Pneumatic Grids
The second major rule of PCB design, and the one most often missed by beginners, is to lay out your board on a
fixed grid. This is called a “snap grid”, as your cursor, components and tracks will “snap” into fixed grid positions.
Not just any size grid mind you, but a fairly coarse one. 100 thou is a standard placement grid for very basic
through hole work, with 50 thou being a standard for general tracking work, like running tracks between throughhole
pads. For even finer work you may use a 25 thou snap grid or even lower. Many designers will argue over
the merits of a 20 thou grid vs a 25 thou grid for instance. In practice, 25 thou is often more useful as it allows
you to go exactly half way between 50 thou spaced pads.
Why is a coarse snap grid so important? It’s important because it will keep your components neat and
symmetrical; aesthetically pleasing if you may. It’s not just for aesthetics though - it makes future editing,
dragging, movement and alignment of your tracks, components and blocks of components easier as your layout
grows in size and complexity.
A bad and amateurish PCB design is instantly recognisable, as many of the tracks will not line up exactly in the
center of pads. Little bits of tracks will be “tacked” on to fill in gaps etc. This is the result of not using a snap grid
effectively.
Good PCB layout practice would involve you starting out with a coarse grid like 50 thou and using a progressively
finer snap grid if your design becomes “tight” on space. Drop to 25 thou and 10 thou for finer routing and
placement when needed. This will do 99% of boards. Make sure the finer grid you choose is a nice even division
of your standard 100 thou. This means 50, 25, 20, 10, or 5 thou. Don’t use anything else, you’ll regret it.
A good PCB package will have hotkeys or programmable macro keys to help you switch between different snap
grid sizes instantly, as you will need to do this often.
There are two types of grids in a PCB drafting package, a snap grid as discussed, and a “visible” grid. The visible
grid is an optional on-screen grid of solid or dashed lines, or dots. This is displayed as a background behind your
design and helps you greatly in lining up components and tracks. You can have the snap grid and visible grid set
to different units (metric or imperial), and this is often very helpful. Many designers prefer a 100 thou visible grid
and rarely vary from that.
Some programs also have what is called an “Electrical” grid. This grid is not visible, but it makes your cursor
“snap” onto the center of electrical objects like tracks and pads, when your cursor gets close enough. This is
extremely useful for manual routing, editing and moving objects.
One last type of grid is the “Component” grid. This works the same as the snap grid, but it’s for component
movement only. This allows you to align components up to a different grid. Make sure you make it a multiple of
your Snap grid.
When you start laying out your first board, snap grids can feel a bit “funny”, with your cursor only being able to
be moved in steps. Unlike normal paint type packages which everyone is familiar with. But it’s easy to get used
to, and your PCB designs will be one step closer to being neat and professional.
There is no recommended standard for track sizes. What size track you use will depend upon (in order of
importance) the electrical requirements of the design, the routing space and clearance you have available, and
your own personal preference. Every design will have a different set of electrical requirements which can vary
between tracks on the board. All but basic non-critical designs will require a mixture of track sizes. As a general
rule though, the bigger the track width, the better. Bigger tracks have lower DC resistance, lower inductance, can
be easier and cheaper for the manufacturer to etch, and are easier to inspect and rework.
The lower limit of your track width will depend upon the “track/space” resolution that your PCB manufacturer is
capable of. For example, a manufacturer may quote a 10/8 track/space figure. This means that tracks can be no
less than 10 thou wide, and the spacing between tracks (or pads, or any part of the copper) can be no less than
8 thou. The figures are almost always quoted in thou’s, with track width first and then spacing.
Real world typical figures are 10/10 and 8/8 for basic boards. The IPC standard recommends 4thou as being a
lower limit. Once you get to 6thou tracks and below though, you are getting into the serious end of the business,
and you should be consulting your board manufacturer first. The lower the track/space figure, the greater care
the manufacturer has to take when aligning and etching the board. They will pass this cost onto you, so make
sure that you don’t go any lower than you need to. As a guide, with “home made” PCB manufacturing processes
like laser printed transparencies and pre-coated photo resist boards, it is possible to easily get 10/10 and even
8/8 spacing.
Just because a manufacturer can achieve a certain track/spacing, it is no reason to “push the limits” with your
design. Use as big a track/spacing as possible unless your design parameters call for something smaller.
As a start, you may like to use say 25 thou for signal tracks, 50 thou for power and ground tracks, and 10-15
thou for going between IC and component pads. Some designers though like the “look” of smaller signal tracks
like 10 or 15 thou, while others like all of their tracks to be big and “chunky”. Good design practice is to keep
tracks as big as possible, and then to change to a thinner track only when required to meet clearance
requirements.
Changing your track from large to small and then back to large again is known as
“necking”, or “necking down”. This is often required when you have to go between IC
or component pads. This allows you to have nice big low impedance tracks, but still
have the flexibility to route between tight spots.
In practice, your track width will be dictated by the current flowing through it, and the maximum temperature rise
of the track you are willing to tolerate. Remember that every track will have a certain amount of resistance, so
the track will dissipate heat just like a resistor. The wider the track the lower the resistance. The thickness of the
copper on your PCB will also play a part, as will any solder coating finish.
The thickness of the copper on the PCB is nominally specified in ounces per square foot, with 1oz copper being
the most common. You can order other thicknesses like 0.5oz, 2oz and 4oz. The thicker copper layers are
useful for high current, high reliability designs.
The calculations to figure out a required track width based on the current and the maximum temperature rise are
a little complex. They can also be quite inaccurate, as the standard is based on a set of non-linear graphs based
on measured data from around half a century ago. These are still reproduced in the IPC standard.
A handy track width calculator program can be found at www.ultracad.com/calc.htm, and gives results based on
the IPC graphs.
As a rule of thumb, a 10degC temperature rise in your track is a nice safe limit to design around. A handy
reference table has been included in this article to give you a list of track widths vs current for a 10degC rise. The
DC resistance in milli ohms per inch is also shown. Of course, the bigger the track the better, so don’t just
blindly stick to the table.
Pads
Pad sizes, shapes and dimensions will depend not only upon the component you are using, but also the
manufacturing process used to assemble the board, among other things. There are a whole slew of standards
and theories behind pad sizes and layouts, and this will be explained later. Suffice it to say at this stage that
your PCB package should come with a set of basic component libraries that will get you started. For all but the
simplest boards though, you’ll have to modify these basic components to suit your purpose. Over time you will
build up your own library of components suitable for various requirements.
There is an important parameter known as the pad/hole ratio. This is the ratio of the pad size to the hole size.
Each manufacturer will have their own minimum specification for this. As a simple rule of thumb, the pad should
be at least 1.8 times the diameter of the hole, or at least 0.5mm larger. This is to allow for alignment tolerances
on the drill and the artwork on top and bottom layers. This ratio gets more important the smaller the pad and hole
become, and is particularly relevant to vias.
There are some common practices used when it comes to generic component pads. Pads for leaded
components like resistors, capacitors and diodes should be round, with around 70 thou diameter being common.
Dual In Line (DIL) components like IC’s are better suited with oval shaped pads (60 thou high by 90-100 thou
wide is common). Pin 1 of the chip sould always be a different pad shape, usually rectangular, and with the
same dimensions as the other pins.
Most surface mount components use rectangular pads, although surface mount SO package ICs should use oval
pads. Again, with pin 1 being rectangular.
Other components that rely on pin numbering, like connectors and SIP resistor packs, should also follow the
“rectangular pin 1” rule.
No comments:
Post a Comment