioral model. Because of this, many iterations of the model are required; causing further delay in getting your answer.
A circuit model on the other hand, is a schematic representation of the actual device. For any physical structure, there can be more than one circuit model to describe it. All can give the same performance, up to some bandwidth. When run in a circuit simulator, it predicts a measurable performance of the structure. These models can be parameterized so that worst case analysis can be explored quickly.
The problem with a circuit model is that you often need a behavioral model to calibrate it, or need to use analytical equations to estimate the parameters. But, as my friend Eric Bogatin often says, “an OK answer NOW! is better than a great answer late”.
In the past, it was next to impossible to develop a circuit model of a differential via structure without a behavioral model to calibrate it. These behavioral models were developed through empirical formulas, measured data, or through the use of 3D EM field solvers.
Now, there is another way. I have nicknamed it, “The Poor Man’s PCB Via Modeling Methodology”. Here’s how it works.
Anatomy of a Differential Via Structure:
The via barrel is a plated through hole extending the entire length of a PCB stack-up. The outside diameter equals the drill diameter. The inside diameter is the finished hole size (FHS) after plating. Pads are used on layers to ensure there is sufficient copper for track attachment after drilling operation. When used in this fashion, they are referred to as functional pads. Anti-pads are the clearance holes in the plane layers allowing the via barrel to pass through them without shorting.
The via portion is the length of the barrel connecting one signal layer to another. It is often referred to as the through via since it is part of the signal net. The stub portion is the rest of the barrel extending to the outer layer of the PCB. In high-speed designs, a good rule of thumb to remember is that a via stub should be less than 300mils/BR in length; where BR is the bit rate in Gb/s.
Building a Simple Scalable Circuit Model:
On close examination of Figure 2, a differential via structure can be represented by a twin-rod transmission line geometry with excess capacitance (shown in red) distributed over its entire length. The smaller the anti-pad diameter, the greater the excess capacitance. This ultimately results in lower via impedance, causing higher reflections.
In all high-speed serial link designs, it is common practice to remove all non-functional pads and to maximize the anti-pad clearance as much as practically possible. Oval anti-pads are often used in this regard to further mitigate excess via capacitance.
Figure 3 illustrates the equivalent circuit for a differential via that could be used in a channel topology simulation. Here it is modeled with Agilent ADS software using a coupled line transmission line model for each section. This equivalent circuit model can be scaled for any combination of layer transitions and integrated in any channel simulation scenario.
Since the cross-section of the via is constant throughout its length, the differential impedance of all sections of the via are the same. We only need to know the physical length of each segment and the effective dielectric constant (Dkeff) to get the time delay of each segment.
When driven differentially, the odd-mode parameters of each via are of major importance. Since the even-mode parameters have no impact on differential performance, both odd and even-mode parameters are set to the same values in the model.
The challenge then is to calculate the odd mode impedance (Zodd), representing the individual via impedance (Zvia), of a differential via structure and the effective dielectric constant (Dkeff) based on its geometry. Simple equations are used to determine these parameters.
Developing the Equations:
Anti-pads can vary in size and shape. They can be anything from round, to oval around each via, or even a large oval surrounding both vias as illustrated in Figure 4. Square, or rectangular variations (not shown) are similar.
Referring back to Figure 2, we see the structure of each via looks a lot like two coaxial transmission lines with the inner layer reference planes acting like a shield. Electrostatically this is a good approximation, but because the shield is not continuous, the magnetic fields are not contained like they are in a coaxial structure. Instead they behave more like magnetic fields around a twin-rod structure.
So here lies the secret in modeling a differential via. We take the best of both geometries to calculate the odd-mode impedance representing Zvia.
For inductance, we will use the odd-mode inductance formula from the twin-rod transmission line geometry to calculate Lvia :
Referring to Figure 4, we then calculate the odd-mode capacitance for Cvia derived from an approximate formula for an elliptic coaxial structure developed by M.A.R. Gunston in his book, “Microwave Transmission Line Impedance Data” . In the original formula, both shield (W’+b) and inner conductor (w+t) are elliptical in shape and are dimensioned as shown. When the anti-pads are circular, then ln[(W’+b) /(w+t)] reduces to just ln[b/t)]; which is the denominator in the Ccoax equation. If we use Gunston’s approximation to calculate Cvia, then the equation becomes:
Since conventional FR4 type laminates are fabricated with a weave of glass fiber yarns and resin, they are anisotropic in nature. Because of this, the dielectric constant value depends on the direction of the electric fields. In a multi-layer PCB, there are effectively two directions of electric fields.
The one we are most familiar with has the electric fields perpendicular to the surface of the PCB; as is the case of stripline shown here in Figure 5. The dielectric constant, designated as Dkz in this case, is normally the bulk value of the dielectric specified by the laminate manufacturer’s data sheet.
The other case has the electric fields running parallel to the surface of the PCB, as is the case when a signal propagates through a differential via structure. In this situation, the dielectric constant, designated as Dkxy, can be15-20% higher than Dkz .
Therefore, assuming a nominal 18% anisotropic factor, Dkxy = 1.18(Dkz)
Now that we have defined Lvia, Cvia and Dkavg, Zvia can be estimated using the following equation:
But we are not finished yet. We still need to determine the effective dielectric constant (Dkeff) in order to accurately model the delay through the via and stub portion. Without the correct value, the quarter-wave resonant nulls in the insertion loss plot, due to the stub length, cannot be accurately predicted. The value for Dkeff is determined based on how much the via’s odd-mode impedance is decreased due to the distributed capacitive loading of the anti-pads.
To help us with this task, we start with the twin-rod formula. The odd-mode impedance (Zodd) is half the differential impedance (Ztwin), and is expressed as:
By substituting Equation 1 for Zodd into the equation above, and solving for Dkeff we eventually come up with the following equation:
Validating the Model:
A simple 26 layer test vehicle was fabricated to compare the accuracy of the differential via circuit model to real vias. It consisted of two differential via pairs separated by 6 inches of 100 Ohm stripline differential pairs. Three sample via structures representing long, medium and short via stubs, as summarized in Figure 6, were measured using an Agilent N5230A VNA.
The differential vias had the following common parameters:
Via drill diameter; D = 28 mils
Center to center pitch; s = 59 mils
Oval anti-pads= 53 mils x 73 mils
Dk of the laminate = 3.65
Anisotropy in Dkxy = 18%
Zvia = Zstub = 31.7 Ohms (per Equation 1)
Dkeff = 6.8 (per Equation 2)
Agilent ADS software was used to model and facilitate simulation correlation of the measured data as captured in Figure 7. This simple model accounts for the discontinuity of the long through section and the long stub section. The top half is the measured channel using an S-parameter file. The bottom half is a circuit model of the channel. Since the probes were not calibrated out, they are part of the device under test. The balun transformers are used to facilitate the display of the S-parameter and TDR results.
The comparison between the measured and simulated results of the insertion loss and TDR response for the three via stub cases using this simple approximation methodology is summarized in Figure 8. The insertion loss plots, in the frequency domain, are shown on the left, while the TDR plots are shown on the right.
The resonant nulls in the SDD21 plots are due to the stub lengths. As you can see, the longer the stub, the lower the resonant frequency null. If this null happens at the Nyquist frequency of the bit rate, the eye will be totally closed. This is why we back-drill them out after the board has been fabricated.
The simulation correlation is excellent up to about 12 GHz. The TDR plots show excellent impedance matching and delay for all three cases, while the simulated stub resonant frequencies match the measured frequencies very well. As you can see, these simple approximations for Dkeff and Zvia are perfectly adequate in providing a quick and accurate circuit model for differential through hole vias typically used in backplane applications.
As illustrated, a simple twin-rod model (Figure 2) is used as the basis for a practical differential via circuit modeling methodology. By using Equation 1 and Equation 2, you can quickly determine the odd-mode impedance and effective dielectric constant needed for the circuit model.
Of course, you should use this methodology first as a rough starting point to quickly estimate the performance of your differential via design. If your worst case topology simulations show the performance is marginal, then it is worth while to invest the time and money to develop a 3D full wave model to perform a more accurate analysis.
On the other hand, if you find this approximation shows the vias have little impact on the channel performance, it may be of greater value for you to invest your time and money in resolving other critical issues with your design.
Try it the next time you are losing sleep over your design challenges.
For more Information:
If you liked this design note and want to learn more, or get more details on this innovative via modeling methodology, you can visit my web site, LAMSIM Enterprises.com , and download a copy of the white paper I wrote along with Eric Bogatin and Yazi Cao titled, “Method of Modeling Differential Vias” .
While you are there, feel free to investigate my other white papers and publications.
If you would like more information on our signal integrity and backplane services, or how we can help you achieve your next high-speed design challenge, email us at: firstname.lastname@example.org.
PCB cross-sectional geometries describe the details of the dielectric substrates, traces and reference planes within a PCB stack-up. Their physical relationship with one another can then be used to predict the characteristic impedance of the respective traces. There are only three generic cross-sectional geometries with variations within each. They are:
Coplanar geometry, or sometimes called coplanar waveguide (CPW), is a signal conductor sandwiched between two coplanar reference conductors or planes. These reference planes are usually ground. The characteristic impedance is controlled by the signal trace width and the gap between it and reference planes. This is a common transmission line structure for RF and microwave designs using single-sided printed circuit board technology. As a rule of thumb, the width of the reference plane on each side of the signal trace should be at least five times the distance between the left and right plane.
The microstrip line is the most popular transmission line geometry used in two or four layer printed circuit boards. The characteristic impedance is controlled by the signal trace width, on one side of the substrate, and the thickness of the substrate to the reference plane below it. The embedded microstrip line has the signal trace covered with prepreg or other dielectric material.
Cross section views below showing Microstrip line (left) and embedded microstrip line (right).
Cross section views below shows an example of single stripline (left) and dual stripline (right) geometries. These are geometries are typically found in multi-layer PCBs of 6 layers or more. The characteristic impedance is controlled by the trace width, thickness and its proximity to the reference planes above and below.
Single stripline has one signal layer sandwiched between two reference planes. If the signal layer is exactly spaced between the two reference planes, the geometry is called a symmetrical stripline; as opposed to an asymmetrical stripline, where the signal trace is offset from the center of the cross-section.
Dual stripline geometries have two signal layers sandwiched between reference planes, and are mainly used to save layers; caveat is a trace on one layer is routed orthogonal to the trace on the other to mitigate crosstalk.
Differential Pair Geometry:
Differential signaling is when a signal and its complement are transmitted on two separate conductors. These conductors are called a differential pair. In a PCB, both traces are routed together with a constant space between them as edge-coupled or broadside-coupled.
Edge-coupled routes the traces side-by-side on the same layer as microstrip or stripline. The advantage is that any noise on the reference plane(s) is common to both traces and thus cancelled at the receiver. Most differential pairs are routed this way.
Broadside-coupled routes one trace exactly over the other on 2 separate layers as dual stripline. Since each trace is more tightly coupled to its adjacent reference plane than the opposite reference plane, any noise on the planes will not be common to both traces and thus, will not be cancelled at the receiver. Because of this, and the fact that it usually results in a thicker PCB, this geometry is rarely used.
Consider a pair of equal width microstrip line traces, labeled 1 and 2, with a constant spacing between them. Each individual trace, when driven in isolation, will have a characteristic impedance Zo, defined by the self-loop inductance and self-capacitance of the trace with respect to the reference plane.
When a pair of traces are driven differentially, the mode of propagation is odd. If the spacing between the transmission lines is close, there will be electromagnetic coupling between the two traces. This coupling is defined by the mutual inductance and capacitance.
The proximity of the traces to a reference plane(s) influences the amount of electromagnetic coupling between traces. The closer the traces are to the reference plane(s), the lower the self-loop inductance, and the stronger self-capacitance to the plane(s); resulting in a lower mutual inductance, and weaker mutual capacitance between traces. The result is a lower differential impedance.
A 2D field solver is usually used to extract the parameters for a given geometry. Once the RLGC parameters are extracted, an L C matrix can be set up as follows:
The self-loop inductance and self-capacitance for trace 1 and 2 are L11, C11, L22, C22 respectively. The off diagonal terms in each matrix, L12, L21, C12, C21, are the mutual inductance and mutual capacitance. We use the LC matrix to determine the odd-mode impedance.
The odd-mode impedance is the impedance of one trace, of a differential pair, when driven differentially. It can be calculated by the following equation:
Zodd = odd mode impedance
Lo = self-loop inductance = L11 = L22
Co = self-capacitance = C11 = C22
Lm = mutual inductance = L12 = L21
Cm = mutual capacitance = |C12 |=|C21|
Even Mode Impedance:
When current flows down both traces, of the same polarity, the mode of propagation is even and the coupling is positive. The even mode impedance can be calculated using the following equation:
The differential impedance is twice the odd-mode impedance:
When current flows down two traces randomly, as if they were single-ended, the mode of propagation is a combination of odd and even. The average impedance of each trace is affected by its proximity to the adjacent trace(s); calculated by the following equation:
The coupling coefficient, Kcc, is a number that conveys the amount of electromagnetic coupling between two traces. Knowing the odd and even mode impedances, Kcc can be calculated by the following equation:
Backward Crosstalk Coefficient:
Two traces near one another will couple a portion of its own signal to the other. If we consider one trace as the aggressor, and the other as the victim, the amount of coupled noise travelling backwards on the victim’s trace, opposite to the aggressor’s direction, is called Near-End crosstalk (NEXT) or backwards crosstalk. The amount of coupled noise, travelling in the same direction as the aggressor’s direction, is called Far-End crosstalk (FEXT).
In stripline, there is little to no FEXT, but backwards crosstalk will saturate to a fraction of the amplitude of the aggressor’s voltage for the length of time the traces are coupled. This fraction of the aggressor’s voltage is called the backward crosstalk coupling coefficient Kb. It is equal to one half of the coupling coefficient Kcc :
A 8-9-8 mil differential pair; with 12mil core; 12 mil prepreg; Dk=4; stripline geometry; 1/2 oz copper; has the following R L G C matrix extracted from a 2D field solver:
If the two traces are driven differentially, then the differential impedance is 100 Ohms and there is 14% coupling of the two traces. On the other hand, if the traces are driven single-ended then the characteristic impedance of each trace is 57 Ohms. With 9 mils of space between them, the backward crosstalk is 7%.
If you increase the spacing between traces until Zodd equals approximately Zeven, the coupling will reduce to near zero, and there will be little backward crosstalk. For this particular geometry, increasing the space to 50 mils gives Zodd = 61.5 Ohms and Zeven = 61.7 Ohms for Kb = 0.07 %. Depending on your design and your noise budget, you may be able to live with a certain amount of backwards crosstalk. The only way to know the spacing between traces to achieve the budget is to plug in the numbers.
I would like to thank my old Nortel colleague, Dick Goulette for sharing these equations many years ago. They have served me well over the years.
Thick backplanes with long via stubs will cause unwanted resonances in the channel insertion loss compared to vias with little or no stub length as shown by the red and green traces in the plot of Figure 1. If these resonances occur at or near the Nyquist frequency of the bit rate, there will be little or no eye-opening left at the receiver.
Figure 1 Topology circuit model of 2 differential vias with 30 inches of PCB etch. Insertion loss plot of Long via-no stub (green); short via-long stub (red); stub terminated (blue). Received eye diagrams after optimized FFE receive equalization at 10GB/s. Modeled and simulated using Agilent ADS.
In a typical backplane application, the signal entering the via structure from the top will travel along the through portion until it reaches the junction of the internal track and stub. At that point, the signal splits with some of the signal continuing along the trace, and the rest continuing along the stub. If the signal was Arnold Schwarzenegger, he would say, “I’ll be back!”. Having done this gig before, he knows that when he reaches the end of the stub it’s like hitting a brick wall; there’s no where to go but back up the stub. Like Arnold, when the signal reaches the end of the stub, it reflects back up the stub. When it arrives at the same junction, a portion combines with the original signal and the rest continues back toward the source. If the round trip delay is half a cycle, the two waves are completely 180 degrees out of phase and there is cancellation of the original signal. The frequency where maximum cancellation occurs is called the ¼ wave resonant frequency, fo. Resonance nulls due to stubs in an insertion loss plot, like the one shown in Figure 1, occurs at the fundamental frequency fo and at every odd harmonic.
If you know the length of the stub (in inches) and the effective dielectric constant Dkeff, the resonant frequency can be predicted with the following formula:
It is common practice to reduce stub lengths in high-speed backplane designs by back-drilling the stubs as close as possible to the active internal signal layer. This is a complex and costly process involving setting individual drill depths on a per board basis. Special design features must be designed into the artwork to set correct back-drill depth. Furthermore, it is difficult to verify ALL back-drilled holes were drilled correctly. I know of a case where a backplane came back and one via (that they knew of) had a significantly longer stub than was specified. The problem showed up by accident when they were characterizing the channel using a VNA and saw an unexpected resonant null in the SDD21 insertion loss plot. When all was said and done, it turned out there was a glitch in the fabricator’s software controlling the back-drilling process. There is no practical way to find these faults; short of doing VNA measurements on 100% of the back-drilled holes. With hundreds of them in a typical high-speed backplane, the cost would be prohibitive. Thus we have to trust the fabrication process of the vendor(s).
If only there was a way to terminate the stub and get rid of all this back-drilling. Well there just might be a solution. After returning from last year’s DesignCon2010, I was intrigued by a paper presented by Dr. Nicholas Biunno on a new matched terminated stub technology developed by Sanmina-SCI Corporation. They call this technology MTSviaTM and it allows the embedding of metal thin-film or polymer thick film resistors within a PCB stack-up during its fabrication. I like to call it “The Stubinator”. They developed this technology as an alternative to back-drilling. The beauty of this is you can terminate all the high-speed via stubs on just one resistive layer at the bottom of the PCB.
Of course, for this to work, we need to terminate the vias with a resistance equal to the differential via impedance to be most effective. But how do we determine the via differential impedance without going through a bunch of trial and error builds? In a DesignCon2009 paper titled, “Practical Analysis of Backplane Vias” I coauthored with Eric Bogatin from Bogatin Enterprises L.L.C., Sanjeev Gupta and Mike Resso from Agilent Technologies, we showed how you can model and simulate differential vias as simple twin-rod transmission line structures using simple transmission line circuit models as shown in Figure 1. You can download a copy of this award-winning paper from my web site at: Lamsimenterprises.com .
After determining fo (either by measurement of a real structure or through 3D modeling) and solving for Dkeff by rearranging equation (1), the differential via impedance calculated using the following equation:
s = the center to center spacing of the vias
D = Drill diameter.
The differential vias used in the model of Figure 1 has the following parameters:
s = 0.059 in.
D = 0.028 in.
stub_length = 0.269 in.
Dkeff = 6.14 by Equation (1) and fo=4.4GHz ;
Zdiff = 66 Ohms by Equation (2).
By adding a 66 Ohm resistor across the bottom of each via stub in the model, the blue trace in the plot shows the stub resonance has completely disappeared at the expense of an additional flat loss of about -10dB. The eye has opened up nicely.
This “Stubinator” technology looks like it could be a promising alternative to back-drilling. It resolves many of the issues and limitations highlighted above. Combined with silicon that can accommodate the additional signal loading, it may extend the life of traditional copper interconnections for next generation of Ethernet standards beyond 10GB/s.
According to Wiktionary, an Architect is: “A person who plans, devises or contrives the achievement of a desired result.” Because the backplane is the key component in any system architecture, the sooner you consider the backplane’s physical architecture near the beginning of a project, the more successful the project will be. If you think about it in the same way as designing a building, you would never consider building it without first engaging a building architect to plan and oversee the detailed design. Likewise, the backplane architect plans and oversees the physical backplane design before any layout is ever started. He or she works closely with a system-packaging engineer to satisfy the system requirements before any concept becomes final. Sometimes the original system architecture needs revisions due to physical limitations the backplane imposes. This can only be established with due diligence and planning during the high-level design stage.
Unlike other circuit pack designs used in the system, the backplane is much like the keel of a ship of which the rest of the ship’s construction depends on for support and structural integrity throughout its lifetime. Backplanes need to be right the first time so that circuit packs can interoperate together day one and be capable of supporting future system upgrades as technology advances. Once the system has been deployed into the field, it is next to impossible to change the backplane to correct any deficiencies or to upgrade for performance like you can by redesigning the plug-in circuit packs.
The seasoned backplane architect is a unique individual usually tasked to turn the system architect’s ideas and dreams, like the system block diagram example shown to the left, into reality. An often-misunderstood profession, backplane architects wear many hats to accomplish their goals. Often they must juggle the design requirements from many disciplines and decide on the best trade-offs for the final design. They must converse fluently with system architects, mechanical designers, circuit pack designers, connector suppliers, PCB layout designers, ASIC/FPGA and software engineers. They must be organized and meticulous in their documentation and design. But, most importantly, they must have a sound knowledge of mechanical, PCB layout/fabrication, signal integrity, power and EMC issues.
The greatest danger in leaving the backplane design as an afterthought is the connector selection and pin-out definition. If left to system packaging engineers and board designers to define, they may not be optimum for either performance or system cost. Many times system architects and packaging engineers will merely take the total number of signals and choose a connector with the highest pin density per inch without considering PCB routing or signal integrity implications. Inefficient routing of the traces leads to an increase in layer count and results in a thicker board. Thicker boards leads to higher hole aspect ratios and longer vias affecting high speed performance. Additional layer count impacts common equipment cost.
The high-level design stage is where the physical backplane architecture starts to take shape. It uncovers potential layout routing issues and gives you the confidence the design will work the first time. The importance of this stage cannot be overstated. It primarily drives these key activities:
Sanitizes the system architecture.
Defines the final selection of appropriate connectors.
Defines the connector signal partitioning and circuit pack pin-outs.
Provides the routing plan and design rules for layout.
Defines the net topologies for signal integrity analysis and link budgeting.
Facilitates the mechanical design of shelf and system packaging.
Defines the minimum slot pitch for optimum routing channels.
Facilitates early circuit pack floor planning and final card size.
Facilitates ASIC and FPGA pin selection for optimum routing to backplane connectors.
Estimates PCB layer count and board thickness.
Establishes an estimate for system cost of goods to support the business case.
Proper route planning and connector pin-out definition is vital for optimum performance. When done correctly, the final schematic capture and actual PCB layout will flow smoothly with no surprises. As an example, the left half of the figure (labeled HLD Plan) shows a sample of an inner layer high-level design route plan I did using Framemaker as the drawing tool on a design before any schematic was ever captured or pin-outs defined. Everything was planned from the number of layers to how the tracks needed to break out of the connector fields. The right half of the figure is the actual layout done in Cadence Allegro showing the inner layer routing of the artwork. The due diligence done in the high-level design stage made the actual layout fairly trivial. If you forgo this step, the worst-case scenario is the project will need to be reset to redesign shelf mechanicals or redefine card pin-outs causing delay in meeting time to market objectives and ballooning R&D costs. It’s a classic case of pay me now or pay me later.
At Lamsim Enterprises Inc., we can help you with these or any other design challenges you may have by providing innovative signal integrity and backplane solutions. Visit us at our web site at: lamsimenterprises.com .
Backplane Architecture Terms and Definitions
The following is a list of common terms and definitions associated with system architecture and backplane design:
A backplane is a multi-layered printed circuit board assembly serving as the backbone of a system. Its purpose is to interconnect several printed circuit board assemblies called circuit packs or cards using plug in connectors to form a complete system. These cards plug into one side of the shelf assembly. Usually in mission critical system applications like central office telco or data centers, the backplane is passive meaning it does not contain active semiconductor devices permanently attached as part of the final assembly. Usually only connectors are the only components, but occasionally capacitors and resistors are also used. Active backplanes on the other hand, contains active components and often found in enterprise or consumer grade applications
A midplane is similar to a backplane in function except that the circuit packs plug into both sides of the shelf assembly. In these systems, cards with I/O cabling from the faceplate plug into one side of the shelf, while non-I/O circuit pack plug in on the other side. Some midplane architectures have the front card plugged in orthogonally to the rear cards for high speed applications.
Parallel Bus Topologies
Parallel bus topologies carry data words in parallel on multiple traces from card-slot to card-slot across a backplane or from chip to chip on a circuit pack. Up until the late 1990’s, most system architectures used this form of interconnect. Due to signal integrity and timing issues associated with some parallel bus architectures with 10 to 16 card slots, the speed of the bus was limited to 25-66 MHz Two popular industry standard systems still using parallel busses today are CompactPCI and VMEbus.
The main issue with a parallel bus topology is fault tolerance where a single point of failure on the bus can bring down the entire system. Mission critical systems often had to employ redundant busses to guard against single point failures.
As performance demand increased, newer high speed system architectures were designed using serial technology in a point-to-point or point-to-multi-point switched fabric topologies.
Switched fabric, or just plain fabric, is the term most popular used in telecommunications and high-speed networks, including InfiniBand, Fiber Channel, PCIe, ATCA and other proprietary fabric based architectures. In these architectures, all data passes through the fabric before continuing to its destination. It offers better total throughput than parallel busses because traffic is spread across multiple physical links. It manages and controls all functions of the network and acts as a repeater for the data flow.
Single Star Topology
Star topologies are one of the most common high-speed serial topologies used in networks today. The advantage is it reduces the chance of network failure by connecting all of the systems to a central node. A failure of a link from any peripheral node to the central node results in the isolation of that peripheral node from all others. As a result, the rest of the systems remain unaffected.
In its simplest form, a single star topology consists of one central hub node interconnected point-to-point to other peripheral nodes resembling a spoke wheel or star configuration. When implemented in a backplane, the central node is usually the switched fabric card and the peripheral nodes are line cards. The fabric card switches messages between the other line cards in the network. The line cards usually have faceplate I/O connectors to connect to other shelves in a network.
The main disadvantage with a single star topology is high dependence of the system on the functioning of the central fabric. Failure of the fabric card can bring down the entire system. Because of this, mission critical systems employ two fabric cards for redundancy in a dual star topology configuration.
Dual Star/Multi-star Topology
The dual star or multi-star topology is similar to the star network topology except it has two or more central hub nodes interconnected point-to-point to other peripheral nodes. When implemented in a backplane application, these central nodes are usually the switched fabric cards and peripheral nodes are the line cards. The additional fabric(s) provides redundancy in mission critical system applications in case of failure, or for upgrading fabric card hardware.
Fully Connected Mesh Topology
A fully connected mesh topology, when applied to a backplane application, does not have one central fabric node(s) as in the case of star topologies. Instead, each line card node connects with all other line card nodes forming a mesh. Its major disadvantage is the number of connections grows significantly with the number of nodes. This requires additional backplane connector pins and layers to interconnect them. Because of this, it is impractical for large systems and only used when there are a small number of cards needing to be interconnected.
Fiber weave effect timing skew is becoming more of an issue as bit rates continue to soar upwards. For signaling rates of 5GB/s and beyond, it can actually ruin your day. For example, the figure on the left shows a 5GB/s received eye is totally closed due to 12.7 inches of fiber weave effect. It was modeled and simulated using Agilent ADS software.
So what is fiber weave effect anyways and why should we be concerned about it? Well, it’s the term commonly used when we want to describe the situation where a fiberglass reinforced dielectric substrate causes timing skew between two or more transmission lines of the same length. Since the dielectric material used in the PCB fabrication process is made up of fiberglass yarns woven into cloth and impregnated with epoxy resin, it becomes non-homogeneous.
The speed at which a signal propagates along a transmission line depends on the surrounding material’s relative permittivity (er), or dielectric constant (Dk). The higher the Dk, the slower the signal propagates along the transmission line. When one trace happens to line up over a bundle of glass yarns for a portion of its length, as illustrated by the top trace in the figure on the left, the propagation delay is different compared to another trace of the same length which lines up over mostly resin. This is known as timing or phase skew and is due to the delta Dk surrounding the respective traces.
Fiber weave effect is a statistical problem. It is not uncommon for PCB designs to have long parallel lengths of track routing without any bends or jogs. This is particularly true in large passive backplane designs. Because the fiber weave pattern tends to run parallel to the x-y axis, any traces running the same way will eventually encounter a situation of worst case timing skew if you build enough boards. This was demonstrated by Intel after compiling more than 58,000 TDR and TDT measurements over two years. In 2007, Jeff Loyer et al presented a DesignCon paper “Fiber Weave Effect: Practical Impact Analysis and Mitigation Strategies” where they published the data and proposed techniques to mitigate the effect of fiber weave skew. They showed statistically it is possible to have a worst case timing skew of approximately 16ps per inch representing a delta Dk of approximately 0.8.
In high speed differential signalling this is an issue because any timing skew between the positive (D+) and negative (D-) data converts some of the differential signal into a common signal component. Ultimately this results in eye closure at the receiver and contributes to EMI radiation.
You can calculate the timing skew using the following equation:
tskew = total timing skew due to fiber weave effect length (sec)
Dkmax= dielectric constant of material predominated by fiberglass.
Dkmin= dielectric constant of material predominated by resin.
c = speed of light = 2.998E+8 m/s (1.18E+10 in/s)
A practical methodology you can use to estimate the minimum and maximum values of Dk is by studying the material properties available from PCB laminate suppliers. Consider two extreme styles of fiberglass cloths used in modern PCB laminate construction as illustrated by the figure on the left. The loose weave pattern of 106 has the highest resin content of all the most popular weaves, while the tight weave pattern of 7628 has the lowest. Therefore, you could use the specified values of Dk for cloth styles 106 and 7628 to get Dkmin and Dkmax respectively. Once you have these and apply a tolerance, you can estimate the tskew .
Assume Fr4 material; one inch of fiber weave effect; Dk106= 3.34(+/-0.05) and Dk7628= 3.97(+/-0.05), then timing skew is calculated as follows:
Modern serial link interfaces use differential signalling on a pair of transmission lines of equal length for interconnect between two points. In a DesignCon 2007 paper, “Losses Induced by Asymmetry in Differential Transmission Lines” by Gustavo Blando et al, they showed how intra-pair timing skew between the positive (D+) and negative (D-) data caused an increase in the differential insertion loss profile due to timing induced resonances. These resonances appear as dips in the differential insertion loss profiles of the channel as shown in the following figure:
This figure presents the results from an ADS simulation I did recently of a PCIe Gen2 channel running at 5GT/s. The eye diagrams are at the receiver after approximately 30” of track length chip to chip. The channel model was parameterized to allow for adjusting the fiber weave effect length as required.
As you can see, when the length of the fiber weave effect induced skew increases from 0 to 12.7 inches, the fundamental frequency nulls in the differential insertion loss plots decrease. These nulls occur at the fundamental frequency (fo) and every odd harmonic.
Also, the eye shows some degradation at 5.6 inches of fiber weave effect and starts to distort significantly after 7.8 inches. At 12.7 inches, fo equals the Nyquist frequency of the data rate (in this case 2.5GHz) and the eye is totally closed.
You can predict the resonant frequency ahead of time and use it to gain some intuition before you simulate and validate the results. If you know the total intra-pair timing skew, fo is calculated using the following equation:
fo = resonant frequency
tskew = total intra-pair timing skew
Using tskew = 16 ps/in we calculated above and using 12.7 inches from the last simulation results in the figure above, the fundamental resonant frequency null is:
You can find more details of this phenomena plus a novel way to model and simulate it from a recent White Paper I published titled, “Practical Fiber Weave Effect Modeling”. It, along with other papers, is found on my website at LamsimEnterprises.com.
Present day FR4-style laminates used for PCB fabrication rely on woven glass fiber yarns to maintain the structural integrity of the finished product. These yarns are made up of electronic or E-Glass material. Because it is the same glass used in everything from Corvette bodies to boat hulls, it is a very inexpensive reinforcement material. NE-Glass has improved electrical and mechanical performance over E-Glass. It is used for higher performance laminate products such as Park Nelco 4000-13SI.
The table on the left shows five of the most common fiberglass styles used for laminate construction today. When glass fiber yarns are woven into fabric, the “Warp” yarns run the length of the roll, while the “Fill or Weft” yarns run the width. Yarn count refers to the number of warp threads per inch by the number of fill threads per inch.
Prepreg is the term we commonly use for a weave of glass fiber yarns pre-impregnated with resin which is only partially cured. The glass to resin thickness ratio defines the overall thickness of a prepreg mat. You can see from the table above, the typical resin content is a function of the thread count and yarn diameter. For example, the figure on the far left illustrates styles like 106 and 1080 having smaller diameter yarns and higher resin content. The right hand figure is indicative of yarns with larger diameter and lower resin content like style like 2116 or 7628.
When copper foil is attached to one or both sides of fully cured prepreg mats, the finished laminated panel is called a core. Both cores and prepreg mats are available in various panel sizes and thicknesses.
There are several different kinds of resin systems in use today to form prepreg and cores. The general specification FR4 is the most common. It refers to a specific fire-retardant level rather than specific resin chemistry. Since you have a choice of many laminates that meets the FR4 fire specification, there is no such thing as “standard FR4″. That being said, most of us consider “standard FR4” to mean a laminate having a typical dielectric constant (Dk) of about 4.3 and dissipation factor (Df) of 0.020 – 0.025 at 1MHZ and 50% resin content.
Each family of resin systems have their unique electrical and mechanical characteristics depending on the fiberglass style and resin chemistry. For example, Nelco 4000-6 at 50% resin content has a typical Dk of 4.0 and Df of 0.023 at 2.5GHz. A higher performance resin system like Nelco N4000-13 on the other hand, has a Dk of 3.7 and Df of 0.009 for the same resin content and frequency. This tells us two things:
A lower Dk means we can ultimately achieve an overall thinner board for the same characteristic impedance.
A lower DF means less high frequency attenuation allowing us to run at a higher bit rate or have longer traces.
When designing your board stack-up, it is best to refer the manufactures data sheet for exact values. The Park Electrochemical Corp. (Nelco) website is an excellent resource to explore when trying to decide on the best dielectric material to use for your next high-speed design.