Hardware
Design Flow:
Hardware design is very crucial in Electronics Product
Design, if we have any errors (Shorts or Open) in the design then it will lead
to till the product end. So each and every step in hardware circuit design
should be monitored for error free designs.
All the circuit hardware designs
will get through the following process.
•
Creating Block Diagram for the Product
Here, we will have all the blocks
involved in the product say, Power supply, Processor, Memory, Interfacing
connectors like USB and all other circuit blocks, by this way we can get the
possibility to check what is missing, how they have been connected, where the
signal is coming from whether its bi-directional or not. Block diagram also
will help us to troubleshoot the circuit.
•
Splitting up the big circuit design in to blocks
By this way, we can concentrate only
on one section at a time and start creating circuit for that section alone, so
we can get it done correctly without any errors.
•
Merging all different block circuit and complete the whole
circuit design.
•
Checking the design for shorts and opens.
•
Generating the output to be given to the next level process.
Schematics
circuit design flow:
All the
circuits have been created only in PC by using design software and the company
decides to choose the software to be used and all it is depend on customer and
their country.
The Major
processes in both Schematics and PCB Layout design are similar, but under these
there may be some sub process to complete the design.
Schematics design PCB
design
•
Library Creation Footprint
Creation
•
Placing Symbols Placement
•
Wiring Routing
•
DRC Check DRC Check
•
Generating Outputs Generating
Outputs
Library
Creation:
This
is the first very basic step in the schematics design, here we will create
symbols or parts to be used in our design like ICs, connectors and all the
required parts.
Tool might have some default parts
in their Inbuilt Library like Resistors, Capacitors, Inductors, Diodes,
Jumpers, Headers and some small pin count ICs and some large pin out ICs even,
we can directly use those if that fits with our design, if not we have create
it and use.
Symbol or part creation generally
will be in two types.
•
Homogeneous Parts
•
Heterogeneous Parts
Homogeneous
parts
Homogeneous parts are like small pin
count ICs say 10pins, 20 pins and all pins can be grouped and accommodate it in
a single diagram. And there is a general rule of thumb to group and create
Homogeneous parts. We can create Homogeneous parts for maximum pin count IC of
100, if it contains more pins in Homogeneous part then we will lose that
readability and the schematics circuit will look wired
The Homogeneous pins will be grouped
in to four types and they will be placed at default location in the symbol
diagram. Pin groups will be,
•
Power Pins
•
Ground Pins
•
Input Pins
•
Output Pins
By this way of creating symbols or parts for ICs, it will be
easy to create schematic circuits and it will be easy to read or study the
schematics and more over the schematics will look neat and clean. So by simply
seeing any schematics designed by others, we can say Inputs are coming to the
ICs from left side of it and Outputs are going to other ICs from the right side
of it and power and grounds are connected to it at top and bottom sides.
There are more other types of pins and they are,
•
Bidirectional
•
Open collector
•
Open Emitter
•
3 state
•
Passive
•
Configuration Pins
•
Clock Pins
•
Control Pins
•
Command Pins
•
Data Pins
•
Address Pins
•
No Connect Pins (NC)
•
Reserved Pins
Heterogeneous
Parts
These are
parts which will be created for ICs have more pin count like 512 pins BGA, in
this part creation we have to group the pins first as per the functionalities
and have to create symbol diagram for each pin groups separately like one for
Power pin group, one for Ground pin group, one for Data pin group and so on by
splitting the whole IC symbol into many. So this will be also called as Split
parts.
By using Heterogeneous parts, we can reduce the symbol size
and so by reducing the complexity in reading of schematic circuits. We can
place these split parts where ever required and make connection thereby we will
have clean and neat readable schematics circuits.
Here, the single 512-BGA IC has been split into 3 parts and
hence its called as Heterogeneous part. Lets say like, U1 has been split into
U1-A, U1-B & U1-C.
We can have more split parts for an IC based on the pin
groups and the pin counts. The split parts can be suffixed either by letter as
like above U1-A, U1-B & U1-C.or by numbers U1-1, U1-2 & U1-3.
Notes on Library creation
•
The symbol should be either Homogeneous or Heterogeneous.
•
Each pin on every symbol should have unique name and number
like
VCC1 – 1
VCC2 – 2
CLK – 3
DATA – 4
IO – 5
It should not have same name and
number for two or more pins
VCC – 1 CLK – 3
VCC – 2 DATA – 3
•
It should have Reference Designator (Ref Des) like U, R, C,
J, D
•
It should have PCB Footprint name like DIP20, SOIC-32, R0603
•
It should contain name or part number or value to represent.
•
Important thing is, GRID should be enabled in the TOOL while
creating parts, otherwise the created symbol could not sit on the GRID in the
schematic page and its pin will not get connected with the wire to make
connection. This should be checked always.
Library Creation Flow:
•
Add rectangle
•
Place Pins (Either by single or by Array)
•
Name and number the pins
•
Assign Pin Type
•
Save the Library
If we assign pin type as POWER then the name of the pin will
be act as net name and it get connected automatically in schematic design when
we use this symbol or part.
Let’s say, if we assign type for the pin VCC1 – 1 as power
then pin 1 will connect to pins of other ICs directly which have the same name
as VCC1. And if we connect the same pin with other signal or net say 3.3V then
we will get an error of saying that VCC1 & 3.3V got shorted.
Schematic
Page Order:
Once all the required Library Symbols or parts have been
created, it has to bring in to the schematics circuit design tool and place it
as per the Block say if it is Memory block and their symbols have to be placed
and wiring (Connection) should be done.
All our schematics circuits will be created on more number
of pages based on the blocks being used, so we have to follow some sort of
ordering format to arrange these pages. This arranging format will give clear
understanding of the Whole Product design by seeing itself.
•
Title Page
•
Block Diagram
•
System Power Supplies
•
FPGA Power Supplies
•
FPGA Configuration Circuits
•
FPGA Bank IO 0-1
•
FPGA Bank IO 2-3
•
Memory Power Supplies
•
Memory Data Bank
•
Memory Address Control Circuits
•
•
•
•
Interfacing Connectors
Schematic
Design Terms:
Net:
This is referred to the connections between two or more
pins. Example, U5.5, U5.7 & U10.3 got connected
Net Name:
This is referred to the name of the NET. Example “Data1”
Net Alias:
We can connect two or more pins by assigning name to it.
Refer “Data1” in the following. It will connect with the same name within a
page. And it is mainly used to avoid confusing connection by using wires and
directly connecting, refer connections U5.2 & U10.1
If we didn’t assign any Net name then system will assign it
automatically by start with N series number like N0000343.
BUS:
Bus means a group of signals named under a common name. The
some examples of bus are,
•
Address Bus
•
Data Bus
•
Control Bus
“Data{0..7}” means contains 8 different signals in one
common name.
•
Data0
•
Data1
•
Data2
•
Data3
•
Data4
•
Data5
•
Data6
•
Data7
Either we can use “Data{0..7}” or “Data{0:7}” to denote bus
name.
Netlist:
This is list containing information of all available nets
and all available parts in that particular schematic design.
U2 DIP-08
U5 SO-08
U10 SOIC-08
Data1
U2.4, U10.5
N0000343
U5.5, U5.7, U10.3
.
It is very important to remember “ALWAYS GRID SHOULD BE
ENABLED” before starting circuit design or even work on the Library and
schematics.
In order to make connection between two or more pins on two
or more schematic pages, we have to use “off page” to make connection, it will
also work like” Net Alias” but connect between different pages. Refer U10.7
“Data2”. Net Alias will only work within the page.
Power and Ground connection will be made only by using the
appropriate GLOBAL symbols, by using this; we can make connection between two
or more pins on same the page and also between different pages. Refer the
connections at U2.5 & U10.8
Intersheet Reference is used to provide the information on
the schematics at the side of the off page connector that, this connection goes
to these many pages, refer the U10.7 connection”Data2” number 5 9 means that,
Data2 net goes to page 5 and page 9 of the schematic as well. Before providing
Intersheet reference, we must make sure that, we have correctly given the pages
numbers and ordered it in correct sequence. Otherwise, it may create error when
we generate.
Reference Designator, it will be referred as (Ref Des) as short form and it is used to
name the device uniquely by providing a letter with a number combination, for
example U1, U2…
Some of the REF DES used in schematic circuit design are,
BT –Battery
C – Capacitor
D – Diode
E – Antenna
F – Fuse
J – Connector, Jack, female
K – Relay
L – Inductor
P – Connector Plug male
Q – Transistors, FET
R – Resistor
S, SW – Switch
T – Transformer
U – IC
Some letters should be avoided say I, O, V and H, since it
may used to denote the units of some values like Current, Voltage. If we assign
it may produce confusions.
And each device should have unique ref des, since ref des is
also used to identify the faulty part while troubleshooting the PCB, if we have
all resistors as named as R1 then it will be very difficult to identify which
resistor got shorted but if we have unique name then we can say yeah R5, R1 got
error and it can be looked in schematics circuit design and get it replaced.
Annotate, its an option to update the ref des number in
sequential manner by tool, it will start renumbering from Top left corner of
the schematics page and increments its number all the way to right and down to
the bottom right corner. So we will have all consecutive numbers and we will
not have any random numbers like R1, R5, R10, if we have only three resistors
in the design, then by doing annotation, we will have R1, R2 & R3.
Before doing annotation, we have to reset all previous
existing ref des numbers to ?, example
for above we have to make all Resistors to R?, R?, R? so that, tool will
increment it to R1, R2 & R3.
Back Annotation, It is the process of doing annotation in
PCB first, get that report and importing
it in to schematics to make the same changes that have been done on PCB, so
that schematics and PCB will be in sync. On PCB also, it will start renumbering
from Top left corner of the PCB and increments its number all the way to right
and down to the bottom right corner of PCB.
Schematic
DRC:
DRC –
Design Rule Check, it is the process of checking designed schematics to find
out any issues or errors and then correcting it. And this is automated process
and so we can find any possible human errors. It should be done each and every time
before generating the outputs from the schematics. If we miss this process then
there may be chance of getting errors and lead the product to scrap.
Basically this check is used to identify shorts and opens in
the schematic circuits and this is being checked by different forms of checking
like,
•
Checking for Single Node Net
•
Checking for no driving source
•
Checking for matching off page connector
•
Checking for unconnected and disconnected pins
•
Checking for missing connections on BUS
•
Checking for same net alias name on different pages
•
Checking for two more net names assignment on single wire
•
Checking for PCB Footprint names
•
Checking for same Ref Des repetition
•
Checking for extra and missing pins on symbol
•
Checking for Illegal characters }{ ) (, / : ; ‘ “ \ * &
^ % $ # @ !
By only checking all the above will not make sure our
circuit is free of shorts and opens and we have to use our intellectual
thinking to check further to find if anything missed by tool.
Generally, we have to be more concern on the power supplies,
this is back bone of all designs and products, if we miss any open and short in
the power supply in the design stage itself then it will be like waste of time
and energy to proceed further and complete the design and product. So we have
to check all power supplies like where it is getting generated (Source) and
where and all it’s going. We have to check all power pins of IC with the
datasheet, how much the voltage should be connected to this pin and have to
check in our design as well, it was connected as per the datasheets
recommendation or not.
Schematic
Outputs:
Two types
of outputs will be generated from the schematics and they are,
•
BOM (Bill Of Material)
•
Netlist
The first one BOM, will contain all parts information which
have been used in the design and it is used to procure (Buy) the parts. Once
its generated it will be given to Component Engineers (Procurement Team), so
they will order these parts and will suggest the Hardware Engineer, if it’s not
available and all other difficulties if anything.
The BOM should contain the following information,
•
Item
•
Quantity
•
Reference
•
Part / Value
•
PCB Footprint
•
Description
•
Manufacturer Part
Number
•
Manufacturer
•
Voltage
•
Tolerance
•
Package
•
RoHS Status
The BOM output will be mostly in excel format and example of
such BOM is in the following page. The headers in the BOM will be discussed in
the Component Engineering Section.
The Second output from the schematic circuit design is
Netlist, as we discussed Earlier the Netlist is the list of Net and Component
Information. Along with the Netlist, the schematics, the BOM also will be given
to PCB Layout Engineers to proceed with PCB design process.
If we miss to assign any PCB Footprint name in the part
properties then we will not able to generate the Netlist. It will be popped by
a error flag both in DRC check and also in Netlist generation process.
This PCB Design is the Next level Electronics Product Design
Process; we will discuss this in detail in later section of this book.