Estimated reading time: 10 minutes

Beyond Design: Interactive Placement and Routing Strategies

This article originally appeared in the December 2012 issue of The PCB Design Magazine.

PCB layout is a means to combine your artistic side and your creative skills with the power of automation. I always say that if a PCB design looks good, it will probably work well. However, neatness in routing often leads to unwanted crosstalk as trace segments are routed in parallel for long distances.

Back in the late 1970s, I used Bishop Graphics tape and stick-on pads to create PCB artwork, such as it was. Artwork is still an appropriate name for PCB layout because of the artistic qualities required. Good routing requires the PCB designer to have exceptional 3D spatial skills, a thorough and methodical approach, and a keen eye for detail—and all of the above combined with style.

Interactive Placement

To obtain a high route-completion rate, component placement is extremely important. If the board is difficult to route, it may just be the result of poor placement, slots/gates positioned all over the board, or perhaps the sequence of pins on components are flipped. We need to help the router as much as possible by opening route channels and providing space for vias.

Interactive placement is best done by cross-probing and dragging the components one-by-one from the schematic to place on the PCB—taking functionality and design constraints into account.

During placement, consideration should not only be given to routing, but also to inspection and rework. An 80 mil minimum clearance is required for rework tools, and an angle of 60 degrees for visual inspection. However, where possible, 45 degrees (i.e., spacing between components = height of tallest component) is a good rule of thumb.

Figure 1: Space = height of tallest component.

In other words, if a tall electrolytic capacitor is next to a BGA, then the height of the electrolytic is the distance required between components. Along these lines, grouping large, plated, through-hole components together saves board space.

Similar types of components should be aligned on the board in the same orientation for ease of component placement, identification, inspection, and testing. A placement grid of 100 mils is recommended for large components and 25 mils for chip components. Also, similar component types should be grouped together whenever possible, with the net list or connectivity and circuit performance requirements ultimately driving the placements. In memory boards, for example, all of the memory chips are placed in a clearly defined matrix with pin 1 orientation in the same direction for all components. This is a good design practice to carry out on logic designs where there are many similar component types with different logic functions in each package.

On the other hand, analog designs often require a large variety of component types, making it understandably difficult to group similar components together. Regardless of whether the design involves memory, general logic, or analog components, it’s advisable to orient pin 1 on all IC components the same, provided that product performance or function is not compromised in the process.

One issue that is always a problem—especially as trace widths and clearance decrease—is the lack of via space. With high-speed design, traces from a BGA fan-out straight to an internal layer to prevent radiation, and this of course requires a via for each BGA ball. This cannot be avoided. But we can open up space for vias on other surface mount devices (SMDs) when using double-sided placement. Figure 2 Illustrates two PLCCs placed on the top of a board with resistor packs on the bottom side. If the lands on the bottom are aligned with the lands on the top, space is cleared for vias and horizontal routing channels are opened. This is not the case when using blind vias, but certainly helps with through-board vias.

Figure 2: Lands are aligned top and bottom to open up space for vias.

A comment regarding autoplacement: One of the most useless features that all EDA layout tools offer is autoplacement. I guess they all have this feature because some bright guy decided to include this in his tools and it then became a checkbox for product comparisons—so everyone has to have it.

Notwithstanding the uselessness for autoplacement’s intended purpose, I have found a good use for it—to see if all the components will fit inside the board outline before stating placement. If not, then you can re-evaluate the packaging or reduce functionality to fit the required space.

Cross-Probing

Cross-probing, between the schematic and PCB, provides a valuable mechanism for design, review, verification and testing of PCBs, but it is most powerful during interactive placement and routing. Cross-probing is bi-directional, in that you can select parts or nets on the schematic and highlight and identify them on the PCB database, or vice-versa. This feature also gives you the ability to drive the router directly from the schematic design. Figure 3 illustrates a schematic to PCB cross-probe of a component.

Figure 3: Cross-probing between schematic and PCB.

Cross-probing can also be used as a powerful search tool—locating parts and nets on the schematic or PCB. And, cross-probing is not limited to schematic and PCB. AutoVue, for instance, allows the cross-probing between PCB and 3D MCAD tools, enhancing mechanical visualization of the product.

When an engineer creates the schematic he invokes a logical process, typically, grouping components into blocks or sheets that functionally go together. When the PCB designer then places these components, he should also use a logical, sequential process by placing functional components near each other, optimizing trace cross-overs and lengths, keeping constraints in mind.

In years past, I recall having to place components by select list. This seemed logical but the PCB designer was never to know whether they were placing a trivial static pull-up resistor or a critical terminator. Resistors are just resistors—unless you know what they do. This is the beauty of cross-probing. The functionality of the circuit is displayed and each and every component can be placed by functionality and importance—providing error-free transfer of the intended schematic functionality to the design.

Of course, design rules can also be added to the schematic to pass this information on to the PCB designer, but a picture is worth a thousand words.

Interactive Routing

Proper component placement is an important aspect of routing. If the board is difficult to route, it may just be the result of poor placement. So before you start routing, it is important to check the placement and design rules to ensure that there are no issues that may prevent the route completion. The easiest way to check this is to turn the autorouter loose and see how it goes. If you do not get at least 85% completion on this first test route, then you may need to tweak the placement, look at more appropriate packaging, adjust the design rules, and possibly drop some functionality to improve routability.

However, there are some important things to do before you commence with the process of formally routing the board:

1. The stackup should be planned to ensure that controlled impedance signals have been calculated correctly and that the return current for each signal layer has a clear return path. The ICD Stackup Planner can be used to analyze the stackup (download from www.icd.com.au), and help you with material selection, along with input from your fabricator. The resulting stackup configuration should then be transferred to the design rules to define the correct trace width and clearance for each layer, and to specify the differential pairs.
2. The power distribution network (PDN) should be planned, and bypass and decoupling capacitors placed in the appropriate positions. The ICD PDN Planner is an ideal sandbox for analyzing this. It is a good idea to color the power nets with individual colors so that they can easily be recognized without having to name the net. Altium has a great feature, which displays the net name for each net, making identification of power nets extremely clear.
3. Design rules and constraints can be passed from the schematic, which automatically sets the design rules in the PCB database—though there is always some adjustment to be done on the PCB side. Via sizes for different net classes need to be defined. This is important for route completion. (Please see my previous article on PCB Design Techniques for DDR, DDR2 & DDR3, Part 1 and Part 2 for a complete list of the appropriate design rules for DDR2 routing.)  For rules to properly support the design process, they need to be defined in the correct priority so that the most important rules prevail over rules of lesser importance.
4. Set up the routing options. It amazes me that all the EDA tools that I have used do not come with the router set to the most useful functions straight out of the box. So before routing, one must tweak the route options to get the tool to do what you want. Details vary by tool, of course, but the nuisance is near-universal.

Once we have the above set, then it is time to start interactive routing. The real power of cross-probing is driving the router from the schematic. Starting with the most critical nets, cross-probe in the following sequence:

1. Select the components on the schematic and fan-out on the PCB selecting the appropriate pattern. Adjust the fan-out as necessary. The rules should be set such that power traces are routed thick (10 - 20 mils) to reduce inductance. And, each GND and VCC should have its own individual via to the plane—avoid connecting two or more GND’s to the one via.
2. Obviously, matched length, differential pair and critical signals that have specific requirements should be routed first. Fix or lock these traces so they cannot be inadvertently moved.
3. Select the most critical nets, a few at a time, on the schematic and route in the PCB. Adjust the routing as necessary then move on to the next group of nets and so on. In this way you can build up an excellent route in a short time and it is all controlled from the schematic. Feel free to jump in and tweak the routing to your liking.

Once the routing is complete, apart from running design rule checks (DRCs), I like to run a sanity check on the board. I can either do this in the simulation environment or in the PCB database. Simply highlight each net one by one—it is tedious, but gets results. You can quickly see if there are any nets that are longer than the Manhattan length or spiral around the board three times before termination.

Points to Remember:

• Component placement is an important aspect of routing. If the board is difficult to route, it may just be the result of poor placement.
• Components should be placed in functional blocks.
• An 80-mils minimum clearance is required for rework tools, and an angle of 60 degrees for visual inspection. A good rule of thumb: Spacing between components = height of tallest component.
• Similar types of components should be aligned on the board in the same orientation. A placement grid of 100 mils is recommended for large components, and 25 mils for chip components.
• Align lands on the bottom with the lands on the top to open up space for vias.
• Check the stackup, PDN, design rules and routing parameters before interactive routing.
• Run a test autoroute, targeting at least 85% completion.
• Cross-probing, between the schematic and PCB, provides a valuable mechanism for design, review, verification and testing of PCBs, but it is most powerful during interactive placement and routing.
• Cross-probing can also be used as a powerful search tool.
• The real power of cross-probing is driving the router from the schematic. Start with the most critical nets—then continue to lower-priority nets.
• Finally, run a sanity check on the board. Simply highlight each net one by one. You can quickly see if there are any nets that are longer than the Manhattan length.

References

• Advanced Design for SMT—Barry Olney
• Beyond Design: Intro to Board-Level Simulation and the PCB Design Process—Barry Olney
• PCB Design Techniques for DDR, DDR2 & DDR3, Part 1 & 2—Barry Olney
• The ICD Stackup and PDN Planner can be downloaded from www.icd.com.au

Barry Olney is managing director of In-Circuit Design Pty Ltd (ICD), Australia. ICD is a PCB design service bureau specializing in board-level simulation. The company developed the ICD Stackup Planner and ICD PDN Planner software.