- A GUIDELINE ON PRINTED
CIRCUIT BOARD DESIGN
YEAR 3 AND 4 ENGINEERING STUDENTS
UNIVERSITY of AUCKLAND
DEPARTMENT of ELECTRICAL AND ELECTRONIC
BY FRED NASSENSTEIN DEC 1992
UPDATED MAR 1995
UPDATED DEC 1996 BY SLAVEK PRZEPIORSKI
Open Protel list
- THE COMPLETE PROCESS OF CIRCUIT DESIGN
1. SCHEMATIC DESIGN ------------
2. PCB DESIGN------------------------- ---------
3. ARTWORK PLOT------------------
4. MASK (NEGATIVE)
5. BOARD EXPOSURE----------------
- PHOTORESITS REMOVAL-----
8. BOARD ASSEMBLING
Process 2 to 6 are briefly mentioned in this guideline . The work involved with process
4 to 6 is usually carried out by a technician in this department.
1. - Introduction
2. - Chemical Process
3. - Computer Aided Design
4. - Using PROTEL-PCB
5. - Example
6. - Appendix
7. - Library Parts
Having gone through the process and struggle to design an electronic circuit,
which should result in the form of a circuit diagram, you have reached the stage
of needing to create your circuit at a physical level. Printed circuit board design
could be difficult as well, since you may include mistakes from your circuit
diagram and possibly create some more with this procedure (unless you are very
careful). But relax creating a PCB could (hopefully) be a nice expression of your
technical capabilities as well as an expression of your artistic skills.
A PCB is the most common, practical, reliable and low cost (in particular for
larger quantities) solution to assemble a cluster of electronics components (see #1
other techniques). The aim of PCB design is to physically place and interconnect
(using conductive tracks acting as wires) electronic components on an insulating
material according to the plans in the circuit diagram (or schematic).
In practice we do not actually print the physical circuit on a board, this is usually
achieved by means of a photographic and chemical process (see #2 for other
The board is usually made of a glass fibre strengthened epoxy based material
(sheet) with good electrical and mechanical properties (ie.: good insulator and
high mechanical strength).
The epoxy board is covered with a very thin copper layer either on one (single
sided boards) or on both sides (double sided boards) which we have to configure
in such a way so that the copper can be used as individual conductors (see #3 for
multi layers). This is usually achieved with the aid of an additional UV light
sensitive photo resist (plastic film) attached to the surface of the copper layer (see
By exposing the photo resist with Ultra Violet
light the resist will stabilise and
remain unstabilized for the areas not exposed.
With the use of a developing process (similar
to normal film processing) we are then able to
remove the unexposed photo resist areas
leaving the exposed areas which will act as a
protective film for the etching process.
By placing this board into an etching
solution (acid) we are able to etch (remove). Finally with the aid of a solvent we have to
remove the photo resist so that the copper can be soldered on to. Usually the copper
surface will be roller tinned or sprayed with a solder lacquer to improve the soldering
and to avoid corrosion.
It is obvious that with the above described process we are able to create any
shape of a conductive structure and thus electrical connections on an insulating
- material. To obtain the desired structure necessary for our circuit design however
we need to generate a MASK or NEGATIVE (black on transparent film) which
we have to place between our film coated board and the UV light exposure unit.
COMPUTER AIDED DESIGN (CAD)
In the Electrical and Electronics Engineering Department there are several PCB
software packages available on the network able to produce the artwork for such
a mask. In this session however I will only outline the use of PROTEL-
WINDOWS since it is easy to use and performs very well for most designs.
At present we use the above software to create a PLOT ARTWORK FILE in
Postcript format which can be send to an outside firm (ie.:BTL Technologies).
This company is able to produce a high resolution negative film necessary for the
final MASK and manufacturing process of the PCB (see #4 for other
techniques). Before going further in to detail in how to use the PCB software,
you should consider the following:
1- KEEP THE TRACK LENGTH SHORT AND WIDE
The copper layer on the PCB is very thin (30 um) this means that a certain
length of track between two points does not have zero resistance or zero
inductance!! This is not necessarily a problem since most signals will carry
low currents any way, however for very fast and high current signals,
especially power supply tracks, this could cause some problems. Therefore
keep the track length short (especially analogue input signals) and, in
particular for all the power supply connections, as wide as possible (#5).
2- USE DECOUPLING CAPACITORS ON EACH IC SUPPLY
Because of the above reasons it is near to impossible to supply each individual
IC with an ideal (zero impedance) voltage supply especially at high
frequencies. This can cause problems since switching currents will induce
noise in the supply voltage and disturb the function of the circuit. It is
therefore recommended to use decoupling capacitors between the supply pins
(as near as possible to the pins and for every individual IC (#6) this will
reduce the impedance at high frequencies.
Include these decoupling capacitors in the circuit diagram before starting
with the pcb design
3- KEEP THE TRACKS SHORT AND SUFFICIENT SPACED FROM
The impedance (caused by the capacitance and leakage resistance) between
tracks is not zero, this is often the cause of unwanted oscillations in particular
when using fast circuits or high gain amplifier circuits. In some cases it could
be necessary to use a guard ring around sensitive signal tracks. Use sufficient
spacing to other tracks in particular the input signals of amplifier circuits
(exceptions can be made for data signals) and when using high voltages (#7).
- 4- TRY TO USE SINGLE SIDED BOARDS ONLY
Use single sided boards (copper layer on the bottom side) only, unless you
are using so many components and you have no other choice than to use the
second layer as well (#8 and #9). Single sided boards are cheaper and easier to
manufacture than double sided boards !
5- LIST THE PHYSICAL DIMENSIONS OF COMPONENTS
Before using the computer, make a list with all dimensions, lead spacing and
lead diameter of the components you intend to use. This is also important
when you intend to use Protel Schematic!
Example of an axial component:
Note that the lead space is larger than
the component length and that the component
is soldered on the bottom.
Bottom side of the PCB only.
6- LIST THE PIN NUMBERS
In a circuit diagram you normally use symbols for the individual components
where every input or output (of an IC) and any connection to other
components corresponds with a physical pin number (see the Data Books for
physical dimensions and pin configurations). Specify the pin numbers in your
circuit diagram since you will need this information in the PCB design (unless
you have created a netlist with a schematic program such as Protel
USING PROTEL - PCB ADVANCED
1- READ THE MANUAL
Like any other software it is recommended to read the manual first to get
some basic understanding of this package! In some cases there is necessary
to read Help File available from Menu Bar.
2- USING A NETLIST
It is possible, for example after you have created a circuit diagram with
PROTEL-SCHEMATIC and the generation of a so called NETLIST, to “ load
your schematic (as a netlist)” directly in to PCB (see # 10). It is however
very important that all the pins of the components are assigned as well as all
the packages (ie.: dipl4, axial 0.3, etc.) and make sure that all physical
packages you are using exists in the PCB Library!
- Advantages of using a Netlist are;
-mistakes are eliminated to a large extend
-automatic placement of all the components from the schematic diagram (you could
otherwise forget some components!)
-using the DRC option allows you to compare your PCB file with the actual schematic
diagram (and also check your spacings)
-all logical connections are visible with so called rubber bands allowing optimum
placements of components and tracks
Disadvantages of using a Netlist are;
As mentioned above you must specify everything correctly in your Circuit Diagram
otherwise, and especially when you are not that familiar with Protel Schematic, you
could spend quite some time solving problems with netlist transfers which are always
likely to occur. Unless you have enough time to spend to learn this exercise, it is not
recommended to use a netlist when you are an unexperienced user.
3- STARTING PROTEL-PCB
Protel-PCB will ask you what file name it should load, however since you have
not yet created a name and directory yet (when you use PCB for the first
time), you should now press the ESC button, in case your pcb file already
exists type the name of your directory and your design file name.
4- USE IMPERIAL DIMENSIONS
From the Data Books you might have noticed that the semiconductor industry
is not using the metric system as a standard, all dimensions are in inches!!!
The dimensions of passive components on he other hand are often specified
in millimetres! Keeping the above in mind and to avoid too much confusion it is
suggested to select the Imperial sizes in PCB (Options), all dimensions will
then be in 0.001 (mils) of an inch (or multiples).
1000 mils = 1 inch = 25.4 mm = 2.54 cm
10 mils = .254 mm
1 mm = .039 inch = 39 mils
5- VISIBLE GRID and SNAP GRID
PCB is using a visible grid (will not appear in the artwork) which will
help you to place components and tracks in a symmetrical order (you don’ t
want your board to look like a mess!). Snap grid acts like an “ invisible grid”
where when placing components or tracks they will snap or lock on to even
when the cursor is not placed on this grid.
6- Set the VISIBLE GRID to 1000 and the SNAP GRID to 100 mils !!
7 DO NOT CHANGE TOO MANY OF THE DEFAULT SETTINGS
- 8- DEFINING THE BOARD DIMENSIONS
You could in fact now start to define the outline dimensions of your board,
however in many cases it is better to do this at a later stage since the size
depends not only on the number of components but also how you place them
(unless of course you are restricted by a certain size you could start now).
When using a Netlist please refer to #11 !
9- PLACE THE COMPONENTS BY PHYSICAL SHAPE
You might have noticed from the Protel-PCB Manual that you can not place
components by just calling a part from the library with the usual part numbers
(say a LM741), you can only load a physical equivalent such as:
DIP8 - LM741
AXIAL0.4 - RESISTOR (.33 W)
CD0.2/1 - DECOUPLING CAPACITOR (lOOnF)
10-PLACE COMPONENTS FROM THE TOP VIEW
When placing components, place them in such a way as if you are looking on
top of the board since the physical layout or pin configuration of components
in the Data Books are usually shown from the top.
11-KEEP THE COMPONENTS CLOSE TOGETHER
Large spacings between components will cause undesired long tracks and will
increase your PCB dimensions and thus cost.
12-KEEP ANALOGUE AND DIGITAL CIRCUITS SEPARATED
In case your application involves a combination of analog and digital circuits
it is recommended to keep these circuits physically separated on the PCB (to
minimise noise). Try to avoid common supplies and grounds, in case you have
no other alternative, keep the supplies and grounds separate and connect them
at one point only.
13-PLACE COMPONENTS IN ONE DIRECTION AND ORIENTATION
Start placing components either all vertical (i.e.: all with the reference pin1 at
left top corner with IC’ s) or horizontal (when this is more practical) and in
such a way so that it will be the best allocation to make the interconnections
(tracks) as in the schematic diagram. This is more important for larger PCB’ s
and where a “ tidy” appearance is required.
- 14-LABEL AND COMMENT THE COMPONENTS
When placing components Protel-PCB will ask you for a Component Name
(physical type) following a component designator and comment (value or part
NAME=AXIAL 0.4 (for a standard resistor)
PCM5/2.5 (for a standard capacitor)
DIP 8 (for an OPAMP)
DESIGNATOR=R1 (for a resistor, R2 for the next and so on)
C1 (for a capacitor)
IC1 (for an integrated circuit ie.: OPAMP)
COMMENT=10 Kohm (for a particular resistor)
1 nF (for a particular capacitor)
LM741 (for an OPAMP)
NOTE: After placing many components the text might disturb the visibility
when placing tracks, suggestion; turn the comments off (edit
15-USE LARGE PADS
Since you have to solder each component connection or PIN to a particular
track the Autotrax software will create PADS (or donuts) whose size and
shape are determined by a default setting. Try to keep the size of the pads
large enough (in some cases you might have to alter the default settings to a
larger size ie.: Edit Pad).Also adjust the size of the pad in relation to the size
of the holes to be drilled later on, so watch the lead sizes of your components
(#12) ! Do not forget to specify the hole sizes, a not defined hole size (ie.:0)
will cause no pad holes in the artwork plot!
RECOMMENDED MINIMUM PAD SIZES:
60 mils for Via’ s (double sided boards only drill size 0.6mm)
70 mils for resistors, capacitors etc. (drill size 0.8mm)
60x100 mils rounded rectangle for IC pins (drill size 0.6mm)
Use larger pad sizes when increasing the hole or drill sizes!!
16-PLACING THE TRACKS
The best (other people might disagree) way is to start laying tracks for all
signals first and the (wider) tracks for the power supplies last ! Change the
Visible Grid to 100 and Snap Grid to 25.
Always consider your currents especially with power supply tracks!
- When using single sided boards place the tracks as if you are looking through
the board (imagine the circuit board is transparent) and place the tracks on the
solder or bottom side (default: blue layer) only! For double sided boards you
place the tracks on the solder side the same way as single sided, but note the
tracks on the component or top side (default: red layer) are also viewed from
the same perspective. See Figure 2.
Avoid the number of top layers (component side) as much as possible since
soldering (and especially desoldering) components on this side is often
difficult and could, when you are not very careful, damage your tracks !
RECOMMENDED MINIMUM TRACK SIZES:
16 mils for signal tracks (thin tracks are difficult to etch) 100 mils for power
supply tracks, see the trax width graph in the appendix for other sizes.
17-OUTLINE THE DIMENSIONS OF THE PCB BY PLACING
TRACKS ON EACH LAYER USING THE BOARD LAYER.
When you have finished placing all components and tracks, you should define
the outline of the PCB by placing tracks of 16 mils on the board layer (turn it
on in Options!) around the designed board, this will determine the final
dimensions on each layer of your board!
18-GIVE YOU BOARD A NAME BY PLACING A TEXT (STRING)
Do this on each layer used in the design, but do not forget to mirror the text
on the solder side (you look through the board remember!). This can be done
with the EDIT-CHANGE-MIRROR.
19-OPTIMISE YOUR LAYOUT
Increase the width of the power supply tracks (in particular ground) where
possible, reduce the layers on the component side by swapping them to the
solder side and minimise the number of Via’ s!
20-DO NOT FORGET TO SAVE YOUR WORK!!!
Although Protel-PCB will create an automatic back up (usually to harddisk) it is
important that you make a back up to a floppy disk as well. Do this during the time you
are working on your PCB design as well (say every l0 min) to secure your
As mentioned in the beginning (page 4) the actual plot for the final Artwork
should be created in Postcript Format (using the 1270DPI-Linotronix) and
processed by an outside company. Supply your Technician with your PCB
File when you reached this stage! However plotting or printing (to a standard
laser printer) your Artwork on paper could still be useful for the following;
• Checking all connections and holes.
• Final layout of components.
• Final layout of strings(TEXT)
- PRINTOUT YOUR JOB
Printing with Protel-PCB can be done with a submenue of File/Print/Final Artwork.
Before you do so make sure that the bottom left corner of your PCB file is at the
xy coordinates 0,0 (when not move with the block commands).
USING THE (POSTCRIPT) LASER PRINTER FOR MAKING NEGATIVE
The final stage of your PCB design at our department is to create a file which can be
sent outside to make a very high resolution negative on photoplotter.
1-Open your File
2-Select File/Print/Final Artwork - Show Holes always marked
Never use Fit Layer on Page
4-Select Linotronics 200/230(300) on LPT1:
5-Select Options/Enc.Postscript File/ - put name of your file (it will be in current dir.)
6-Select Output/Mirroring - Bottom only
7-Select Output - layers Top and Bottom only
Your file will be as a postscript type. This one or compressed its form can be sent
outside to make a negative for further process.
BILL OF MATERIALS
You can create file contains list of components:
Select File/Reports/Bill of Material.
CREATE NEW COMPONENT
Before you make a new component copy existing library on to your disk.
2-Name new component
3-Draw new component using pads and tracks on appropriate layer (yellow for layout
andmultilayer for pads).
4-Name pads for your component.(Each name should be related to the name
at Protel-Schematic- more convenient way for transferring netlist).
5-Save your work under new name inside your current library.
You can create new component using existing from library and changing
just size of pads, number of pins or pins numbering. Hence always save your
work on floppy-disk or into your directory on C: or other personal drive.
- A PRINTED CIRCUIT BOARD EXAMPLE
1- The Analog and Digital circuits are clearly separated
2- Practically all IC’ s are orientated in one direction
3- The spacings in between the components are kept to a minimum
4- The board and components are shown from top view
5- The bypass capacitors are close to the (mainly) digital IC’ s
6- Power supply tracks are wider than the signal tracks
7- Double sided (100x160 mm) PCB, 150 components, 6 Via’ s and 600 holes.
#1 There are other techniques feasible such as:
-Bread boarding (usually for prototyping and quick results)
-Wire wrapping (mainly for prototyping of digital circuits)
-Strip(Vero) board (for smaller circuits and one offs)
#2 There are (Routing) Machines available on the market able to generate a PCB
(including drilling) directly from a plot file, thus eliminating the chemicals and
environmental hazardous chemical process, however not very satisfactory at
present (likely to be improved in the near future).
#3 For high density and some times high speed PCB’ s and the use of a special
manufacturing process the number of layers can be significantly increased (the
copper and epoxy layers are thinner), this is called a multilayer board (club
#4 When creating a so called Gerber File (instead of normal HPGL Plot File)
it is possible create the artwork (positive) on a Photo Plotter (very accurate but
at high costs). Standard Postscript printers are not very accurate however there
are special Postcript printers such as the Linotronix able to produce negatives
directly with 1270 and 2540 DPI resolution and sufficient accuracy.
#5 Logic circuits (even CMOS) require much higher (switching) currents from
the power supply when they are CHANGING STATE therefore the average
current will increase proportionally with the frequency.
WIDTH: 30 45 oC
This graph can 25 C
be used to deter- 20
mine track width 12
as a function of 10
current and 7
temperature rise 4
Do not allow a 0
higher increase 5
CONDUCTOR WIDTH (MILS)
temperature than 50
20 degrees. 100
Work with 1 0Z 150
copper only. 250
0 1 2 5 10 20 30 50 70 100 150 200 250 300 400 500 600 700
CROSS SECTION (SQUARE MILS)
- #6 USING CAPACITORS
A 100 nF (low inductive) ceramic, preferable multi layer type, capacitor is
usually sufficient. For higher frequencies (>lOMHz) it is recommended to use
an additional lnF ceramic capacitor in parallel, this because the impedance of
the 100nF capacitor will increase (due to the self inductance) at higher frequencies
Some analog IC’ s (such as analog to digital converters and high speed amplifiers)
and voltage regulators often require other values (refer to the Data Books) !
#7 TRACK SPACINGS
This table shows track spacings depending on voltage between tracks:
Voltage Min. Distance Min. Distance
(DC or AC peak) (uncoated) (coated)
up to l5V l5mil-0.38mm 5 mil-0.13mm
l5V.. 30V l5mil-0.38mm 10mil-0.25mm
30V.. 50V l5mil-0.38mm l5mil-0.38mm
50V.. 100V 25mil-0.64mm 20mil-0.Slmm
100V..l5OV 25mil-0.64mm 30mil-0.76mm
150V..300V 50mil-1.27mm 30mil-0.76mm
300V..500V 100mil-2.54mm 60mil-1.52mm
above 500V 0.2mil/volt 0.12mil/volt
Do not forget to check the
following spacings in
Protel-PCB and on your
For some applications such as very fast circuits (>50MHz) you might need
the second layer (usually the top layer) as a so called GROUND PLANE (all
connections to this type of layer will be of low impedance!).
When using a double sided board use vertical tracks on one side and all
horizontal tracks on the other side (to avoid being blocked when placing
- multiple tracks), try to keep most of the tracks on the solder(bottom) side
since soldering components on the top of the board is often a problem.
To generate a Netlist File (your schem.S01) with Protel-Schematic, exit from
Schematic and Execute POST in the Schematic Directory, do not specify the
extension (S01) especially when you have multiple sheets of the same file
name (ie.: fileX.S01.. fileX.S02 etc., schematic will link the sheets).
As mentioned in 2 it is very important that all the pins of the components
are assigned as well as all the packages (ie.: dipl4, axial 0.3, etc.) and make
sure that all physical packages you are using exists in the Library!
In case you have created your own parts library you probably have to merge
components from the Protel-PCB Library in to your library for all
the components you are using in your design!
Loading a Netlist in Protel-PCB
At first you must draw a Box using the Keep Out Layer (turn this on with
Setup Toggle Layers) from X,Y=0,0 (say track width = 15 mils) to the
approximate size you expect your PCB to be.
Select: Netlist, Load (yourfile.net)
This should display:
Missing Components: no. of components
All components should now, although all on top of each other, appear on the screen.
When asked to generate a report file, select YES and read this file and correct errors when
they occur and restart the above! Corrections need to be made inside netlist file or diagram
made by Protel-Schematic.
Particulary consider consistency between Protel-Schematic and PCB in:
names for component patterns(footlayers),
names of pins,
number of pins.
Select Auto, Autoplacement.
Comonents automaticaly co into Box of Keep Out Layer.
This will move (spread out) all components to the appropriate grid as
defined in Autoplace Setup. In case you wish to move all components to a
different grid size, select Move all Components to Grid and specify the
desired grid size.
Components placed from netlist are connected with ratnets (rubberband). They
indicate which pin should be linked to which one.
Happy with the way ‘ Auto Placement’ placed your components??
- I doubt it!
The Auto Placement in Protel-PCB does not work very satisfactory, you will do a
better and faster job by placing the components manually !
The best way to continue from here is to manually place all the components
to a better location. In case you are using many components it is best to define a
block (covering all components, not the Keep Out Layer) and move the block out
side the keep out area (then hide block).
With the Schematic Diagram as a guide for component allocations, move the
components one by one to a suitable position on the board area and similar as the
locations in the diagram, start with IC’ s and connectors first.
During this process you will probably find that some ratnets bands are
crossing one other, avoid these crossings by rotating the components. In some
cases (such as connector pins, IC pins etc.) you might like to swap pins.
Placing / routing Tracks
You could in fact now automatically route the board, however this is not
recommended since you are able (at least I hope so) to do a much better job, by
using the manual router, than the Autorouter from Protel-PCB (which is usually
placing far to many Via’ s).
Manual placing tracks:
Select: Current, Layer and select the Bottom Layer
Select: Current, Track Width and select the desired track width
Select: Edit, Place, Track,
and start to place track.
Manual placing track using netlist:
Select: Auto, Setup Autoroute (Choose layers and other options)
Select: Auto, Manual and point a net (using the cursor) you
wish the to start routing, place the tracks using the rubber bands as a guide for the
connections (as mentioned before try to keep the horizontal tracks on one layer
and the vertical tracks on the other layer) and you will notice that once a
particular net is routed the rubber band will disappear. When all nets are routed
no rubber bands should be left and you should now be able to perform a Design
Rule Check (DRC), this option is very useful since it will compare your PCB file
with the netlist from schematic and check all clearances on the boards.
Since the copper layer is glued to the epoxy board it could easily happen
that the pads (when too small) will come off when soldering (heat will soften the
adhesive). This could also happen when drilling the holes in the PCB !
1- Linear Design seminar, Analog Devices 1987
2- High Speed Design Seminar, Analog Devices 1990
3- Fundamentals of Printed Circuit Design and Manufacturing 1986
4- Printed Circuit Technical Manual 107, Bishop Graphics 1982
5- Protel Autotrax Manual 1988
6- Protel Schematic Manual 1990
7- Printed Circuit Workbook Series, Volume 1, Clyde F.Coombs 1988
The following attached list shows the physical dimensions of components available in the
listed Libraries below. Use this list also to define package outlines in Protel Schematic.
The are 3 Libraries are located in Y:\ELECTRIC\ADVPCB\LIBRARY\*.LIB
RESISTORS, CAPACITORS, SEMICONDUCTORS, TRIMMERS
CONNECTORS, TRANSFORMERS, HEATSINKS, MISC.DEVICES
SURFACE MOUNT DEVICES
If you want to make some changes make a copy of library file to your directory first!!!
In case you are unable tom find a suitable part you must create your own part(s) and store this
part(s) in yours.lib!
In the above directory standard pcb card formats are available such as:
Eurocards 100x160 mm (ie.:euro-a.pcb) and IBM-PC cards (ie.:atboard.pcb)
• To reduce the number of parts and depending on what technology is required (ie. CMOS,
LINEAR etc) Protel Schematic is using many different libraries which can be loaded
individually by the program.
• The Schematic Libraries contains symbols of components whereas the PCB Libraries
contains the physical layout of components.
• The DEVICE.LIB from Schematic only supports basic symbols of certain components.
Example for some stndard components:
TYPE LIBRARY FILE COMPONENT NAME PACKAGE
RESISTOR DEVICE.LIB RES2 AXIAL0.4
CAPACITOR DEVICE.LIB CAP CD0.2/1 (lOOnF)
CAPACITOR DEVICE.LIB CAP PCM5/2.5 (1nF/63V)
ELECTROLYTIC DEVICE.LIB ELECTRO2 R0.1/0.2 (22 uF/25V)