Schematic and PCB Design Process March 7, 2008
Question:
I would like to know how a circuit designer in OrCAD plans the schematic and layout for the digital, analog, power, low speed high speed portion of the PCBs?
Answer:
Wow, this is a big but good question! For anyone considering undertaking a schematic capture and PCB layout for the first time, it can seem like a daunting task. A modern PCB serves not just as a means to interconnect components, but also as a mechanical structure, heat conductor, noise shield, and even as a circuit element, and must go through a complex automated manufacturing process to boot.
Perhaps it is best to start with a simple project to get your feet wet! Aside from that, it also helps to have some background knowledge about how electronic stuff works. Typically, at least a two year degree in electronics is recommended for anyone serious about PCB layout as a career. I can’t describe the whole process - that would take a book. What I can do is briefly touch on some of the basics to help you get started or even decide if PCB layout is something you really want to do.
Assuming you have a circuit design already and you just need to capture the schematic in OrCAD (or a similar tool) and do a PCB layout, I can propose some basic guidelines for how to approach it. As you mentioned, the design is partitioned into logical blocks like digital, analog, power, high speed, etc. It is good to keep the schematic and PCB layout also partitioned in this way. This will allow you to focus on the specific critical aspects of each type of circuitry throughout the process and avoid getting everything all tangled up.
If you are working on a medium to large scale project, there is generally a project team, so it couldn’t hurt to ask the Electrical and Mechanical Engineers who designed the thing and the Manufacturing Engineer who will build the thing and the Test Engineer who will test the thing what their design requirements are. The best way to do this is to have a PCB design kick-off meeting. Other team members may include the Customer, Quality, Reliability, Purchasing, Planning, and Safety representatives. As you go along, have the team sign-off at critical points.
Before drawing anything, start by reading the data sheets and application notes of any critical components to see what the recommendations are for PCB layout. A little bit of research up front can save a lot of time down the road!
Next, it is great to start by drawing a block diagram to use as a guide along the way. Ideally, the block diagram should be part of a hierarchical schematic that drives the design, but it can also be a separate sketch. It should have a logical flow e.g. from left-to-right and top-to-bottom. It should be the type of thing that can be used to show people how the thing works and updated as the project moves along.
Now you are ready to fire up OrCAD or whatever design tools you are going to use.
Draw any new schematic symbols needed
� To save time, first check for built in libraries or ones from part vendors or user groups
� Rather than start from scratch, modify an existing library part when possible
� Use a left-to-right and top-to-bottom flow of signals on the symbols
� Typically you place power pins on top and GND on bottom
� Double check all the symbols for correct pins! A mistake here can make a lot of mistakes in the PCB times the number of PCBs - You don’t want to go there.
Capture each section of the circuit into the schematic
� Again, use a left-to-right and top-to-bottom flow of signals on the schematic
� Each block can be on a page
� Draw critical circuitry like you want it to be laid out on the PCB (i.e. short lines where you want short traces etc.)
� Note any special design rules like length limits, required widths, or controlled impedances
� Name signals in a way that makes it easy to understand the schematic
� Add test points to critical signals (and lots of GND test points)
� Double check schematic against design source with a highlighter etc.
� Get approval from team
Draw any required new PCB footprints and pad stacks
� To save time, first check for built in libraries or ones from part vendors or user groups
� Follow vendor guidelines if available, else use industry standards
� Consult with the manufacturing engineer about process specific requirements
Proceeding to PCB Layout
� Draw board outline with critical cut-outs, mounting holes, and keep outs
� Sketch “rooms” corresponding to each block onto the board outline
� Decide on number of layers, copper thickness, and board stack-up arrangement. This is a function of board density, the sheer number of signals and power planes needed, the controlled impedance scheme, heat conduction requirements, etc.
� Consider routing adjacent signal layers with horizontal / vertical routes to obtain perpendicular overlap. This reduces cross talk and eases routing.
� Place critical components and get approval on the initial placement from the team
� Route critical traces and planes, and then route the rest
� Do a clean up pass to fix any odd things, improve silk screen, etc.
Here are some bullets to keep in mind when doing PCB layout for each type of circuit:
Low Speed Digital
� Not very susceptible to noise
� Generates a medium amount of noise, so keep it away from the most noise sensitive circuits
� The most active signals are the most noisy
� Other than that, layout is not too critical and this can be placed around the board as kind of a “filler” in places where nothing else will want to go and can be easily auto-routed.
High Speed Digital
� Same as low speed digital, plus the following:
� There can be a very high number of interconnecting traces
� Generally uses controlled impedance traces
� Requires controlled, minimized, or matched signal delay times and proper location of termination devices
� Can generate some serious heat - added copper planes to conduct heat away and heat sinks will need to be designed in
Analog
� Usually very sensitive to noise pickup
� Keep away from noise generators
� High impedance nodes and nodes followed by a lot of gain are generally most sensitive to noise
� Look for recommended grounding and shielding in application notes
� May also be sensitive to surface leakage currents, temperature, etc
� Power amplifiers may generate significant heat - added copper planes to conduct heat away and heat sinks will need to be designed in
Power
� Can generate a lot of noise (esp. switching power supplies, class D amplifiers, etc)
� At the same time, some nets are very sensitive to noise (i.e. sense and feedback nets)
� Can generate a lot of heat - added copper planes to conduct heat away and heat sinks will need to be designed in
� Switching nodes are sensitive to layout parasitic inductance and capacitance
� Keep high AC currents confined to small loop areas to reduce noise
� May involve high voltage and safety issues, special spacing and insulation requirements
RF
� Uses controlled impedance traces
� May require traces to be designed as antennas (requires RF design background)
� Receivers are very sensitive to noise
� Transmitters generate noise and dissipate heat proportional to the power involved
� Again, added copper planes to conduct heat away and heat sinks will need to be designed in
� Requires special attention to shielding and grounding
- Posted in : Uncategorized
- Author : Brad
Comments»
I highly appreciate the issues discussed in the answer. Being a hardware designer, I would like to add some comments.
Before I start working on a project, I ask myself:
It may seem absurd, but it is a fact; more often than not, I need to add some extra circuitry to meet standards (in particular, EMI/RFI norms). One must make provision for adding things like decoupling caps if required. Well, you can anticipate the decoupling requirements but not everyone is good at it.
Once you have the schematic ready, make sure you do an ERC (electrical rule check). It tells you about missing connections, wrong connections.
Next, take a copy of the bill of material and spend some time on each of the component regarding its dimensions. You might have a liking for specific unit (mils or mm.). Choose on one and stick to it. Unit conversions done in a time of emergency usually lead to mistakes like one side of a PQFP misaligned with pads. Most of the manufacturers provide mechanical drawings for the packages and footprint libraries. Spend time on them. It will help you a lot.
The best way to check the dimensions is to take a printout of the footprint you are going to use for a particular component in 1:1 scale, place the component on it and check whether you have enough space on pad for soldering.
I will stop here. As Brad said, a book will be required to explain all intricacies.
Thanks Ravi. Your comments ring true.
Can anyone recommend a good book to learn board layout rules and design guidelines? I understand basic electronics and have some experience with OrCAD Capture and drawing schematics, but am starting to learn OrCAD Layout and board design and would appreciate a good reference.
Jody,
Please see:
http://astore.amazon.com/summit2v1-20
Make part outlines for PCB as accurate as possible so actual parts will fit. I use mfr’s dimensions, calipers and a rather large amount of time, but it pays off. I use 3 layers just for the outline - one for the “silkscreen” on the actual board, one for additional details that appear on an assembly diagram, and one for hints for use when doing placement, etc. Extra layers can be useful for prints for panel holes, etc. Silkscreen outlines for SMD’s are of little real use in many cases. I typically just use a dot or line between pads for passives, as an aid to manual assembly of proto’s. Assembly machines don’t need outlines and ink on pads is bad! Put useful outlines on paper prints.
For schematics that require multiple pages, I usually use 3-digit component ref numbers, where the 1st digit matches the page number of the schematic and the 2nd is associated with a functional block on that page. For example, R321 to R329 would be on pg3 of the schematic and associated with the voltage error amp. This approach is quite helpful for anyone who has to understand and/or troubleshoot the circuitry. It isn’t always workable, and there are exceptions, as when sections of an IC are used in different functional blocks.
In general, don’t let the CAD software number your components for you. It is fast, but often VERY messy, and results in “adjacent numbers” that are not “functionally adjacent”.
outta space
On testpoints:
For lots of circuits, scope probe gound leads are unworkable, unless you are using active probes. Probe tip grounds are vastly better, but a real pain because of their tendency to slip, with possibly disastrous consequences. Small vias to ground, placed strategically, can be very helpful as “anchors” for tip grounders. Simply putting small dots on the solder mask layer (to make small voids in the solder mask) can make useful access points to surface ground planes. Where vias are unworkable, making an indent in these access points (with a sewing needle or the like) can reduce tip grounder slipping.
If you have never had to use probe tip gounds (because you KNOW you don’t need to), consider yourself lucky!
Since parts come in an ever increasing variety of packages, with new ones coming out weekly, I suggest evaluating the ease of creating parts in a schematic capture and PCB layout program. The easier & more intuative it is to make parts (symbols & pads), the more productive and less frustrated you will be. Today many new ICs are in leadless packages (i.e. QFN) and bumped chips (the actual silicon with solder bumps) which range in size from 8×8 mm square to way less than 2×2mm square. Many are not square or the “pins” are not symmetrical. Many also have one or more “heat transfer pads” in the middle, in varying sizes and shapes. To make the parts in a PCB layout package (according to the mfgs dimensions) you’ll also have to consider the physical size and space around the part for inspection and probing. The Standard libraries supplied or sold are almost worthless, since they are mostly old DIP parts and companies that don’t exist. Many libraries also include user generated parts, oftem with many problems. Make your own!
As for generating the schematic symbols, many parts now have multiple connections which are connected to the same circuit point. Even simple connectors such as a SMT DC Jack have this feature. So if you intend to use the built in error checking and netlist to veryfy your schematic is properly connected to your PCB (which you should), you need to make sure that the shematic symbol contains enough pins for redundant connections and heat transfer pads.
—cont’d from above—
I have used many PCB programs since 1987, including several full versions each of: ORCAD, Tagngo, Accel, Schema, PADS, P-Cad, Eagle, and many other lesser known programs.
For starting in PCB design, I might suggest a free program called PCB123. It now includes schematic capture and has many features of the “professional” programs (the $10,000 kind). For the last several years my favorite program is EasyPC by Number One Systems in the UK. It’s easy to make parts, highly functional, easy to use and not very expensive.
Hi Imre,
Thanks for the good words from your experience. I have been meaning to try the new PCB123 s/w. They also have some good tutorials in the download area. It should be noted that their free software is pretty much going to force you to purchase your first set of PCBs from PCB123 and then pay to get the gerber files. I still think it is a great thing.