Comparing design data requirements to design resources can result in better electronic performance at a reduced cost.
Proper design of high-speed, analog PCBs can make and break system electrical performance. Complex physical and electrical designs, densely packed boards and faster signal requirements are examples of factors that add complexity to today’s PCB designs. Consequently, designers should be able to easily define, manage, evaluate and validate physical and spacing constraints that apply to critical, high-speed signals. This should be done during the early stages of the design process. At the same time, the designer must ensure that the final layout design meets performance, manufacturing and test specification goals.
A density-predicting calculator is a tool that performs a tradeoff analysis at the feasibility stage, given the constraints of the assigned area. It takes into account the available CAD data analyses, including the electrical schematics, during the early stages of PCB design and layout. These initial data include the number of components, and the type and characteristics of the components once selected. The number of connections is also available, based on the interconnections and busses.
To make effective use of a density-predicting tool, several parameters should be made known prior to the feasibility analysis run:
- The measurement units, imperial or metric, and their impact on the trace/space width at the routing phase. Also important at this stage is understanding the metric structure of the current BGA and µBGA components relative to the via holes going through those components.
- The trace width, which is dictated by current flow level and maximum tolerable temperature rise.
- Component placement strategy, which impacts electrical performance. The designer should keep in mind the board’s electrical flow throughout the entire design phase.
For high-speed, high-frequency design, analyze the trace’s controlled impedance because the trace is now considered a transmission line.
The board technology and the stackup structure; for example, the PCB thickness and the number of signal and non-signal layers. Also, HDI technology, if used, needed to complete the PCB layout routing.
Calculator algorithm. A board’s density can be measured by several methods. One method is based on the number of connections per square inch, with any amount between 65 and 120 connections considered dense. Other methods include the number of components per square inch or the pad count per square inch.
For example, consider two board layouts (Figure 1) for the same product, designed in 1990 and 2000, respectively. The board designed in 2000 has more functions compared with the one from 1990, and it is denser in terms of the number of layers, line/space density and assembly density (Table 1).
For the same product, the newer board is denser, while using a smaller area and fewer layers. The user can define a maximal density factor for a number of PCBs in a given product, and boards would have the same or lower density factor. Obviously, this definition can change as the technology progresses and new design rules are implemented.
To gain confidence in the feasibility of the board design, we define the following terms used as inputs:
- Demand is all available design data requirements.
- Capacity is all available design resources.
Given these two values, we can run the program to get the density result defined as the ratio of demand to capacity.
For the demand part of the equation, we enter all known CAD design data (Figure 2). Usually these data are available once the design is completed. Mechanical design established the board size and its outline structure. After importing the mechanical data into the CAD design workdesk, the available area will be expressed either in terms of square inches or square millimeters.
Design technology is a key parameter in the prediction calculator. Many high-speed designs have electrical signal constraints such as controlled impedance signals, differential signals, fast clocks and tuning requirements. The electrical designer knows most of these data. The program calculates the wiring demand, as shown in the bottom of the dialogue box. The higher the number, the more complex the board. As a rule of thumb, if the wiring demand number exceeds the value of 80, one should consider using HDI.
In the capacity dialogue box (Figure 3), we enter initial concepts such as BGA pitch, typical trace width, typical via hole, number of signal layers expected and type of design. There is always a limit on the amount of routing each board can accommodate. The main contributors include:
- Pitch/distance between vias or holes in the substrate.
- Number of wires that can be routed between vias.
- Number of signal layers required.
- Design type.
- Design versatility.
As a result of the calculation, the wiring capacity appears at the bottom of the dialogue box. Again, the higher the number, the more complex the board.
‘What-if’ analysis. If the capacity value is higher than the demand value, the chosen design rules and technology are sufficient, and cost reduction may be an option. If the capacity value is equal to the demand value, the chosen design rules and technology are sufficient; however, either some effort may be required to finish the layout, a compromise on the constraints will be required during the design, or future changes will be difficult to implement. Finally, if the demand value is higher than the capacity value, the chosen design rules and technology are insufficient, and a set of checkups should take place. These can include the available layout area, the technology used for PCB manufacturing and the layer count. Figures 4 and 5 show comparisons between demand and capacity data.
Since electronic designs are now done with CAD tools, smooth integration is available between the schematic and the layout. All the schematic symbols, pins, connections and constraints are imported to the PCB layout tool in the netlist.
The netlist file brings the schematic and the PCB database together. The embedded data include all available design resources that fit into the definition of capacity of the specific PCB layout. Second, all requirements for that specific design are known as the demand. The demand data include:
- Number of components.
- Number of connections.
- Available area.
- Design type.
The capacity data include:
- Parts pin definitions (pads sizes and pitch, in mm).
- Specific connection names (differential, controlled impedance, power, RF, analog).
- PCB route directives (stripline, microstrip, trace/space width, vias).
- PCB stackup and technology (HDI, number of signal layers, number of plane layers).
- The result of the capacity/demand ratio provides a relative number for the density.
Organizations that have a PCB database information center can standardize their boards to a relative board density factor and keep track of board manufacturability and performance by comparing the density factor data to achieve better electrical performance and PCB cost reduction. PCD&F
This work was funded by Elbit System; Israel.
Ed.: This article is adapted from a presentation at IPC Apex 2009 and is reprinted with the authors’ permission.