I N T E R C O N N E C T A P P L I C A T I O N N O T E Advanced Mezzanine Card (AMC) Connector Routing Report # 26GC011-1 September 21 st, 2006 v1.0 Advanced Mezzanine Card (AMC) Connector Copyright 2006 Tyco Electronics Corporation, Harrisburg, PA All Rights Reserved
Table of Contents Item Page # I. INTRODUCTION...2 II. CONNECTOR OVERVIEW: ADVANCED MEZZANINE CARD (AMC)...3 A. Background...3 B. Typical Implementations...4 III. CONNECTOR DEFINITION...5 A. Drilled Hole Dimensions...5 B. Fabrication Technology...5 1. Pad Size...6 2. Non-functional Pads...6 3. Thermal Reliefs...6 4. Antipad Size...7 C. High-Speed Via Design...9 1. Counterboring...9 2. Blind Vias...9 IV. ROUTING...10 A. Routing Channels...10 B. Trace Widths...11 C. Skew & Propagation Delay...12 V. PART PLACEMENT...12 VI. ADDITIONAL INFORMATION...12 A. Gigabit Research and General Application Notes...12 B. Electrical Models...12 VII. CONTACT INFORMATION...13 The information contained herein and the models used in this analysis are applicable solely to the specified Tyco Electronics connector as dated by the document. All information should be verified that it is representative of the current implementation of the connector. Alternative connectors may be footprint-compatible, but their electrical performance may vary significantly, due to construction or material characteristics. Usage of the information, models, or analysis for any other connector or previous implementation is improper, and Tyco disclaims any and all liability or potential liability with respect to such usage.
Advanced Mezzanine Card (AMC) Connector Routing I. INTRODUCTION The PCI Industrial Computers Manufacturer s Group (PICMG) has recently developed a new mezzanine specification for plug-in cards, carrier boards, and applications, intending to provide the next generation step to the previously existing PCI Mezzanine Card (PMC) definition. The specification will further support and enhance the telecommunication industry s push to increase bandwidth, reliability, capabilities, and features of its systems. The Advanced Mezzanine Card (or AMC) specification additionally offers compatibility with PICMG s latest telecommunications development, the AdvancedTCA architecture. To support these applications from an interconnection perspective, an advanced mezzanine card connector definition was also defined. The AMC specification anticipates supporting single pair speeds as high as 12 Gbps, and at the same time, expects to provide a very robust and cost-effective product. Electrical, mechanical, and manufacturing aspects of the connector were analyzed simultaneously, to develop and optimize the AMC connector design. At the board level, these aspects combine with common board design practices to influence the design of the connector-to-board interface and how the board itself will be routed. The manner in which the connector is designed into the system can significantly impact the system s intended performance. Tyco Electronics has been actively researching these areas in an effort to help customers use the Advanced Mezzanine Card (AMC) connector in gigabit serial systems. The combination of interconnect research and intimate knowledge of the connector is presented to provide insight into the capability of an AMC-based system design. Furthermore, this document provides specific design recommendations that will address layout, electrical performance, and manufacturability tradeoffs of the connector at the board level. PAGE 2 September 21, 2006
II. CONNECTOR OVERVIEW: ADVANCED MEZZANINE CARD (AMC) A. BACKGROUND Figure 1: Advanced Mezzanine Card (AMC) Connector The Advanced Mezzanine Card (AMC) connector is a product combining low cost, high density, and high performance in a robust and durable component capable of intermating with any AMC-compliant (sometimes hot-) pluggable module board. At a contact pitch of 0.75mm, the connector provides 170 total pins in a 65mm package. The open-pin field connector can be arranged in differential or single-ended configurations, or a combination of both. The AMC specification provides for a pre-determined pinout which primarily consists of high-speed differential pairs capable of running up to 12 Gbps. Outstanding features of the product include a rugged overmolded single-piece design, fully-protected card-edge contacts, press-fit carrier board contacts, polarizing carrier board footprint features, additional optional hold-down features, and more. The carrier board contacts use an industry standard compliant pin technology for printed circuit board attachment. Family extensions such as AMC-compliant A+B+, AB, and B versions are expected as needed to support industry developments and further AMC applications. The Advanced Mezzanine Card (AMC) connector is ideally suited for pluggable coplanar mezzanine architectures which reside in high-speed telecommunications equipment, all classes of servers, and data storage and transport applications. PAGE 3 September 21, 2006
B. TYPICAL IMPLEMENTATIONS The AMC connector is a high-speed product that is typically implemented in high-speed differential applications, such as the already existing AMC specification. Although it can be implemented in single-ended applications as well, grounding schemes and pin assignments would require appropriate changes. The AMC connector provides a variety of application spaces, therefore only the most common implementation (the AMC specification definition) is described here. In the differential spec-compliant AMC implementation, only the carrier board footprint requires a detailed routing analysis. The plug-in module side of the connector provides for a straightforward two-sided surface-layer route. A section of the AMC carrier board footprint is shown in Figure 2. The illustrations in this section are specific to a subsection of the AMC connector and application, but can be equally applied across the entire length of the printed circuit board footprint. Refer to the latest customer drawings for overall dimensions and to the appropriate specifications for proper connector to connector spacing. Row B+ Row B Plug-In Card Insertion Side 2.25 mm Differential pair 0.75 mm Ground 1.4 mm 3.0 mm 1.4 mm Figure 2: AMC-Specific Carrier Card Pinout The connector consists entirely of only two rows on a 4.4mm pitch, the short and long rows being referred to as the B and B+ rows, respectively, as called out by the AMC specification. Each row has an alternating pin stagger of 1.4mm, providing for optimal electrical performance and routing capability within the footprint. The pin staggering results on only two distinct contact chiclet designs, alternating throughout the length of the connector, provided for a cost-effective connector design. The footprint also employs a central grounded row of vias on a 2.25mm pitch, providing for enhanced electrical performance within the PCB footprint itself. PAGE 4 September 21, 2006
III. CONNECTOR DEFINITION A. DRILLED HOLE DIMENSIONS Full mechanical dimensioning and tolerances are available for the Advanced Mezzanine Card (AMC) connector. These drawings can be located at www.tycoelectronics.com. The dimensions critical to the routing of the AMC connector are related to the hole pattern, or footprint, of the connector. Table 1 is provided to quickly identify critical hole dimensions for the circuit board. Hole Dimension Carrier Card Hole Diameter w/snpb Plating mm (in.) Carrier Card Hole Diameter w/out SnPb Plating mm (in.) Drill Hole Size 0.50 ± 0.02 (0.0197 ± 0.0008) 0.50 ± 0.02 (0.0197 ± 0.0008) Finished Hole Size 0.40 ± 0.05 (0.0157 ± 0.002) 0.425 ± 0.05 (0.0167 ± 0.002) Hole Copper Thickness 0.0375 ± 0.0125 (0.0015 ± 0.0005) 0.0375 ± 0.0125 (0.0015 ± 0.0005) Hole SnPb Thickness 0.0081 ± 0.0043 (0.00032 ± 0.00017) N/A B. FABRICATION TECHNOLOGY Table 1: Connector Hole Dimensions Other important dimensions for board layout are determined by the capabilities of the circuit board fabricator. Current high-tech PCB industry fabrication technology (i.e. capability) requires minimum pad sizes ranging from D+10 mils through D+16 mils, where D is the diameter of the drilled hole size (1 mil, or 0.001, is 0.0254 mm). The resultant pad size for a given technology is typically defined as the minimum pad size required to maintain 0.05 mm (0.002") of annular ring for a given PCB manufacturer s capability. Annular ring is an industry standard measure of the clearance between the pad edge and worst-case drill edge after manufacturing. For the AMC connector this results in minimum pad sizes ranging from 0.75 mm (0.0297") to 0.91 mm (0.0357"). Because the AMC connector has a rather dense footprint and is typically used in high speed or dense applications where routing issues are most significant, all pad dimensions in this document will assume a D+10 mil pad size, unless otherwise specified. The pad diameter may be optimized for specific project needs, and should be evaluated on a project and vendor basis. Designing with a PCB technology less than D+10 mils could mean reduced yields or breakout, potentially adding cost to the PCB or violating industry specification compliance. Note: A minimum pad to trace clearance of 0.10 mm (0.004") will also be assumed for calculating routing dimensions. PAGE 5 September 21, 2006
1. PAD SIZE Based upon the D+10 mil fabrication technology assumption, a 0.75 mm (0.0297") diameter pad should be used with all AMC connector pins. For higher-tech PCBs (D+8 mils, for example) the pad would be 0.70 mm (0.0277 ). Table 2 summarizes different pad sizes for common manufacturing capabilities. Connector Pins Signal & GND Pad size High-tech Low tech D+8 D+10 D+12 D+14 D+16 0.70 mm 0.75 mm 0.81 mm 0.86 mm 0.91 mm (0.0277 ) (0.0297 ) (0.0317 ) (0.0337 ) (0.0357 ) Table 2: Pad sizes for AMC Connector In some cases, the reduced manufacturability of a D+8 mil technology PCB or smaller is required to reduce pad sizes. A smaller diameter pad may potentially reduce yields by causing breakout or open connections, which results in added cost of the PCB. Where possible, the largest appropriate pad size should be used to provide the PCB manufacturer with the greatest flexibility, thereby reducing overall system costs. Although an increased pad size also reduces electrical performance by increasing the capacitance of the plated through-hole, this effect has only a minor impact when unused pads are removed from the signal via. 2. NON-FUNCTIONAL PADS The removal of non-functional internal pads will improve signal integrity and manufacturability of the PCB. However, some assembly facilities prefer that unused pads are retained in order to maintain hole integrity through various soldering processes. For electrical reasons, it is recommended that unused pads be removed on internal layers. 3. THERMAL RELIEFS Thermal reliefs are not required on ground or power pins, because the AMC connector uses a press-fit technology. A direct connection to reference and power planes will offer the lowest inductance connection to the circuit board. PAGE 6 September 21, 2006
4. ANTIPAD SIZE Via Antipads, or plane clearances (Figure 3), are required to separate signal holes from reference voltages to avoid shorting. Pad Choosing the proper size of these Trace clearances is critical in determining several other design parameters: signal integrity, EMI, voltage breakdown, and manufacturability. Determining the proper antipad size for Plane Antipad the AMC connector depends upon system design goals. Several scenarios are Figure 3: Antipad Illustration exemplified below. Antipad sizes are minimized: To reduce noise by closely shielding adjacent pins with reference planes To reduce EMI by minimizing aperture sizes in reference planes To maintain a strong reference to ground for single-ended traces and ground referenced differential traces Antipad sizes are maximized: To maximize voltage breakdown spacing between the pin and the reference plane To increase manufacturability by reducing the chance of shorting. To reduce reflections in a high-speed gigabit serial system by reducing the capacitive effect of the plated through-hole. In cases where antipads are minimized, the recommended antipad size is the pad diameter plus 0.25 mm (0.010 ). This size maximizes trace coverage, while not risking shorting the plane to the barrel in the case of drill breakout. Using a minimal antipad will increase the capacitance of the via and could degrade system performance at high speeds. When antipads are maximized, the antipad geometry is dependent on the type of signals passing through the vias. PAGE 7 September 21, 2006
The suggested antipad structure for differential signals encompasses two adjacent signal vias. This structure minimizes the via capacitance for both vias, while maintaining coupling between the two signals within the differential pair. The recommended antipad is designed to maximize routable trace widths and associated ground coverage. The antipad width can likely be increased to better balance trace ground coverage and minimization of via capacitance, once a trace geometry is determined. Figure 4 shows the recommended differential antipad in both oval and octagon geometries. Pad Pad W W L L Figure 4: Differential Antipad Geometries These antipad recommendations are related to the D+10 pad technology used. The D+10 pad size, labeled as Pad in Figure 4 is 0.75 mm (0.0297 ) in diameter. The antipad width labeled as W (top-bottom in the above figures) is 0.25 mm (0.010 ) bigger than the pad size. The resulting antipad width W should be 1.00 mm (0.0397 ). The antipad length L is dictated by the pad size, as well as adjacent in-row ground vias and the routing channel that may need to remain between the differential pair and in-row ground vias. Taking both pad size and ground vias into account, the antipad length L should be 2.60 mm (0.102 ). These resulting antipad dimensions of 2.60 mm (.0102 ) x 1.00 mm (.0397 ) represent a geometry which maximizes routable trace widths and associated ground coverage assuming a D+10 technology. A board design that uses a non-d+10 pad sizing, will result in different antipad length L and width W geometries. A board design that does not require the entire width of the routing channel (routable space between the differential pair and ground vias) should use a larger antipad width W and length L, to help with minimization of via capacitance. Routing geometries are discussed further in section IV. PAGE 8 September 21, 2006
C. HIGH-SPEED VIA DESIGN At gigabit speeds, one of the limiting factors in system design is the effect caused by the via stub in the board. A via stub is the portion of the via that is not in series with the transmission path of the signal, as shown in Figure 5. At high frequencies, this parallel path creates a significant capacitive discontinuity, which degrades the throughput of the link. Although it has a small impact at lower frequencies, this stub typically becomes critical at speeds greater than 3.125 Gbps. Figure 5 Via Stub The AMC connector was designed to allow for various techniques to be applied to treat the via and remove the stub, without impacting the press-fit contact in the hole. When fully seated, the bottom tip of the eye of needle extends 1.6 mm (0.063 ) into the hole. Beyond this depth, various techniques can be employed to modify the via to eliminate the stub. Consult your board fabrication facility regarding their capabilities for these advanced technologies. 1. COUNTERBORING Counterboring is a technique that has been used for years by the microwave industry to treat vias in microwave designs. With digital signaling approaching microwave frequencies, similar techniques can be employed to enhance the signal integrity of a link. Counterboring is performed as one of the final steps in the board manufacturing process. After the multilayer board is laminated, drilled, and plated, designated holes are control-depth drilled to remove any via stub that is present. This controlled-depth drill should allow a minimum length of barrel to remain in the hole to allow the eyeof-needle to engage the via. These minimum lengths Figure 6 Counterbored Via are given above. Figure 6 illustrates a counterbored via. 2. BLIND VIAS An alternative approach that is equally as effective as counterboring is the use of blind vias. Like counterboring, care must be taken to ensure that the depth of the blind via is sufficient to fully engage the eye-of-needle. These minimum depths are given. Figure 7 illustrates a blind via. Figure 7 Blind Via PAGE 9 September 21, 2006
IV. ROUTING Because the Advanced Mezzanine Card connector can be used for both horizontal as well as vertical routing of differential signals, the routing of both versions will be examined. Whether routing into or through the AMC connector pinfield, the general guidelines are the same. A. ROUTING CHANNELS A routing channel is defined by the space between adjacent vias in the connector pinfield. In the AMC connector, both vertical (between rows of vias) and horizontal (between columns of vias) routing can be achieved. Typical carrier card routing is implemented horizontally, as silicon devices and backplane connectors will reside in this direction relative to the footprint of the AMC connector. Figure 8 provides the general layout of an AdvancedTCA carrier card fully loaded with AMC plug-in modules. AMC Module AMC Connector Silicon Device ATCA Carrier Card Front Panel AMC Module AMC Module AMC Module AMC Connector AMC Connector AMC Connector Silicon Device Silicon Device HM-Zd Connectors to ATCA Backplane Figure 8: AdvancedTCA Carrier Card Example Layout Vertical routing is also possible, and may be required, especially for cases when signals from one AMC connector on a carrier card are required to route directly to a second AMC connector on the same carrier card. (The AdvancedTCA specification requires multiple AMC connectors on the same carrier card to be located with their footprints directly in-line with one another.) Vertical routing is recommended to occur between the signal rows of the connector, on either side of the central row of ground vias. Figure 9 illustrates horizontal and vertical routing techniques. PAGE 10 September 21, 2006
Horizontal Routing Vertical Routing Figure 9: Routing Configurations B. TRACE WIDTHS The maximum trace width that can be utilized in a routing channel is a function of the via pitch, the pad size, and the trace-to-pad clearance. If a D+10 pad size is utilized, the remaining space allows for 7 mil differential line widths with a 7 mil intra-pair space. 7 mil traces with 7 mil spaces can be easily routed through the footprint. However, due to the footprint hole layout and the orientation of the widest routing channel through the footprint, optimal trace routing needs to occur on angles other than 45-degree increments. This is a straightforward process for hand-routed designs, but can pose some difficulties for auto-routed designs, as auto-routers commonly have limitations of 45-degree increments for trace bends and turns. For optimal routing capability, and when taking advantage of general auto-router capabilities, trace widths and intra-pair spaces must be reduced to allow for 45-degree bends through the AMC connector footprint. Differential line widths of 4 mils and intrapair spaces of 4 mils provide for the 45-degree routing capability. The horizontal routing example of Figure 9 demonstrates the 4-4-4 routing technique and the ability to use 45- degree angles to route through the entire footprint. Table 3 illustrates the calculation of the maximum available routing channel. Metric English Vertical Via pitch 1.50 mm 0.059 Pad diameter (D+10) -0.75 mm -0.030 Trace-pad clearance (x 2) -0.10 mm -0.004-0.10 mm -0.004 Available routing channel 0.55 mm 0.022 Table 3: PCB Routing Channel Calculation PAGE 11 September 21, 2006
For trace width determination, it is also important to ensure that traces have adequate ground coverage underneath them at all times. When routing through the connector pinfield, this coverage can be improved by reducing the antipad size on connector vias. However, antipad reduction can result in reduced performance of the via at high speeds. Conversely, with a narrower differential geometry, the antipad size may be increased to improve performance of the via at high speeds. Please refer to section III.B.4 for antipad size recommendations. C. SKEW & PROPAGATION DELAY Typical right-angle connectors have differing lengths for the two component signals in a differential pair. In the right-angle AMC connector, the component signals within a differential pair have been length matched to each other, such that the differential skew within a pair is negligible. In order to have a zero-skew system, length compensating within a pair should be implemented in the differential routing. For current skew values for the AMC connector, refer to documentation and models at http://www.tycoelectronics.com/documentation/electrical-models V. PART PLACEMENT Part placement and spacing guidelines as well as associated up-to-date mechanical dimensions should be obtained in addition to this document. Placement related information is contained within the application specification, document #114-13181. The full mechanical dimensioning and tolerances are available for all versions of the AMC connector within the customer drawing for the specific part number of interest. All of this information can be found at www.tycoelectronics.com, and also by contacting either your local Tyco Electronics sales support or the appropriate contact listed below. VI. ADDITIONAL INFORMATION A. GIGABIT RESEARCH AND GENERAL APPLICATION NOTES More information regarding Tyco Electronics research into the transmission of electrical signals at gigabit speeds or general application notes are available for download from the Internet at http://www.tycoelectronics.com/documentation/electrical-models. B. ELECTRICAL MODELS Electrical SPICE and S-parameter models for the AMC connector may be requested at modeling@tycoelectronics.com. PAGE 12 September 21, 2006
VII. CONTACT INFORMATION The following key contacts can be used to obtain additional information on the AMC connector product family. Technical Support Center 1-800-522-6752 www.tycoelectronics.com/help Tim Minnick, (717) 986-5284 tim.minnick@tycoelectronics.com Signal Integrity Engineer Dave Szczesny, (717) 985-2844 dave.szczesny@tycoelectronics.com Mechanical Dev. Engineer John Larkin, Product Manager (717) 592-2074 jtlarkin@tycoelectronics.com PAGE 13 September 21, 2006