1. technology and computing
2. electronic components

Cadence PCB Editor Tutorial
Version 16.6
Josh Bishop and Kirsch Mackey
Department of Electrical Engineering
University of Arkansas, Fayetteville, AR
Email: [email protected]
APRIL 7, 2015
UNIVERSITY OF ARKANSAS
3217 Bell Engineering Ctr, Fayetteville, AR, 72701
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Contents
Preamble ................................................................................................................................... 2
1. Introduction to the Astable Multivibrator ................................................................................. 3
1.1 The idea behind the astable multivibrator ...................................................................... 3
1.2 Basic Astable Multivibrator Circuit ................................................................................. 3
1.3 Astable Multivibrators Periodic Time ............................................................................. 4
1.4 Frequency of Oscillation ................................................................................................ 5
1.5 Waveforms .................................................................................................................... 5
1.6 Example ........................................................................................................................ 5
2. Creating Component Pads and Footprints ............................................................................. 7
2. Preliminary Work ................................................................................................................ 7
2.0.1 Collecting data sheets ................................................................................................ 7
2.0.2 Circuit Footprints ........................................................................................................ 8
2.1 Padstacks & Footprints for Surface Mount Parts............................................................... 8
2.1.1 Surface Mount Resistor .............................................................................................. 8
2.1.2 Surface Mount Capacitor...........................................................................................11
2.1.3 Surface Mount Transistor ..........................................................................................14
2.2 Padstacks & Footprints for Through-hole Parts................................................................18
2.2.1 Through-hole Resistor ...............................................................................................18
2.2.2 Through-hole Capacitor.............................................................................................18
2.2.3 Through-hole Transistor ............................................................................................22
3. Circuit Design in OrCAD Capture ..........................................................................................28
3.1 Schematic Creation and Simulation .................................................................................28
3.2 Getting ready for PCB......................................................................................................30
3.2.1 Assigning Footprints to Parts.....................................................................................31
3.2.2 Annotation of parts ....................................................................................................33
3.2.3 Creating the Netlist....................................................................................................34
4. PCB Editor Design Layout.....................................................................................................37
4.1 Setting the Environment ..................................................................................................37
4.2 Setting the Design Constraints ........................................................................................38
VIAs ...................................................................................................................................39
4.2 Creating the Board Outline ..............................................................................................40
4.3 Placing Parts ...................................................................................................................41
4.4 Routing the Board............................................................................................................43
5. Gerber Files and Drill File......................................................................................................48
1
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
5.1 Creating Apertures .......................................................................................................49
5.2 Creating the Drill File ....................................................................................................50
5.3 Checking the Gerber Files............................................................................................51
6. Milling the PCB .....................................................................................................................54
6.1 Training & Scheduling......................................................................................................54
6.2 On Making an Appointment .............................................................................................54
7. Soldering the Parts to the PCB..............................................................................................55
8. Verification ............................................................................................................................55
9. Appendix ...............................................................................................................................55
9.1 Minimum Spacing Guidelines for PCB Layout .................................................................55
9.2 Changing Vias dynamically ..............................................................................................55
9.3 How to adjust trace widths ...............................................................................................58
9.4 Routing Corrections & Techniques ..................................................................................58
9.4.1 Crooked Lines ...........................................................................................................58
9.4.2 Making Angled Connections ......................................................................................59
10. References..........................................................................................................................63
Preamble
This document was written primarily to assist the students taking ELEG 4061 and ELEG 4073
and anyone in the department wanting to take a circuit design from paper to a physical printed
circuit board (PCB).
Organization
This document falls into two parts:
 The tutorial that guides the student through a design and layout of a PCB from a
commonly used circuit – the frequency oscillator.
 The appendix contains some techniques and guides to help refine the design process.
Links to different parts of the appendix are given throughout the tutorial.
Learning Objectives
By the end of this tutorial, the student would have learned:
 How to properly annotate a circuit design in OrCAD
 How to set footprints for parts in an OrCAD circuit design
 Layout in Allegro PCB Editor for the circuit
 Creation of Gerber manufacturing files for milling machines
 Making sure your layout will mill correctly
 Soldering techniques for through-hole and surface mount devices
2
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
1. Introduction to the Astable Multivibrator
1.1 The idea behind the astable multivibrator
Below is an overview taken from Storr [1].
Oscillators are circuits which are designed to switch back and forth between states indefinitely,
rather than settling on a stable output at some point in time. Here, we design a circuit to oscillate
between off/on states, giving an output that appears as a square wave.
The Astable Multivibrator is another type of cross-coupled transistor switching circuit that
has NO stable output states as it changes from one state to the other all the time. The astable
circuit consists of two switching transistors, a cross-coupled feedback network, and two time
delay capacitors which allows oscillation between the two states with no external trigger signal
to produce the change in state.
The basic transistor circuit for an Astable Multivibrator produces a square wave output from a
pair of grounded emitter cross-coupled transistors. Both transistors either NPN or PNP, in the
multivibrator are biased for linear operation and are operated as Common Emitter
Amplifiers with 100% positive feedback.
This configuration satisfies the condition for oscillation when: ( βA = 1∠ 0o ). This results in one
stage conducting “fully-ON” (Saturation) while the other is switched “fully-OFF” (cut-off) giving a
very high level of mutual amplification between the two transistors. Conduction is transferred
from one stage to the other by the discharging action of a capacitor through a resistor as shown
below.
1.2 Basic Astable Multivibrator Circuit
Figure 1. Astable Multivibrator
Assume that transistor, TR1 has just switched “OFF” and its collector voltage is rising
towards Vcc, meanwhile transistor TR2 has just turned “ON”. Plate “A” of capacitor C1 is also
rising towards the +6 volts supply rail of Vcc as it is connected to the collector of TR1. The other
side of capacitor, C1, plate “B”, is connected to the base terminal of transistor TR2 and is at 0.6v
3
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
because transistor TR2 is conducting therefore, capacitor C1 has a potential difference of 5.4
volts across it, 6.0 – 0.6v, (its high value of charge).
The instant that transistor, TR1 switches “ON”, plate “A” of the capacitor immediately falls to 0.6
volts. This fall of voltage on plate “A” causes an equal and instantaneous fall in voltage on plate
“B” therefore plate “B” of the capacitor C1 is pulled down to -5.4v (a reverse charge) and this
negative voltage turns transistor TR2 hard “OFF”. One unstable state.
Capacitor C1 now begins to charge in the opposite direction via resistor R3 which is also
connected to the +6 volts supply rail, Vcc, thus the case of transistor TR2 is moving upwards in a
positive direction towards Vcc with a time constant equal to the C1 x R3 combination.
However, it never reaches the value of Vcc because as soon as it gets to 0.6 volts positive,
transistorTR2 turns fully “ON” into saturation starting the whole process over again but now with
capacitor C2taking the base of transistor TR1 to -5.4v while charging up via resistor R2 and
entering the second unstable state. This process will repeat itself over and over again as long
as the supply voltage is present.
The amplitude of the output waveform is approximately the same as the supply
voltage, Vcc with the time period of each switching state determined by the time constant of
the RC networks connected across the base terminals of the transistors. As the transistors are
switching both “ON” and “OFF”, the output at either collector will be a square wave with slightly
rounded corners because of the current which charges the capacitors. This could be corrected
by using more components as we will discuss later.
If the two time constants produced by C2 x R2 and C1 x R3 in the base circuits are the same,
the mark-to-space ratio ( t1/t2 ) will be equal to one-to-one making the output waveform
symmetrical in shape. By varying the capacitors, C1, C2 or the resistors, R2, R3 the mark-tospace ratio and therefore the frequency can be altered.
We saw in the RC Discharging tutorial that the time taken for the voltage across a capacitor to
fall to half the supply voltage, 0.5Vcc is equal to 0.69 time constants of the capacitor and
resistor combination. Then taking one side of the astable multivibrator, the length of time that
transistor TR2is “OFF” will be equal to 0.69T or 0.69 times the time constant of C1 x R3.
Likewise, the length of time that transistor TR1 is “OFF” will be equal to 0.69T or 0.69 times the
time constant of C2 x R2 and this is defined as.
1.3 Astable Multivibrators Periodic Time
Where, R is in Ω’s and C in Farads.
By altering the time constant of just one RC network the mark-to-space ratio and frequency of
the output waveform can be changed but normally by changing both RC time constants together
at the same time, the output frequency will be altered keeping the mark-to-space ratios the
same at one-to-one.
4
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
If the value of the capacitor C1 equals the value of the capacitor, C2, C1 = C2 and also the
value of the base resistor R2 equals the value of the base resistor, R3, R2 = R3 then the total
length of time of theMultivibrators cycle is given below for a symmetrical output waveform.
1.4 Frequency of Oscillation
Where, R is in Ω’s, C is in Farads, T is in seconds and ƒ is in Hertz.
and this is known as the “Pulse Repetition Frequency”. So Astable Multivibrators can produce
TWO very short square wave output waveforms from each transistor or a much longer
rectangular shaped output either symmetrical or non-symmetrical depending upon the time
constant of the RC network as shown below.
1.5 Waveforms
Figure 2. Multivibrator Waveforms
1.6 Example
An Astable Multivibrators circuit is required to produce a series of pulses at a frequency of
500Hz with a mark-to-space ratio of 1:5. If R2 = R3 = 100kΩ’s, calculate the values of the
capacitors, C1 and C2required.
5
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
and by rearranging the formula above for the periodic time, the values of the capacitors required
to give a mark-to-space ratio of 1:5 are given as:
The values of 4.83nF and 24.1nF respectively, are calculated values, so we would need to
choose the nearest preferred values for C1 and C2 allowing for the capacitors tolerance. In fact
due to the wide range of tolerances associated with the humble capacitor the actual output
frequency may differ by as much as ±20%, (400 to 600Hz in our simple example) from the
actual frequency needed.
If we require the output astable waveform to be non-symmetrical for use in timing or gating type
circuits, etc, we could manually calculate the values of R and C for the individual components
required as we did in the example above. However, when the two R’s and C´s are both equal,
we can make our life a little bit easier for ourselves by using tables to show the astable
multivibrators calculated frequencies for different combinations or values of both R and C. For
example,
Table 1. Astable Multivibrator Frequency Table
Capacitor Values
Res.
1nF
2.2nF
4.7nF
10nF
22nF
47nF
100nF 220nF 470nF
1.0kΩ 714.3kHz 324.6kHz 151.9kHz 71.4kHz 32.5kHz 15.2kHz 7.1kHz 3.2kHz 1.5kHz
2.2kΩ 324.7kHz 147.6kHz 69.1kHz 32.5kHz 14.7kHz 6.9kHz 3.2kHz 1.5kHz 691Hz
4.7kΩ 151.9kHz 69.1kHz 32.3kHz 15.2kHz 6.9kHz 3.2kHz 1.5kHz 691Hz 323Hz
10kΩ 71.4kHz 32.5kHz 15.2kHz 7.1kHz 3.2kHz 1.5kHz 714Hz 325Hz 152Hz
22kΩ 32.5kHz 14.7kHz
6.9kHz
3.2kHz 1.5kHz
691Hz
325Hz 147Hz 69.1Hz
47kΩ 15.2kHz
6.9kHz
3.2kHz
1.5kHz
691Hz
323Hz
152Hz 69.1Hz 32.5Hz
100kΩ 7.1kHz
3.2kHz
1.5kHz
714Hz
325Hz
152Hz 71.4Hz 32.5Hz 15.2Hz
220kΩ 3.2kHz
1.5kHz
691Hz
325Hz
147Hz
69.1Hz 32.5Hz 15.2Hz 6.9Hz
470kΩ 1.5kHz
691Hz
323Hz
152Hz
69.1Hz 32.5Hz 15.2Hz 6.6Hz 3.2Hz
325Hz
152Hz
71.4Hz 32.5Hz 15.2Hz
1MΩ
714Hz
6
6.9Hz 3.2Hz 1.5Hz
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
By changing the two fixed resistors, R2 and R3 for a dual-ganged potentiometer and keeping the
values of the capacitors the same, the frequency from the Astable Multivibrators output can
be more easily “tuned” to give a particular frequency value or to compensate for the tolerances
of the components used.
For example, selecting a capacitor value of 10nF from the table above. By using
a 100kΩ’spotentiometer for our resistance, we would get an output frequency that can be fully
adjusted from slightly above 71.4kHz down to 714Hz, some 3 decades of frequency range.
Likewise a capacitor value of 47nF would give a frequency range from 152Hz to well over
15kHz.
2. Creating Component Pads and Footprints
2.0 Preliminary Work
Before we begin using OrCAD Capture CIS design software, we need all appropriate
components for the parts we intend to use. We will need 2 capacitors, 2 resistors and 2
transistors. For each of these components we need the appropriate data sheet so we can then
create the pads and footprints to place in the OrCAD design.
2.0.1 Collecting data sheets
For any PCB project, you need a physical or electronic copy of every device/component you will
be using. Do not assume anything about the devices you are using, because the measurements
for every component and device are very specific. Luckily, we have selected all the devices and
components for this tutorial and put them in Table 2.
Part
5kΩ resistor
(surface mount)
5kΩ resistor
(through-hole)
Table 2. Parts List for astable multivibrator
Model Number
Image
RC0603FR074K99L
CMF075K0000
JNEK
470kΩ resistor
(surface mount)
470 kΩ resistor
(through-hole)
Company data sheet
Yageo datasheet
Vishay datasheet
0.47 µF capacitor
(surface mount)
RC0603JR07470KL
Generic carbon
film resistor (¼
W, ±5%)
GRM188R71C4
74KA88J
0.47 µF capacitor
(through-hole)
ECEA1HKSR47
Panasonic datasheet
2N3904 NPN transistor
(surface mount)
MMSS805-HTP
NPN transistor
(through-hole)
2N3904BU
Micro Commerical
Components
datasheet
Fairchild datasheet
7
Yageo datasheet
any
Murata datasheet
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Go ahead and download all data sheets and put them into a folder designated for this project.
Call the folder “Datasheets”.
Now that you have all the data sheets, you need to make sure they have information on the
physical layout of the devices. Set that information aside and we will use them to create
footprints and padstacks using Cadence software packages.
2.0.2 Circuit Footprints
In order to translate the schematic onto a PCB, each component needs a footprint.
A footprint is the physical interface a device (such as a transistor) makes with a PCB. It allows
you to place parts, which connect with traces. Since some parts are very small, these footprints
need to be incredibly accurate.
Sometimes we can get lucky and the footprint we need is already in the Cadence library.
Common components like through-hole resistors (RES500) are already in the library, but for
everything else you should make your own footprints.
You can view the footprints in C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols and they can
be opened with PCB editor. You will need to be absolutely sure that these footprints work with
your devices, but there is no good way to measure these already-made footprints in PCB Editor.
For these reasons, it is best just to make your own footprints.
2.1 Padstacks & Footprints for Surface Mount Parts
2.1.1 Surface Mount Resistor
We will go over how to create the pads and footprint for the surface mount resistor.
A. PADS FOR THE SURFACE MOUNT RESISTOR
1. Go to Windows Start > All Programs > Cadence > Release 16.6 > PCB Editor Utilities >
Pad Designer.
2. Open the data sheet for the surface mount resistor in this project (model RC0603FR074K99L).
3. Page 4 has the dimensions of the resistor illustrated below.
8
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
4. In Pad Designer, Go to File > New. In the New Padstack window, type a suitable name
in the Padstack Name field (e.g. RC0603.pad).
5. Click OK.
6. In the Pad Designer window, change the Units field to Millimeter (select Continue when
prompt about accuracy appears).
7. Select the Layers tab. Check the box that says Single layer mode.
8. Ensure that the Views section has Top selected instead of XSection.
9. In the Geometry field, select rectangle from the dropdown menu.
10. The Width field will be 0.5000.
11. The Height field will be 1.0000 mm.
12. Your padstack should look like the illustration below.
13. When that’s done, go to File > Save As….
14. Save the file to the directory C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
15. Save it as “rc0603.pad”.
16. Exit Pad Designer.
B. FOOTPRINT FOR THE SURFACE MOUNT RESISTOR
1. Go to Start > Programs > Cadence > Release 16.6 > PCB Editor.
2. Go to File > New.
3. In the New Drawing window, type the drawing name RC0603.dra.
4. In the Drawing Type field, select Package symbol (wizard) from the list.
9
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
5. Make sure the Project Directory is located in
C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
6. Once this is all confirmed, click OK.
7. For the resistor, we select SMD (Surface Mount Device) DISCRETE packaging.
8. Once selected, click Next.
9. Have “Default Cadence supplied template” selected.
10. Click the Load Template button. A prompt will appear. Click Yes.
11. Hit Next.
12. In this Package Symbol Wizard window, change the units in both fields from Mils to
Millimeter.
13. In the Reference designator prefix field, type “RC0603*”.
14. Click Next.
15. In the window “Package Symbol Wizard – Surface Mount Discrete Parameters”, we’ll
look at the datasheet again for the resistor. Page 4 has all the information we need to fill
in to the next PCB Editor window.
Where Table 1 on the data sheet has the following information:
TYPE
L (mm)
W (mm)
H (mm)
I1 (mm)
I2 (mm)
RC0603
1.60 ± 0.10
0.80 ± 0.10
0.45 ± 0.10
0.25 ± 0.15
0.25 ± 0.15
The values to place in our windows settings were calculated,
Parameter
Terminal pin spacing (e1)
Package width (E)
Package length (D)
Calculation
L – 2 × ½∙I1 = 1.60 – 2 × ½ × 0.25
L – 2 * I1 = 1.60 – 2×(0.25)
W value on data sheet
Value (mm)
1.350
1.100
0.800
Once the information is filled in, your window should look like below:
16. Click Next, then click the
box in the “Padstack to use for pin 1:” field.
17. In the Package Symbol Wizard Padstack Browser, scroll down to the pad we created
earlier called “Rc0603”.
10
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
18. Click OK. Click Next.
19. Leave the default choices in the Package Symbol Wizard – Symbol Compilation.
20. Click Next. Click Finish.
21. Your footprint should look like below.
22. Go to File > Save.
23. If it asks you to overwrite, choose Yes, just to make sure.
2.1.2 Surface Mount Capacitor
A. PADS FOR THE SURFACE MOUNT CAPACITOR
The process for the capacitor is similar to that for the resistor. However, there are some
differences.
1. Open the data sheet for the surface mount capacitor in this project (model
GRM188R71C474KA88J).
2. Page 1 has the dimensions of the capacitor illustrated below.
3. Open Pad Designer from the Windows Start menu.
4. Select File > New. In the New Padstack window, type a suitable name in the Padstack
Name field (e.g. CAPD16V.pad).
5. Click OK.
6. In the Pad Designer window, change the Units field to Millimeter (select Continue when
prompt about accuracy appears).
7. Select the Layers tab. Check the box that says Single layer mode.
8. Ensure that the Views section has Top selected instead of XSection.
9. In the Geometry field, select Rectangle from the dropdown menu.
11
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
10. The Width field value (for the pad rectangle) should have a width equal to the “e” value
for the surface mount capacitor edge, i.e. Width = e = 0.2 to 0.5 mm.
11. Choose 0.4 mm. This will make soldering onto the pads easier.
12. Change the Height field value equal to the W of the capacitor. So, 0.8 mm in this case.
13. Your padstack window should look like it does below.
14. When that’s done, go to File > Save As….
15. Save the file to the directory C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
16. Save it as “CAPD16V.pad”.
17. Exit Pad Designer.
B. FOOTPRINT FOR THE SURFACE MOUNT CAPACITOR
Now to make the footprint for the surface mount capacitor we just made.
1.
2.
3.
4.
5.
6.
7.
8.
9.
Go to Start > Programs > Cadence > Release 16.6 > PCB Editor.
Go to File > New.
In the New Drawing window, type the drawing name CAPD16V.dra.
In the Drawing Type field, select Package symbol (wizard) from the list.
Make sure the Project Directory is located in
C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
Once this is all confirmed, click OK.
We will select SMD (Surface Mount Device) Discrete.
Once selected, click Next.
Have “Default Cadence supplied template” selected.
12
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
10. Click the Load Template button. A prompt will appear. Click OK.
11. Hit Next.
12. In this Package Symbol Wizard – General Parameters window, change the units in both
fields from Mils to Millimeter.
13. In the Reference designator prefix field, type “CAPD16V*”.
14. Click Next.
15. For the Surface Mount Discrete Parameters use the following values and calculations
based on the data sheet (shown in previous section A. Pads for the Surface Mount
Capacitor):
Parameter
How to calculate
Value (mm)
Terminal pin
g+2×½×e =
0.9
spacing (e1)
0.5+2×½×0.4*
Package width (E)
E=g
0.5
Package length (D)
D=W
0.8
16. So your screen should look like below.
17. Click Next.
18. Click the
button in the field “Padstack to use for pin 1:”.
19. Choose “Capd16v” from the list, then click OK.
20. Click Next.
21. The defaults choices in the new window are fine so click Next, then click Finish.
22. Your footprint will show up and look like the picture below.
13
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
23. Save CAPD16V.dra to the C:\...\symbols folder you were using already (should already
be selected).
24. Close PCB Editor.
2.1.3 Surface Mount Transistor
A. PADS FOR THE SURFACE MOUNT TRANSISTOR
Now we’ll do the surface mount transistor.
1. Go to Windows Start > All Programs > Cadence > Release 16.6 > PCB Editor Utilities >
Pad Designer.
2. Open the data sheet for the surface mount NPN transistor in this project (model
MMSS8050-H-TP).
3. Page 1 has the dimensions of the transistor illustrated below.
4. While we can use the dimensions, the data sheet already has suggested solder pad
layout values, so we’ll use those instead (shown below).
14
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
5. In Pad Designer, Go to File > New. In the New Padstack window, type a suitable name
in the Padstack Name field (e.g. NPNSOT23.pad).
6. Click OK.
7. In the Pad Designer window, change the Units field to Millimeter (select Continue when
prompt about accuracy appears).
8. Select the Layers tab. Check the box that says Single layer mode.
9. Ensure that the Views section has Top selected instead of XSection.
10. In the Geometry field, select Square from the dropdown menu.
11. The Width and Height fields are equal to 0.8000 mm, but we would suggest increasing
that to 1.1 to allow more space for soldering.
12. Your padstack should look like the illustration below (anywhere from 0.8 to 1.1 mm).
13. When that’s done, go to File > Save As….
14. Save the file to the directory C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
15. Save it as “npnsot23.pad”.
16. Exit Pad Designer.
15
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
B. FOOTPRINT FOR THE SURFACE MOUNT TRANSISTOR
Now to make the footprint for the surface mount transistor padstack we just made. The footprint
for the transistor does not have the same number of pads on both sides so we’ll have to use a
technique to work around that.
1.
2.
3.
4.
5.
Go to Start > Programs > Cadence > Release 16.6 > PCB Editor.
Go to File > New.
In the New Drawing window, type the drawing name “npnsot23.dra”.
In the Drawing Type field, select Package symbol (wizard) from the list.
Make sure the Project Directory is located in
C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
6. Once this is all confirmed, click OK.
7. For the transistor, we will select SOIC packaging.
8. Once selected, click Next.
9. Have “Default Cadence supplied template” selected.
10. Click the Load Template button. A prompt will appear. Click Yes.
11. Hit Next.
12. In this Package Symbol Wizard – General Parameters window, change the units in both
fields from Mils to Millimeter.
13. In the Reference designator prefix field, type “NPNSOT23*”.
14. Click Next.
15. For the Surface Mount - SOIC Parameters use the following values:
Parameter
How to calculate
Value (mm)
Number of pins (N)
6 (we will delete 3
6 pins
later)
Lead pitch (e)
Datasheet suggested
0.950
values
Terminal row
Datasheet suggested
2.000
spacing (e1)
values
Package width (E)
E = C (datasheet)*
1.300* (extra room)
Package length (D)
D=W
2.900* (extra room)
16. So your screen should look like below.
16
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
17. Click Next.
18. Click the
button in the field “Padstack to use for pin 1:”.
19. Choose “Npnsot23” from the list, then click OK.
20. Click Next.
21. The defaults choices in the new window are fine so click Next, then click Finish.
22. Your footprint will show up and look like the picture below (Note: the pin pads may
overlap if you chose larger pads ~1.1 mm. That’s still fine since we will delete 3 pins).
23. Left click pin 6. Right click. Click Delete.
24. Repeat this step for pins 2 and 4.
25. Left click pin 1. Right click it, go to > Selection set > Text “1”.
26. Right click on the number 1 and go to “Text Edit”.
27. Replace 1 with the number 2 (this is the Base on the transistor according to our data
sheet).
28. Repeat steps 25 – 27 so that pin 3 becomes pin 1, then finally pin 5 becomes pin 3 (in
that order).
29. Save “npnsot23.dra” to the C:\...\symbols folder you were using already (should already
be selected).
30. Close PCB Editor.
17
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
2.2 Padstacks & Footprints for Through-hole Parts
2.2.1 Through-hole Resistor
A. PADS FOR THE THROUGH-HOLE RESISTOR
The padstack for the through-hole resistor is already provided by OrCAD and Allegro.
B. FOOTPRINT FOR THE THROUGH-HOLE RESISTOR
The footprint for a standard through-hole resistor is “RES500”. We will use that in our design.
2.2.2 Through-hole Capacitor
A. PADS FOR THE THROUGH-HOLE CAPACITOR
The through-hole capacitor we will use is the Panasonic ECE-A1HKSR47 capacitor.
The rest of the datasheet shows our capacitor’s specifications are in the first column above.
So Body Diameter ϕ D = 4 mm, Lead Diameter ϕd = 0.45 mm and Lead space F = 1.5 mm.
So the hole we make will be the diagonal length of the 0.45 mm lead dimensions (to insert the
capacitor lead completely without jamming.). Using the Pythagorean Theorem, hole diameter =
2
√0.452 + 0.452 = 0.63639 mm .
We’ll make our pad such that the pads won’t be touching. So 1.1 mm pad surface spacing is
suitable and the separation between the pads needs to be 1.5 mm. We will set this separation in
PCB Editor Device wizard. Through-hole pads are on two layers (top and bottom).
1. Go to Windows Start > All Programs > Cadence > Release 16.6 > PCB Editor Utilities >
Pad Designer.
2. Go to File > New. In the New Padstack window, type a suitable name in the Padstack
Name field (e.g. CAPTH4MM.pad).
3. Click OK.
4. In the Pad Designer window, change the Units field to Millimeter (select Continue when
prompt about accuracy appears).
5. Select the Layers tab. Make sure Single layer mode is Unchecked.
18
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
6. This time ensure that the Views section has XSection selected instead of Top.
7. Click on the
layer button.
8. In the Geometry field, select Circle.
9. Change the Width field value for the circle to 1.0000.
10. The height changes automatically and a bar (red or blue) shows up in the diagram.
11. Click on the
button then repeat steps 8 through 10.
12. Click on the
button next to Default Internal and repeat steps 8 through 10.
Your screen should look similar to this (the colors may not match exactly).
13. Click on the Parameters tab. You will see a filled yellow circle.
14. In the Drill/Slot hole section, you should see the field Hole type with “Circle Drill”
selected. If not, then change it to Circle Drill.
15. In the field “Drill diameter”, type 0.6364 mm (because that’s the diagonal we calculated
above for the hypotenuse of the capacitor’s square/shaped lead legs, ϕd by ϕd).
16. In the Drill/Slot symbol section, inside the Figure field, change it from “Null” to “Cross”.
17. Then change both its Width and Height to 0.45 mm.
19
University of Arkansas
PCB Editor Flow Tutorial
Verify that your screen looks similar to below.
20
January 24, 2015
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
18. If everything looks good, go to File > Save As….
19. Save the file to the directory C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
20. Save it as “capth4mm.pad”.
21. Exit Pad Designer.
B. FOOTPRINT FOR THE THROUGH-HOLE CAPACITOR
Now to make the footprint for through-hole capacitor we just made.
1.
2.
3.
4.
5.
Go to Start > Programs > Cadence > Release 16.6 > PCB Editor.
Go to File > New.
In the New Drawing window, type the drawing name “capth4mm.dra”.
In the Drawing Type field, select Package symbol (wizard) from the list.
Make sure the Project Directory is located in
C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
6. Once this is all confirmed, click OK.
7. Select SIP (single inline package) for the Package Type.
8. Once selected, click Next.
9. Have “Default Cadence supplied template” selected.
10. Click the Load Template button. A prompt will appear. Click Yes.
11. Hit Next.
12. In this Package Symbol Wizard – General Parameters window, change the units in both
fields from Mils to Millimeter.
13. In the Reference designator prefix field, type “CAPTH4MM*”.
14. Click Next.
15. In this window, Package Symbol Wizard – SIP Parameters, use the following values:
Parameter
How to calculate
Value (mm)
Number of pins (N)
Same as number of capacitor 2 pins
leads
Lead pitch (e)
e = lead space F
1.500
Package width (E)
E = ϕD (datasheet)
4.000
Package length (D)
D = E = ϕD (datasheet)
4.000
16. So your screen should look like below.
21
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
17. Click Next.
18. Click the
button in the field “Padstack to use for pin 1:”.
19. Choose “Capth4mm” from the list, then click OK.
20. Click Next.
21. The defaults choices in the new window are fine so click Next, then click Finish.
Your footprint will show up and look like the picture below.
22. Save “CAPTH4MM.dra” to the C:\...\symbols folder you were using already (should
already be selected).
23. You may be asked to overwrite the already existing file. Choose Yes.
24. Close PCB Editor.
2.2.3 Through-hole Transistor
A. PADS FOR THE THROUGH-HOLE TRANSISTOR
We will use the through-hole transistor 2N3904 with ‘ammo pack’ lead adjustments. The ‘ammo
pack’ is different from standard leads, because the end leads are now crimped, whereas they
normally would not be. The exact package type looks like below:
22
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
The pads for the transistor can be made similar to the capacitor pads.
1. Go to Windows Start > All Programs > Cadence > Release 16.6 > PCB Editor Utilities >
Pad Designer.
2. Go to File > New. In the New Padstack window, type a suitable name in the Padstack
Name field (e.g. 2N3904AMMO.pad).
3. Click OK.
4. In the Pad Designer window, change the Units field to Millimeter (select Yes when
prompt about accuracy appears).
5. Select the Layers tab. Make sure Single layer mode is unchecked.
6. Ensure that the Views section has XSection selected instead of Top.
7. Click on the
layer button.
8. In the Geometry field, select Circle.
23
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
9. Change the Width field value to 1.23 mm (a little less than half the pseudo average
distance between transistor leads).
10. The height changes automatically and a bar (red or blue) shows up in the diagram.
11. Click on the
button then repeat steps 8 through 10.
12. Click on the
button next to Default Internal and repeat steps 8 through 10.
13. Click on the Parameters tab. You will see a filled yellow circle.
14. In the section Drill/Slot hole, in the field Hole type, you should see “Circle Drill”. If not,
then change it to Circle Drill.
15. Change the field “Drill diameter” value to 0.7640 mm because that’s the hypotenuse of
the length and width of each lead (0.52 mm by 0.56 mm).
16. In the Drill/Slot symbol section, inside the Figure field, change it from “Null” to “Cross”.
17. Then change both its Width and Height to 0.5600 mm.
Verify that your screen looks similar to below (the colors may not match exactly).
24
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
18. If everything looks good, go to File > Save As….
19. Save the file to the directory C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
20. Save it as “2n3904ammo.pad”.
21. Exit Pad Designer.
B. FOOTPRINT FOR THE THROUGH-HOLE TRANSISTOR
Now to make the footprint for through-hole transistor we just made.
1.
2.
3.
4.
5.
Go to Start > Programs > Cadence > Release 16.6 > PCB Editor.
Go to File > New.
In the New Drawing window, type the drawing name “2n3904ammo.dra”.
In the Drawing Type field, select Package symbol (wizard) from the list.
Make sure the Project Directory is located in
C:\Cadence\SPB_16.6\share\pcb\pcb_lib\symbols.
25
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
6. Once this is all confirmed, click OK.
7. Select ZIP (zig-zag inline package) for the Package Type.
Important Note: we could have chosen SIP packaging, however, soldering the pins while
all in a single row would be difficult for such a small spacing between leads. So, we are
staggering the spacing between the leads to make soldering them easier.
8. Once selected, click Next.
9. Have “Default Cadence supplied template” selected.
10. Click the Load Template button. A prompt will appear. Click Yes.
11. Hit Next.
12. In this Package Symbol Wizard – General Parameters window, change the units in both
fields from Mils to Millimeter.
13. In the Reference designator prefix field, type “2N3904AM*”.
14. Click Next.
15. In this window, Package Symbol Wizard – ZIP Parameters, use the following values:
Parameter
How to calculate
Value (mm)
Number of pins (N)
Same as number of leads
3 pins
Lead pitch (e)
e = lead space 2-3
2.80 (maximum)
Terminal row spacing (e1)
Suitable soldering space
2.80
Package width (E)
E = thickness of transistor top 4.19 (maximum)
Package length (D)
D = width of transistor top
5.20 (maximum)
16. So your screen should look like below.
17. Click Next.
18. Click the
button in the field “Padstack to use for pin 1:”.
26
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
19. Choose “2N3904ammo” from the list, then click OK.
20. Click Next.
21. The default choices in the new window are fine so click Next, then click Finish.
Your footprint will show up and look like the picture below.
22. Save “2n3904ammo.dra” to the C:\...\symbols folder you were using already (should
already be selected).
23. You may be asked to overwrite the already existing file. Choose Yes.
24. Close PCB Editor.
Now that we have finally created the pads and footprints for all our parts, we can implement the
astable multivibrator circuit design in OrCAD Capture CIS.
27
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
3. Circuit Design in OrCAD Capture
In this part of the tutorial we will cover:


How to convert a new OrCAD Capture project from Analog Design/Schematic to a PCB
Editor board
How to correctly annotate schematic components so they match with the PCB Editor
layout
3.1 Schematic Creation and Simulation
First we will create the new analog design/schematic in OrCAD.
1. Go to Start > Programs > Cadence > Release 16.6 > OrCAD Capture CIS
2. Select the top-most version of OrCAD Capture CIS if prompted.
3. Check mark Use this as Default if you would like.
4. Go to File > New > Project…
5. Type whatever name you want for the project
6. Select “PC Board Wizard”
7. In the Location field, click Browse and choose any folder to store the project.
8. Click OK.
9. In the new window, check “Enable project simulation”.
10. Choose the option “Add analog or mixed-signal simulation resources.”
11. Click Next.
12. Another window will show up asking which PSpice Part symbol libraries you will use.
13. Enough libraries (shown below) should already be loaded by default.
14. We should add 2 more libraries at this point. Select “eval.olb”, click Add>>. Also select
“EVALAA.OLB”, click Add>>. Then click Finish.
15. If those libraries existed for you to add, your window should look like below.
Note: standard resistors and capacitors are in the ‘analog.olb’ library. The transistor is called
Q2N3904 and is located in the “eval.olb” library.
28
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
16. Create the circuit below.
R1
5k
R2
470k
V+
R3
470k
C1
C2
0.47uF
0.47uF
R4
5k
V-
V1
6Vdc
Q1
Q2
Q2N3904
Q2N3904
0
Note: to draw straight lines at an angle from the capacitors C1 and C2, go into Wire mode, hold
down the Shift key then click on the start node. Move your cursor to the end point while still
holding down the Shift key and click (or double-click) your end node to terminate the wire
connection.
17. Create a Transient Simulation profile.
18. Have the run time equal 2 seconds with a 0.01 second step in the “Maximum step size”
field. This will ensure it begins to oscillate properly.
19. Once the simulation profile is set up, place a Differential Voltage probes at the outputs of
the circuit (just below the 5 kΩ resistors).
20. Run the simulation.
21. The wave should look something like this:
6.0V
5.0V
4.0V
3.0V
2.0V
1.0V
0V
-1.0V
-2.0V
-3.0V
-4.0V
-5.0V
-6.0V
0s
50ms
V(Q1:c,C2:2)
100ms
150ms
200ms
250ms
300ms
350ms
400ms
450ms
500ms
550ms
600ms
650ms
700ms
750ms
800ms
850ms
900ms
950ms
Time
You can do a Fast Fourier Transform (the
frequency of 3.12 Hz.
button) to make sure it oscillates at the right
29
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
6.0V
5.0V
4.0V
3.0V
2.0V
1.0V
0V
0Hz
2Hz
V(Q1:c,C2:2)
4Hz
6Hz
8Hz
10Hz
12Hz
14Hz
16Hz
18Hz
20Hz
22Hz
24Hz
26Hz
28Hz
30Hz
Frequency
The other peeks are normal harmonics that occur when generating a wave.
3.2 Getting ready for PCB
Now that we verified our circuit behaves correctly, we need to prepare it for PCB layout. This
means we’ll remove ground and source and replace them with jumpers. When you’re doing your
own project, you will know what kind of connector you will have for power, output, etc. Power
and ground connectors will also need footprints designed for them. For basic headers, there is
already footprints made for them.
Jumpers and connectors are in the connector library and are not loaded by default.
1.
2.
3.
4.
Close the PSpice simulation window if it is still open.
In OrCAD Capture, go to Place Part, then go to Libraries section.
Click on the Add Library button .
If you’re in the “pspice” directory, go up one directory and select the “Connector.olb”
library to Open.
5. With the Connector library now selected (or all libraries if you’d like), type “CON2”.
30
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
6. Press Enter and place two copies of that part onto your schematic design. One
connector for the Vdc and ground pins. The other connector for the output nodes.
Your schematic should now look like this:
R1
5k
R2
470k
R3
470k
C1
C2
0.47uF
0.47uF
R4
5k
J2
1
2
J1
CON2
1
2
Q1
CON2
Q2
Q2N3904
Q2N3904
3.2.1 Assigning Footprints to Parts
31
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Now we will set the footprints for each of the components using footprints we made in Section 2
of the tutorial and some pre-made footprints.
1. Select all components on the schematic by either dragging your cursor across all of
them or typing Ctrl + A.
2. Go to Edit > Properties… (Ctrl+E).
3. On the bottom tabs, select Parts tab.
4. Use the bottom scroll bar to move over to the right of the list where you see a column
named PCB Footprint.
5. Change the values of the names in PCB Footprint to the appropriate footprints for each
part.
6. In this tutorial the footprints we created for each part are shown in the table below.
REFERENCE
PCB Footprint
C1
capd16v
C2
capth4mm
J1
jumper2
J2
jumper2
Q1
npnsot23
Q2
2n3904ammo
R1
rc0603
R2
res500
R3
rc0603
R4
res500
7. Make sure you have a surface mount footprint for each resistor, capacitor and transistor
and a through-hole footprint for each resistor, capacitor and transistor.
8. Save your project.
32
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
3.2.2 Annotation of parts
Finally, we must annotate all parts in case the names for all the parts are out of order (Note: this
is not necessary if you’ve placed the names intentionally in an order you like).
1. Go to the Project window then select the projectname.dsn* file from the list as shown
below.
2.
3.
4.
5.
Right click the project file and a dropdown menu will appear.
In the drop-down, click Annotate….
Choose the “Reset Part References to “?”” radio button.
Adjust all settings shown in the figure below then click OK.
6. A prompt appears asking if you wish to continue. Click OK.
33
University of Arkansas
PCB Editor Flow Tutorial
7. In the project window, select the Hierarchy tab
8. All parts have a “?” symbol next to them.
January 24, 2015
.
9. To correct this, you may either rename the parts to whatever you like or…
10. Go to back to the File tab (right next to the Hierarchy tab), right click the .dsn file name
again and click “Annotate” from the dropdown menu.
11. But this time, select “Incremental reference update” radio button. Click OK.
12. Click OK when the prompt asks you to continue.
13. Your schematic will look like below.
R1
5k
R2
470k
R3
470k
C1
C2
0.47uF
0.47uF
R4
5k
J1
1
2
J2
CON2
1
2
Q1
CON2
Q2
Q2N3904
Q2N3904
Note: Ensure that no parts have the exact same name. If two parts share the exact same name
you will have issues during layout.
3.2.3 Creating the Netlist
Now that the schematic is ready for PCB Editor we need to create the netlist and connect the
PCB we’re going to create with the higher level OrCAD schematic.
1. While still in OrCAD Capture, go back to the Project files window and right click on the
project .dsn file.
34
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
2. Go to menu Options > Preferences > Miscellaneous tab.
3. Check mark “Enable Intertool Communication” in the section named “Intertool
Communication”.
Note: This option allows OrCAD to highlight the same components in both OrCAD and PCB
Editor whenever you select a part in either program.
4. Now go to menu Tools > Create Netlist…
5. In the Create Netlist window, click Setup button
.
6. Ensure that the correct path is in the field named Configuration File. The path should
read “C:\Cadence\SPB_16.6\tools/capture/allegro.cfg”.
7. Confirm this then click OK.
8. Back in this Create Netlist window, check mark “Create or Update PCB Editor Board
(Netrev)”.
9. Under the section Board Launching Option, select the “Open Board in Allegro PCB
Editor” radio button.
10. Your window should look like this.
35
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
11. Click OK and the software will ask if you want to continue. Click Yes button.
12. If you did everything correctly, OrCAD should generate the netlist and you’ll just wait
until it tries to open it in Allegro PCB Editor.
13. A window may show up asking with Allegro PCB Design product to use. Select Allegro
PCB Design L (legacy) or Allegro PCB Designer (was Performance L). Click OK.
PCB Editor will open up with a blank project.
TIP: Sometimes you have to make changes to the PCB layout in PCB Editor and find yourself
having to go between Editor and OrCAD Capture. This usually happens if you find you have the
wrong part or wrong footprint for a part. To manage these issues, use the Input Board File,
Output Board File fields. To use this feature correctly:




Save your layout in PCB Editor (which needs correcting) then exit PCB Editor.
Make any corrections necessary in your schematic in OrCAD Capture.
When you go to Create Netlist again, choose your Input Board File location to be the
layout board that needs correcting.
Choose your Output Board File to be a new board that will have the corrections (if you
choose the input and output boards to be the same file, OrCAD will overwrite the
incorrect board with the updated corrected board).
36
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
4. PCB Editor Design Layout
In this section you will learn how to set up PCB editor for:




Spacing your board traces
Sizing the holes on the board
Laying out parts
Routing the parts together
4.1 Setting the Environment
The first step is to set up the environment behavior and parameters. The minimum spacing
should be smaller than most the components so one can move at the finest resolution when
placing parts. We also want to set the default constraints.
1. In PCB Editor, go to menu Setup > Design Parameters.
2. In the Design Parameter Editor window, select the “Setup Grids” button.
3. In the TOP and BOTTOM areas, set the Spacing, x:, y: fields to 10.00 (or even 5.00 if
you’d prefer) for all of them.
4. Do the same for the ALL ETCH area in its respective x and y fields.
5. Check mark Grids On.
6. Leave the Offset fields at 0.00. Your window should look like this:
7. Click OK out this window.
8. Next, change the user units back in the first window by going to the Design tab.
9. Change the “User Units” field to “Mils” and the “Size” field to “A” with accuracy of 2.
37
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Your screen should look like this:
10. Click “Apply”, then go back to the Display tab and check mark “Grids On” if it’s not
checked.
11. Then click Apply in that window, too (if the option is there). Then click OK.
4.2 Setting the Design Constraints
When using the milling machine to mill out PCBs it is important to make your traces and spacing
larger than the minimum tool sizes of the machine. You will also set the size for your VIAs.
1. Go to menu Setup > Constraints > Physical…
2. Set the DEFAULT, Line Width column Min value to 20.00 – 30.00 mil (30 is easier to
solder onto).
3. Set the Neck column Min Width value to 10.00 mil. These settings are shown below.
38
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
4. In the Worksheet Selector section on the left pane of this window, select the “Spacing”
section.
5. Expand the Spacing Constraint Set section, then expand the All Layers section.
6. Click the “All” section.
7. Click on the DEFAULT row on the right window so that the entire default row is
highlighted.
8. Right click the highlighted DEFAULT section and in the dropdown menu, select “Change
all design unit attributes”.
9. Type 20.
10. Click OK.
11. All the fields should show 20.00 (mils).
Note: to learn more about how to select minimum spacing for your design projects see the 9.
Appendix.
4.2.1 VIAs
39
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Vias connect layers together. With a two-layer board, they are simply holes. We will use a small
piece of wire to connect a trace on the top to the bottom. By default, PCB Editor uses a hole
size that is incredibly too small to use. We will correct this later.
1. In the same Constraints Manager window go to Physical section > Physical Constraint
Set > All Layers.
This project
already had its
“Vias” section
corrected to
“VIA26”
2.
3.
4.
5.
6.
7.
Click on the default row under the Vias column.
A new Edit Via List window will show up.
Under the “Via list” select the VIA part then click the Remove button.
Scroll down the list to the “VIA26” item.
Double click VIA26. It should be the only via in the Via list on the right now.
Your window should look like this
8. You must click the OK button for this change to take effect.
9. Your previous window will now look like this
10. Exit Allegro Constraint Manager
4.2 Creating the Board Outline
40
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
This is a relatively simple design so we will use a small board. We’ll make a 2 in. × 2 in. outline.
1. In PCB Editor go to menu Shape > Rectangular.
2. On the right side of PCB Editor, hover over the Options tab. The tab will jut out.
3. Make sure that the Active Class and Subclass field says “Board Geometry” and that the
field below that says “Outline”.
4. Once that is confirmed, move the cursor to coordinate 0.00,0.00 on the screen.
5. Left click once, then move the cursor to point 2000.00,2000.00 (the dimensions don’t
need to be this exact. Just a board around 2000 by 2000 mils is fine).
6. Left click again to finish the shape.
7. Right click the screen then left click “Done” on the drop-down menu to end Rectangular
Shape mode.
Note: In general, any time you initiate a mode of operation or function, you will have to right click
the work area then left click “Done” in order to end that mode.
4.3 Placing Parts
Now that we have the outline and planes set up, it is time to place the parts.
41
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
1. Go to menu Place > Manually…
2. You may or may not see all the parts listed.
3. Ensure that under the Placement List tab, you have “Components by refdes” selected.
4. Once that is confirmed, expand the Components by refdes list below that drop-down
field.
5. Left click the check box of the first part you would like to place. For us this is C1.
6. Click the Hide button on this window to hide the window.
7. The part will appear where your cursor is, waiting for you to click a location to place it.
8. Place the part in a location near the center of the board (like in your OrCAD design).
Tip: To make placing easier, zoom into the screen by scrolling up with the mouse. Scroll down to zoom
out. The computer zooms in to wherever the mouse cursor is at the time. To pan and navigate the screen
while trying to place parts, use the arrow keys on your keyboard.
Tip: The parts may not be oriented properly while you’re trying to place them. To re-oriented the floating
part before placing it:
1. Right click the screen.
2. Left click the “Rotate” option from the drop-down menu.
3. Move your cursor clockwise or counter-clockwise until you see the part rotate 90 degrees or
more.
4. Keep moving the cursor around until the part rotates to your liking.
42
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
5. Left click that spot when you want to stop rotating it.
6. The part is now rotated and will continue to move with the cursor until you place it by left
clicking the work area again.
9. Go to menu Place > Manually…
10. Repeat steps 5 through 8 until all parts are placed in locations similar to like in OrCAD
Capture.
11. Remember to right click the work area then select “Done”.
12. Your board might look like something similar below.
4.4 Routing the Board
After you’ve placed the parts you will need to route the parts together. This is where you set
your trace, which connect the parts together. All of the routing can be done manually but first we
will complete it using the Autorouter.
43
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
a. Go to menu Route > Connect.
b. This mode allows you to select the end of a part, move the cursor to another part, select
that end point and route those two points together.
c. Manual routing is one of the best ways to ensure parts are connected favorably.
d. For simpler designs however, autorouting works just as well.
e. So, right click the work area then select “Done” to get out of manual routing mode.
f. Go back to menu Route > PCB Router > Route Automatic…
g. Ensure that the “Smart Router” radio button is selected.
h. Then click Route. PCB Editor will take a moment then route the board.
44
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
When that is completed, some of the corners just seem a bit too sharp, lines are too close to
each other and a few other problems. To solve all these issues, go to 9.4 Routing Corrections
& Techniques and follow through each problem/section as necessary, then come back to these
instructions. Once you’re done correcting all the problems/warning areas, you’re ready to
continue.
i. Go to menu Route > Gloss > Parameters…
j. Make your settings like below
45
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
k. PCB Editor will update the traces like shown below (this image is just as an example.
The actual design in this tutorial is different and un’smoothed’).
The actual design for this project came out unsmoothed and looks like below:
46
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Notice the DRC (Design Rules Check) has red triangles
around two of the nets on the left
and between two pins in the center (at component C2). Depending on the error, there will be
letters placed in each triangle. In this case we have L-W, L-L and P-P for Line Width, Line to
Line and Pin-to-Pin, respectively.
These just mean that the widths and spacing between these components are smaller than what
was specified in the Design Parameters we made. If you know what you want your design to be
like, this may or may not be fine. For our project, these errors aren’t an issue.
TIP: While PCB Editor Autorouter is great, check to see how difficult it might be to solder around the
traces. There are a few checks you should make:
 That the Via holes (if any) are not close to the footprints for your parts). Move and delete the
traces as needed.
47
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015

That the traces themselves are not too close to the part footprints, as this may be a problem for
the diameter of the insulation tool during milling. The tool needs enough space to mill out traces
without disturbing other traces or footprints.
 That in general, there won’t be any spacing issues that can cause soldering issues.
TIP: Vias provide many issues if they are too small.
 In most cases, even the Via26 are far too small to find wires to feed through.
 Additionally, these Vias have a hole diameter of 13.00 mils only. This would be okay normally, but
the smallest drill bit in the Accurate CNC milling machine is 16.00 mils in diameter.
 We recommend changing the hole size of the Vias in Allegro PCB Editor.
Go to 9.2 Changing Vias dynamically before continuing with this tutorial.
Finally, maximize the space available on the board. There is a lot of space!
5. Gerber Files and Drill File
Now that we have completed our PCB, it’s time to create Gerber files for the machine milling.
1. In PCB Editor, go to menu Manufacture > Artwork…
You will notice that there are only two layers in the list, BOTTOM and TOP. You must create a
third layer for the outline of the circuit board so the Accurate CNC Milling machine can cut it out.
2. Right click on the layer that says “TOP”. Left click “Add Manual” from the dropdown list.
3. Type in the name “Outline” (the name is case-sensitive. If you type “OUTLINE”, the
software will not add a new folder like we intend to).
4. Click OK.
5. A new list will appear. Expand “Board Geometry”, then check mark the box that says
“OUTLINE”.
6. Click OK then you will return to the Artwork Control Form window.
7. Click on BOTTOM, then under the Film options area on the right, change the value in the
field “Undefined line width” from 0.00 to 10.00.
8. Repeat this change from 0.00 to 10.00 for each of the folders on the left (‘Outline’ and
‘TOP’).
48
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
5.1 Creating Apertures
1. Back in the Artwork Control Form window, click the Apertures… button near the bottom
of the window.
2. An Edit Arpeture Wheels window appears.
3. Click the Edit… button under the area of this window called Operations.
4. In the Edit Aperture Stations window that appears, click the Auto-> button.
5. Click “Without Rotation”.
6. This window will then populate the list with new information.
7. Click OK.
8. Click OK again.
9. In the Artwork Control Form window, check mark each layer: BOTTOM, TOP and
Outline.
10. Click the Create Artwork button and it will show its status in a smaller window and create
the artwork Gerber files.
49
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
5.2 Creating the Drill File
The drill file is very important because it dictates how the milling machine will drill holes into the
PCB. Let’s create the frill file.
1. Go back to menu Manufacture > NC > NC Parameters.
2. Change the settings so the:
a. Leader field is 12
b. Code is ASCII
c. Under Excellon format: Format is 2 . 5
d. Checked “Leading zero suppression”
e. Checked “Enhanced Excellon format”
f. Coordinates: Absolute
g. Output units: English
3. Verify that your window looks like the above settings then click the
button.
4. Go to menu Manufacture > NC > NC Drill….
5. In the NC Drill window make sure you have these settings:
a. Some correct root file name in the same directory as the ‘allegro’ folder where
your project is stored (this should automatically be done for you)
b. Scale factor: 1.00
50
University of Arkansas
c.
d.
e.
f.
PCB Editor Flow Tutorial
January 24, 2015
Tool sequence: Increasing
Check “Auto tool select”
Check “Optimize drill head travel”
Under Drilling, select “Layer pair”
6. When the settings are like above, click
(drill).
7. A file named ‘projectname-1-2.drl’ will be made in the project’s allegro folder
5.3 Checking the Gerber Files
It is easier to check your design before you schedule milling machine use.
1. Go to Accurate CNC’s Demo Software page to download the software if you don’t
already have it on your work station.
2. If you don’t have security access to install software on your computer, email
[email protected] and we’ll get it installed for you.
3. Download and install the software on your work station.
4. After it is done installing, launch the demo software.
5. Click the Import Gerber button
in the upper left corner of the software.
6. Browse to your project location.
51
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
7. Copy your Gerber files (OUTLINE.art, BOTTOM.art, TOP.art, boardname-1-2.drl) from
your project’s “allegro” folder into a separate folder so they are easier to find and work
with.
8. Select the .drl drill file in the Gerber & Drill Import window. It will appear in the Layers
section on the right.
9. Check the box that says “Top” and a new window will appear like below. “Top” here
specifies that drilling will be done through the top layer of the board.
10. You will now need to specify the drill settings. These are the same settings used earlier
when we made the drill file (recall that in PCB Editor went to Manufacture > NC > NC
Drill Parameters…).
11. Sometimes clicking the “Auto detect” button will work as well.
12. Click OK when the settings look correct.
13. Now back in the Gerber & Drill Import window, click once on the TOP.art file. It shows up
on the right window. Check mark the box that says TOP
14. Select the BOTTOM.art file and check mark BOTTOM on the right for that file.
15. Select the Outline.art file and check mark “Mech” (for mechanical).
16. Finally, click the
button on the upper right portion of the screen
52
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Your board will look similar to this board below (with no warnings).
We want to make sure the board looks right before using the milling machine. You can click the
button in the upper right of the above window to look at the different layers and see if
they will mill out properly. Also click on the
button to see the copper view and what the
53
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
board is supposed to look like once the machine is done milling. The Bottom views are available
also. It looks like the board will mill just fine.
Now that it looks correct, you are ready to use the milling machine.
6. Milling the PCB
6.1 Training & Scheduling
Before you use the milling machine you must be trained. This part of the project can be a
substitute board for when you’re about to complete training on the milling machine.
The milling machine instructions are in a separate tutorial located on the desktop of the
computer connected to the milling machine and on the ELEG Help website link found
here [3]. The computer and milling machine are located at the University of Arkansas in White
Engineering Hall Room 115.
You must request a time to use the milling machine according to the instructions found here.
Never use the milling machine without requesting a time as per the instructions. If you’ve
found to be using the machine without being scheduled, all privileges and use of the machine
will be revoked.
All milling must be done between 8 AM and 5 PM Monday through Friday. To see when there
are available times for training or milling, go to the Milling Machine Calendar. You cannot edit
this calendar.
6.2 On Making an Appointment
Appointments are absolutely mandatory in order to use the milling machine. When you request
an appointment:



Be aware that you must be trained in order to use the machine, so your very first
encounter with the machine will be for training purposes only. There are no exceptions.
Request a time that isn’t already taken
Make sure to include your EE Design/Research Group name, day and time.
54
University of Arkansas






PCB Editor Flow Tutorial
January 24, 2015
Request 2 times/dates…Your first preferred time and date, then your second available
time and date.
Know that a training session typically takes 2 hours.
There are several people who use this machine.
A document must be signed before and after you go through training on the milling
machine.
Once all the information you need (group name, 2 preferred training times/dates) is in
your email, again, send it according to the instructions found here.
Once you receive confirmation of your requested time/date, put your 4 artwork/Gerber
files on your Tesla network drive or a USB flash drive.
7. Soldering the Parts to the PCB
Soldering requires some practice to get good at, but the better your soldering skills, the cleaner
your circuit design and the less likely there will be errors.
Solder surface mount parts first then through-hole parts afterward!
For instructions on how to solder surface mount parts and regular parts:
Solder Surface Mount Parts with Hot Air (Use the hot air gun on the SMD workstation in the
back of EE Design lab)
More on Surface Mount Soldering
Soldering Tutorial
8. Verification
Connect the power and test points (via power supply and oscilloscope, respectively). Verify on
the o-scope the 3.2 Hz square wave. Capture the waveform using OpenChoice Desktop on a
Windows computer that has the oscilloscope connected to it via USB.
9. Appendix
9.1 Minimum Spacing Guidelines for PCB Layout
When working on your design project, voltage and current decide the spacing widths. In the
case for this tutorial, 20 mils is one of the easier settings to use for the Accurate CNC 427
milling machine. The smallest separation that can be done in the ENGR 115 lab is 10.0 mils.
You can find more trace width information on trace widths here.
9.2 Changing Vias dynamically
In most cases the vias are too small, even the Via26. To correct this and make soldering and
wiring easier, follow these instructions (alternative ways are found in this video).
1. In Allegro PCB Editor, right click on the work area for your board.
2. Go to Super Filter > Via
55
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
3. This option allows only the selected layer (Via in this case) to be click-able, so you’re
not clicking on multiple things when working.
4. The via in the picture above may have a hole size larger than yours because ours is
already updated from the default (default hole: 12.00 mils to new hole: 16.00 mils).
5. Once in Superfilter Via mode, right click on the Via26 hole, then go to Modify Design
Padstack > All Instances.
6. The Padstack Designer: Editing Pad Definition VIA26.pad window will appear.
7. Change your pad settings to suitable settings, like a drill hole size that’s at least
16.00 mils (You’ll have to change the units from millimeters to mils)…larger if you
would like to run a wire more easily.
For this astable multivibrator circuit, we changed both the pads and drill hole size for the VIA26
because simply increasing the hole size would have left very small pads to solder some
through-wire to.
The changes are like what are shown below.
56
University of Arkansas
PCB Editor Flow Tutorial
57
January 24, 2015
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
If you are satisfied with your custom settings (or if your settings are similar to above), then
8. Go to File > Update to Design and Exit.
9. If there are no problems, Pad Designer will close then take you back to PCB Editor
and all your VIA26 vias will be updated for the entire design!
This can pose a problem if your traces are too narrow, however. To correct trace widths, look at
9.3 How to adjust trace widths.
9.3 How to adjust trace widths
Sometimes when routing, you’ll need to change your trace widths. To do this in PCB Editor:
1. Go to menu Route > Connect (F3) to go into Route mode.
2. In the “Options” menu on the right of the screen, change the “Line width” field to
whatever line width you want.
3. Note that if the line width changes to blue, then the width is less than what you put in
your constraints. Sometimes this can just be ignored if you know that small a trace is
not a problem for your design.
4. Drop your line with the appropriate length and make your connection. See the
images below to get an idea of what we mean.
9.4 Routing Corrections & Techniques
9.4.1 Crooked Lines
When routing, avoid crooked lines. Make as many straight connections or 45° angle
connections as possible. When we did automatic route, we got this:
58
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
Let’s straighten up these connections:
1. Right click on one of the nets (N00217 in this example) then choose Delete from the
dropdown menu.
2. Delete as many unwanted nets as you see fit until no connections are made between
the top hole of the PWR connector and the top hole of the R4 resistor.
3. Reposition the R4 resistor so that it’s perfectly in line with the PWR connector’s top
connector/hole.
4. Then go to menu Route > Connect (or press F3) and click.
5. You’re now in connect mode, so click once on the PWR connector’s top
connector/hole, then carefully move the mouse over to the R4 connection.
6. There should be no strange red DRC symbols if you’re in the correct location (dead
in the center of the R4 connector).
7. Click on that R4 resistor connector once to complete the connection.
8. Your circuit connection should now look like below.
9. Repeat this procedure until as many parts are lined up nicely as possible.
10. However, this isn’t the only way to connect parts. You’ll have to smooth some
corners, which is next…
9.4.2 Making Angled Connections
It is usually better for a printed circuit board milling machine to make 45° turns and to go straight
across to a part (hence the previous section on making straight connections).
To make an angled connection, simply click once in some open area while you’re making a
trace. The click will make an angle and you can continue making traces.
59
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
9.4.3 Creating a Part
A ‘part’ in Cadence is a block with input and output pins having a footprint associated with it. It
has no simulation/model information and is used solely for going from schematic to PCB Editor.
Let’s say you’ll be making an operational amplifier chip containing 4 op-amps. Typically it is a
part that has 14 pins and an associated 14-pin footprint. If you have 4 op-amps in a circuit, you
can replace the 4 op-amps with a single new part that you will create.
Note: You must already create a footprint for each of the parts being placed inside your new
part.
1. In OrCAD 16.6 in an open project go to menu File > New > Library.
2. You will see a new library called “library2.olb”. (Belwo shows “library3.olb” but that’s fine)
3. Right click on the library file and choose “Save as..” from the dropdown menu.
4. Save this library2.olb file anywhere on the computer (or on a network drive).
5. Once the file is saved, right click on Library2.olb then choose “New Part”.
60
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
6. Name the part something meaningful and simple, like “quadopamp”.
7. The part reference prefix is what the schematic will name the part number when you
place it.
8. For the PCB footprint field type the name of the footprint you already have created.
9. For “Parts per Pkg:” field, type in the number of parts you’ll be including in your created
part. In this case, type 4 because this part will have 4 operational amplifier parts.
10. For the “Package Type” section:
a. If your part has all one type of part, e.g. all opamps, then it’s Homogenous.
b. If your part has different items in it then it’s Heterogenous.
11. Once your settings are good, click “OK”.
12. You’ll be presented with something similar to the image below.
13. Go to menu Place > Rectangle then draw your rectangle over the same area as the
dotted lines.
14. Right click the work area then choose “End Mode”.
15. How you draw the part depends on the number of pins your part has.
16. This part has 14 pins, so it is somewhat large (image above on the right).
17. Grab the data sheet for your parts going into this larger part, because the pin numbers
should be matched what you used for this larger part’s footprint.
18. Go to menu Place > Pin.
19. Name each pin as depicted on its datasheet. Keep the number of the pin the same.
20. Ensure you have the correct pin Type, Name, Shape, Number and Width.
21. Make input pins of Type Input and output pins of Type Output.
22. For power pins, make sure it has Pin visible check-marked or you won’t be able to attach
it to anything on your schematic when the part is finished being made.
23. You should end up with something similar to the picture below.
61
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
24. It has only 8 pins in the image above, but you get the general idea.
25. Save the part by going to menu File > Save.
26. Go back to your schematic/project you want to place your new part.
27. Click on the Place Part button in the area shown:
28. Clicking on that button will allow you to add a new library file.
29. Add the library you just created (Library#.olb). It will be in the same folder you created
the project (not in the directory where the other standard libraries are located).
30. Once the library is added, you’ll be able to see your part.
31. Add it to your design.
62
University of Arkansas
PCB Editor Flow Tutorial
January 24, 2015
10. References
[1] W. Storr, “Astable Multivibrator and Astable Oscillator Circuit,” Basic Electronics Tutorials.
[Online]. Available: http://www.electronics-tutorials.ws/waveforms/astable.html. [Accessed:
03-Apr-2015].
[2] “Senior Design Circuit Plan and Tutorial.pdf.” [Online]. Available:
http://elegfiles.uark.edu/Milling%20Machine/Senior%20Design%20Circuit%20Plan%20and
%20Tutorial.pdf. [Accessed: 03-Apr-2015].
[3] “Accurate CNC 427 Manual - Accurate CNC 427 Quick Start Guide.pdf.” [Online]. Available:
http://elegfiles.uark.edu/Milling%20Machine/Accurate%20CNC%20427%20Quick%20Start
%20Guide.pdf. [Accessed: 03-Apr-2015].
[4] storm, “Tutorials,” 25-Apr-2014. [Online]. Available: http://www.orcad.com/resources/orcadtutorials. [Accessed: 03-Apr-2015].
63