Microsoft Altium_Designer_Intermediate_Guide [Compatibility Mode] Altium Designer Intermediate Guide

Altium_Designer_Intermediate_Guide

User Manual:

Open the PDF directly: View PDF .
Page Count: 352 [warning: Documents this large are best viewed by clicking the View PDF Link!]

Altium Designer Guide

Beginning & Intermediate Version

Glenn Mercier

mercierg@unlv.nevada.edu

Research Engineer, TBE-B311

University of Las Vegas, Nevada

Part 1: Beginning Guide

This guide is a beginner’s guide to PCB

design using Altium Designer and is

geared towards the following individuals:

◦Possess ample theoretical electronics

knowledge

◦Has little or no PCB design experience

◦Has little or no Altium Designer experience

Beginning Guide

Before proceeding to the actual software

tutorial, It is important to understand

when it is absolutely necessary to use a

PCB rather than design with a

breadboard

Most students have a reluctance to

learning new software and spending

money for something they could possibly

build on a breadboard.

Breadboard vs. PCB

For many electronic designs, one has a

choice to build a circuit on either a

breadboard or on a printed circuit board.

Most students have a certain comfort

zone working with breadboards, but there

comes a time when the complexity of the

project or the physical requirements

requires electronic design through CAD

(computer aided design).

Breadboard Advantages

Very quick to prototype using standard

components

Can easily make changes to schematic or

the functional working of the circuit

Easy to connect to electronic equipment

such as function generator, oscilloscope,

power supplies, etc.

Breadboard Disadvantages

Unprofessional appearance

Difficult to troubleshoot due to human

error and poor connections

Works very poorly for high speed design

Difficult to modify complex SMD

components for prototyping

Excessive capacitance

Difficult to replicate

Printed Circuit Board Advantages

Professional appearance

Repeatable and controllable stray

inductance and capacitance

Can handle most power requirements

Can make very compact

Excellent high speed capabilities

Easy to assemble and replicate

Printed Circuit Board Disadvantages

Increased design time

Drastically increased schematic-to-finished

product timeframe

Development Cost

Difficult to modify once board is fabricated

Must learn at least a basic form of CAD software

Quality of PCB can be affected by limited

knowledge of software package

Capabilities vary greatly with different software

packages.

High end CAD software is very expensive

Required PCB Design

Small Packages,

such as a BGA,

MLF, QFP are

practically

impossible to

prototype on a

breadboard due

to their small

size and MUST

be designed on a

PCB.

http://content.answers.com/main/content/img/CDE/_MCROBGA.GIF

Required PCB Design

Just dealing with the sheer number of pins

on modern practical designs required a

PCB.

It is common to see single components

containing up to 1,500 pins

High speed design cannot be performed

using traditional prototyping methods

Altium Designer

This is based off the current version of Altium Designer,

6.9.0.12759

The Altium Designer Suite contains many unified features such as:

◦FPGA schematic design

◦VHDL/Verilog compilers

◦C/ASM compilers

◦Scripting

◦Simulation

◦2D Field Solver

◦Simulation Engine

◦Library Management

◦Database and advanced query language

◦CAM display management

◦Schematic Capture

◦PCB Layout

System Requirements

Getting Started

Start the software by

clicking

START

PROGRAMS

ALTIUM DESIGNER

Altium Designer 6

Create a start bar shortcut

if you plan on using the

software a lot. (shown on

right)

Project File

Project files are like a container for your project.

There are many different things you will need for

even a basic project, such as:

◦PCB Footprint libraries

◦Schematic libraries

◦Schematic documents

◦PCB documents

◦Scripts

◦CAM files

◦Settings

◦Generated reports

◦Generated files

◦Version Control features

◦Etc.

Creating a Project

When the

software starts,

follow the

menu sequence

in the image to

create a new

‘PCB Project’

Many people

skip this step

and just create

a schematic file.

This a huge

mistake!

Absolutely

everything in

Altium

Designer is

based on

project files

Project Name

We need to save our project and rename the project to something

more meaningful.

Right click on PCB_Project.prjPCB and save the project as

‘PROJECT- EE495’ to a new folder (preferably on a flash drive)

called ‘EE495 Project’ inside a root folder called ‘EE495 Altium’

EX: F:\EE495 Altium\EE495 Project\PROJECT-EE495.prjPCB

Inside this folder, we will place all relevant project data

Organization

It is useful to place all project information inside this folder.

Inside this root folder, create subfolders called ‘CODE’ and

‘DATASHEETS’

Organization and centralization is also important for backing up all

your data properly, version control, and copying project data to a

CD for all finished projects (which you should do for future

reference)

(Group) Quiz Project #1

For the first quiz project, we are going to create

a schematic that will contain:

Atmega8 - Atmel Microcontroller , 16 MHz, QFP

USB-B Connector

FT232 USB- UART interface chip , TSSOP28

2x5 Programming Input Header (0.1” Pitch)

SMD (Surface Mount Device) LEDs , 0805 Size

This project contains all the necessary parts to create a

PCB that can communicate directly with a computer

through a USB (Male B- Male A) Cable.

◦You are encouraged to actually build this PCB as an

inexpensive, functional development board.

◦This project is to be finished by next Wednesday (5/28)

with a possible in-class portion

Adding a Schematic Drawing

Follow the menu sequence shown to

create a new schematic. This will

automatically be added to the project

tree we created.

Schematic Entry

The ‘sheet1’ schematic document is now added

to the project tree as shown below.

Rename this file to something with a more

meaningful name such as ‘Main’. There are many

times when you will have multiple schematic

entries and it helps to have a descriptive name

Any open project files will appear in the menu

area above where the blank schematic page

appears.

Libraries

Similar to a real laboratory, to build a design

from a schematic you must first add real

parts to the project.

For this, we must add what are called

‘libraries’ to our project. Libraries contain

vital information about the parts we are

going to add.

Once libraries are added to the project, any

component inside that library can be freely

inserted into your design.

Types of Libraries

There are three main types of libraries for PCB

design:

◦Schematic Library- Contains schematic drawings of parts,

when we look at a schematic, we are looking at a collection

of schematic parts

◦PCB Footprint Library- This contains the physical dimensions

of a real component. This information is readily available in

datasheets.

◦Integrated Library- These are the most useful libraries

because they combine a physical part (footprint) with a

schematic drawing.

Libraries

Libraries are located in the folder:

C:\Program Files\Altium Designer 6\Library

Updated libraries are available online at

http://www.altium.com/Community/support/Libraries/Designer6libraries/

Altium has since changed some of their

library files, I have included a ZIP file on

the course website with library files we’ll

be using.

Download and unzip the file into the

‘library’ folder in your project directory

Libraries

Copy the following Libraries to a folder called ‘Libraries’ in your Custom Altium

folder:

Integrated Libraries (*.IntLib)

Atmel Microcontroller 8-bit AVR

Miscellaneous Connectors

Miscellaneous Devices

NSC Operational Amplifier

ON Semi Operational Amplifier

Schematic Libraries (*.SchLib)

<none>

Footprint Libraries (*.PcbLib)

Chip Capacitor – 2 Contacts

Chip Diode – 2 Contacts

Chip Inductor – 2 Contacts

Chip Resistor – 2 Contacts

Crystal Oscillator

Miscellaneous Connector PCB

Miscellaneous Devices PCB

Miscellaneous Devices

Miscellaneous

NOTE: When you create your own schematic and footprint libraries, you should

place them in the same library directory in your project folder

Adding Libraries To A Project

We have organized all the libraries in a

folder, now we need to add these to the

project

Follow the following prompt to add

libraries to the project

Adding Libraries

There are two methods of adding libraries

◦Project Libraries- Libraries available only for the scope of this project

◦Installed libraries – Libraries available to ALL projects by default. These do not show

up in the project tree.

The Search Path modifies the search location when searching for parts.

Adding Libraries

We want to make these libraries project-

specific only instead of global availability with

the ‘Installed’ tab

Make sure the ‘Project’ tab is selected, and add

all libraries from your project library folder

Project Hierarchy

By expanding the ‘+’

next to libraries, you

should see a list of all

the project libraries.

Make sure you have all

these libraries

installed before

continuing.

Notice how the

project tree separates

source documents and

libraries automatically

Open, Saved, Unsaved Files

Open files are indicated

with a ‘white paper’

Example: Main.SchDoc

Open modified and

unsaved files are

indicated with a ‘red

paper’

Example: The Project file

itself has been modified.

Closed files have

nothing in the column

Example: The Atmel

Microcontroller library

All open files are

accessible by clicking on

them in the project tree,

or in the top bar in a

windows- taskbar type

window

Project Documentation

We can’t create

a schematic

without knowing

more details

about the parts

we’ll be using.

Obtain the FTDI

FT232R UART

IC Datasheet

Rename the file

something less

cryptic such as

FT232 USB.pdf

Project Documentation

Specifications are often given or required for components, You should check and

double check each meets the project specifications.

Atmega8 Microcontroller, QFP Package, 16 MHz, ROHS Compliant

Mouser P/N: 556-ATMEGA8-16AU

Save as ‘Atmega8 QFP Atmel Microcontroller.pdf’

USB-B (Female/Socket) , ROHS Compliant, Right Angle Mount

Mouser P/N: 806-KUSBX-BS1N-B30

Save datasheet as ‘USB-B Connector’

SMD LEDs (0805), ROHS Compliant

Mouser P/N: 638-172BHC-AN1P23T

2x5 Box Header (Prog. Connector), Gold Plated, ROHS Compliant, Pitch=0.1”

Mouser P/N: 649-66506-066LF

Save datasheet as ‘2x5 Box Header.pdf’

Chip Sizing Information

‘Chip’ components are devices that come in small rectangles

The 0805 specification for the LED are actually dimensions of the chip component

itself (Size Code).

Split up the numbers to 08 05, These are the dimensions in inches

The Length of the chip diode is 0.08” = 80 mils

The Width of the chip diode is 0.05” = 50 mils

Therefore, the larger the numbers, the larger the chip device:

Larger chip sizes can handle more power

Smaller chip size can handle higher frequencies (ideally)

Chip Sizing Information

1) Tantalum Capacitor (A-Case)

2) Tantalum Capacitor (D-Case)

3 & 4) Electrolytic Capacitor

5) 0805 Ceramic Capacitor

6) 1206 Ceramic Capacitor

7) 1210 Ceramic (Same length, but wider)

¼ Watt through-hole resistor

given as size reference

(Same as in our lab)

http://www.geocities.com/vk3em/smtguide/pics/caps.jpg

Chip Sizing Information

1) 1218 (1 Watt)

2) 1206 (1/4 Watt)

3) 0805 (1/8 Watt)

4) Potentiometer (Bottom & Top)

¼ Watt through-hole resistor

given as size reference

(Same as in our lab)

http://www.geocities.com/vk3em/smtguide/pics/resistor.jpg

Chip Sizing Information

1) 20 Pin DIP Package

2) SOIC20, Wide

3) SOIC8, W/Power Tab

4) SOIC8, Standard

5) SSOP20

¼ Watt through-hole resistor

given as size reference

(Same as in our lab)

http://www.geocities.com/vk3em/smtguide/pics/ic.jpg

Placing Parts

We have now added all the necessary

libraries for the project, now we need to

draw the schematic.

Follow the menu sequence below to place

a part

Placing Parts

After clicking ‘place

part’ from the

previous screen, you

will have an option to

place from standard

libraries or database

libraries. Keep this on

standard libraries

Click the button to

the right of the

‘History’ button to

bring up a list of

available libraries.

Creating a Schematic

At the top of the screen, there is a dropdown box which lists available schematic and integrated

libraries (but not PCB footprint libraries). For the highlighted library, in this case Miscellaneous

Devices, there will be a list of the parts inside that library in the bottom left.

Creating a Schematic

Select the Atmel

Library and navigate

down to Atmega8.

Notice there are

many options for the

same chip. This is

because although the

device is the same,

there are many

different ‘packages’

that this chip comes

in.

NOTE: The Atmega8

costs about $3.50

Creating a Schematic

Add the ATmega8-16AC

Looking at the datasheet for the ATmega8, we can see exactly what the -16AI stands for.

◦Supports up to a 16 Mhz clock

◦Commercial grade fabrication (Temperature ranges from 0C to 70C

Creating a Schematic

Here are the three

common packages for

the ATmega8

microcontroller.

These are scaled relative

to each other with the

close to the same

functionality with each

package.

NOTE: Why does the

QFP package have 4

more pins than the DIP

package?

Creating a Schematic

We were given constraints with the assignment of

this project. Sometimes constraints are based on:

◦Economics, Size, Power handling, ability to assemble the part

, etc ..

For the microcontroller, we were told it must

function with a clock rate of 16 MHz, and must have

a QFP Package

It is crucial to take note of all constraints BEFORE

entering the schematic and/or pcb layout. It is a

HUGE waste of time to design around a part that

doesn’t meet the specifications.

Creating a Schematic

Looking again at the ordering information available in the datasheet, we know

that:

◦The Chip must be able to work with a 16 MHz clock, we can eliminate all 8MHz rated

microcontrollers

◦The DIP package is 28 pins, we can eliminate any package that has a ‘28’ in the

package information

◦The 32M1 refer to the MLF packaging, we can eliminate all those items

◦This leaves us with a decision to choose between commercial rated or industrial

rated temperature ranges, Either the ending in -16AC, -16AI, -16AU are acceptable

Creating a Schematic

Usually the industrial rated components are more costly than the commercial

rated components, so we will choose the Atmega8-16AC

QUESTION: A temperature rating doesn’t affect the footprint or simulation

of the device, is there a reason we can’t/shouldn’t just choose any of the three

possible options ???

Creating a Schematic

Notice to the right, there is the schematic drawing and associated pinout

of the device, beneath that is a drawing of the PCB Footprint (this should

match what you expect from the datasheet)

The bottom shows all footprints associated with the part

◦Why do you think there are three different footprints for a QFP32 ?

Creating a Schematic

Many vendor supplied integrated libraries contain much more than just a

schematic drawing and PCB footprint

Shown below is a rendering of a 3D Image of the chip. Altium has an option to

view the PCB in 3D, and this image will represent the Atmega8 in the 3D

rendering

Also included are SPICE files and/or IBIS files (more on this later)

Creating a Schematic

Place the Atmega8 into the schematic drawing

◦You can always move the location later

◦What function does pin 20 perform ?

Zooming In and Out

You can’t see the function of pin 20 because the image is zoomed out.

To Zoom In/Out

◦Wheel Mouse and Control Key

◦Page Up/Page Down Key

To Pan Left/Right/Up/Down

◦Wheel Mouse and Shift Key

◦Left/Right/Up/Down Arrow (Small Pan)

◦Shift Key and Left/Right/Up/Down Arrow (Larger Pan)

Pin Functions

Pins can be setup for the following functions:

◦Input, Output, I/O

◦Open Collector, Passive, HiZ, Emitter,

◦Power

Depending on how the pin is set, will determine how the DRC (Design Rule Check)

Interprets the Pin and what connections are allowed

Add the USB-B Connector

It seemed obvious which library contained the Atmel Atmega8, but

now we need to add a USB-B connector.

An easier method than searching each component and each library is

to search the libraries.

Click the ‘Find’ button to the right of the library selection

(It doesn’t matter which library is selected/active)

Add the USB-B Connector

Ty p e i n th e key wo rd

you are looking for

We are looking for a

USB-B connector, For

now let’s just search

for ‘USB’ and narrow

down the search after

that.

NOTE: Using

wildcards *before and

after allow for words

such as xxxUSBxxx

to be recognized.

Add the USB-B Connector

The search can take a

while depending on

how many libraries

you are searching

through.

We are searching

through only the

libraries we added to

the project, so it

should happen very

quickly.

The result of this

search came back

negative, That means

there are no USB

items in any of our

project libraries.

Click the ‘Search’ tab

in the top right corner

Add the USB-B Connector

Change the scope of

the search from

available libraries

(available to the

project) to ALL

libraries in the path.

The path will

automatically be

entered for the default

library location in

Altium

* make sure ‘include

subdirectories’ is

ticked.

Click the search

button

Add the USB-B Connector

USB is a very common term, so very quickly the list fills up

Expanding the box to read the description helps with identifying what each

part is (in case names such as ‘1-353576-1’ mean nothing to you)

We are looking for a SINGLE Through Hole, Right Angle, USB-B

Receptacle socket, which is located at the 8th row down

Add the USB-B Connector

Select the 1-1470156-1

and click OK

You will get a message

stating that the library is

not available to the

project, but Altium is

willing to install it for you,

click yes

Click ‘OK’ again to add

the part

Add the USB-B Connector

The library AMP Serial Bus is added automatically to the ‘Installed’ libraries,

NOT the project libraries

This action DOES NOT MOVE ANY LIBRARIES PHYSICAL LOCATION

For ease of future design, it is a good idea to move libraries added by this

method to your ever-growing list of libraries

You can do this by copying the AMP Serial Bus USB from the path given in

the ‘available libraries’ below

C:\Program Files\Altium Designer 6\Library\Amp

to your custom library in your flash drive

X:\EE495 Altium\EE495 Project\Altium Libraries

Add the USB-B Connector

AMP makes several different libraries, so be sure to copy the correct one!

Rotating Parts

The easiest way

to rotate parts is

to select the item

and hold the left

mouse button

down, and tap

the space button,

this will rotate 90

degrees each tap.

Another method

is to double click

the component

to open up the

component

properties

window, and in

the bottom left

corner you can

set the

orientation

NOTE: the

‘mirrored’ tab

will flip the

component

about its axis

Component Properties

In the top left corner of the

component properties, you can set

comments, descriptions, designator

values and library link information

NOTE: Unique ID is a unique value

which links the schematic part with

the PCB document.

In the bottom left corner, you can set

graphical properties such as

orientation, mirrored, locked (stuck

in schematic)

The ‘Edit Pins’ button will allow you

to reassign pins, pin functions, and pin

numbers. This should only be used if

you are absolutely positive you know

what you are doing!!

Component Properties

In the top right corner of

component properties of a

standard component will contain

information such as publishing

date, termination length, URL’s,

drill sizes, etc.

NOTE: You can add your own

custom fields (such as ordering

information, ordering part

numbers, etc.)

NOTE: You can also add a

custom PCB rule to the

component while you are still in

schematic capture mode

The bottom right corner

contains model information for

the component, such as

footprint model information and

signal integrity models.

Component Properties

Mirror the

USB-B

connector

and orient

the parts so

they match

the diagram

to the right.

Programming Header

Add a part from the Miscellaneous Connectors library called ‘Header

5x2’

Make sure to use caution when selecting parts. If you accidentally add

‘Header 5x2a’ they make look the same, but look at the numbering

system of the pins. Always make sure the numbering method is the same

as you expect it to be.

FTDI Chip- FT232 (TSSOP28)

A quick search for

the FT232 chip we

will be using gives

the following result

Although there are

three matches for

the FT232, We are

actually looking for

the FT232RL as we

will see on the next

slide

FTDI Chip- FT232 (TSSOP28)

Like all aspects of

PCB layout, you

must pay attention

to every detail on

everything.

The datasheet

states that the

FT232RL is a 28-pin

SSOP package.

Since this footprint

is not available, we

must create the

part in a custom

library

FTDI Chip- FT232 (TSSOP28)

Follow the menu

sequence shown to

the right to create a

new PCB library.

This library will

house ALL of your

components

FTDI Chip- FT232 (TSSOP28)

The new library is

automatically added to

the project.

Right click and click

‘save as’ and rename

the library to a more

appropriate name:

EE495 and save it in the

directory with the rest

of your libraries

FTDI Chip- FT232 (TSSOP28)

Notice the small tabs in

the bottom left corner.

Double click the new

PCB library you

created to open it, and

click on the one titled

‘PCB Library’ to work

inside that library.

FTDI Chip- FT232 (TSSOP28)

With the PCB Library

tab selected, we can see

that there is only one

component inside our

library called

PCBCOMPONENT_1

FTDI Chip- FT232 (TSSOP28)

From inside your PCB library, click TOOLS > IPC Footprint Wizard

to open the IPC Footprint Wizard.

This will help you easily create the footprint for the device

You will see why it is so important and helpful to have standards

when it comes to documentation, naming conventions, etc…

FTDI Chip- FT232 (TSSOP28)

The first step is selecting what type of part it is. They don’t

specifically have SSOP, but SSOP is just a modified version of the

SOP so select that

There is a diagram of what the chip looks like to the right

NOTE: check the note on the bottom of the wizard: All wizard

measurements must be entered as metric (mm) units

FTDI Chip- FT232 (TSSOP28)

At first this might seem a bit daunting and intimidating, but when you

pull up the datasheet to find the values, you will see that the graphics

and naming convention matches what we must entered

FTDI Chip- FT232 (TSSOP28)

The first entry is for width range. The datasheet gives a width range

of 7.80 +/- 0.40mm (Min width = 7.4mm, Max = 8.2mm)

FTDI Chip- FT232 (TSSOP28)

The max height of the chip (A) is

2.00mm

Enter this in for maximum height

Question: Why would the height

of the chip matter ??

FTDI Chip- FT232 (TSSOP28)

Fill out the rest of the values, you should get the numbers below

NOTE: Watch as you enter values, the graphic on the right will

dynamically change

FTDI Chip- FT232 (TSSOP28)

Accept the automatically entered values for the next few slides until

you get to the slide below

Uncheck the ‘use suggested values’ and change the name to FT232RL

Click ‘Finish’ and the part will be added to your library

FTDI Chip- FT232 (TSSOP28)

Your library will

automatically open

with your new part

included.

Notice how there

are two yellow

dots , those are ‘pin

1 indicators’ so

the board is

assembled properly

You can now be

confident that the

FT232RL chip will

fit on this footprint

FTDI Chip- FT232 (TSSOP28)

Click the ‘Projects’ tab on the

bottom left to return back to

the project file hierarchy

Since a PCB footprint is useless

as far as a schematic is

concerned, we must create a

schematic drawing and link the

drawing with the footprint we

created

FTDI Chip- FT232 (TSSOP28)

Keep in mind that

we cannot keep the

schematic drawing

of the FT232 and

change only the

footprint because

sometimes pins are

added, removed, or

are different.

Shown to the right

is the pinout of the

device obtained

from the datasheet

Creating a Schematic Part

Create a Schematic

library like we

created a PCB

footprint library

Rename the library

to EE495, and save

in the same

directory as the

rest of your

libraries.

Double click the

schematic library to

open the library,

and then view the

library by clicking

the ‘SCH Library’

tab in the bottom

left of the screen

Creating a Schematic Part

The large portion of the screen is for creating your schematic drawing, the

top left part contains all the parts in the library, the towards the bottom left

is the pins and associated function/name

Creating a Schematic Part

Double click the component and enter the values as shown below

Creating a Schematic Part

Your component should have a descriptive component name and

description such as the one below

Click the ruler tab to see the dropdown list

as shown in the right. This is the main icon we’ll

Be using in creating the schematic drawing

Creating a Schematic Part

Place a rectangle and draw it so it looks like below

(Size doesn’t matter)

Creating a Schematic Part

Click the ‘place pin’ and place 28 pins around the rectangle

like below

Click and drag the rectangle to the proper size

Creating a Schematic Part

Double click Pin 1 and change

display name to TXD,

Change electrical type to

OUTPUT

Creating a Schematic Part

Sometimes the datasheet

will explicitly give the

function of the pin, this is an

added bonus and not usually

given

You must usually define the

pin type from reading the

description of what the pin

does

Defining pin types is not a

necessity, and things may

work fine without defining

them properly, but you

should usually add the pin

function to allow the DRC

to catch your errors.

Creating a Schematic Part

There are usually typical applications schematics which will help

you properly use the device.

You should always read each and every pin description to see if

you need to add functionality, but it is always a good starting point

to use the typical application sheet

Creating a Schematic Part

Usually these typical application notes have corresponding notes

associated with it that you should consider.

The following rules for this device are a combination of rules for

the USB standard, and for the FT232

These notes should be regarded as bible, written by people who

understand and have tested their product to death.

Creating a Schematic Part

Now that we have verified that the pins all match the ones in the

datasheet (with the correct pin numbers!) we can move pins

around and make it look more like the application schematic given

This usually allows for a cleaner looking schematic drawing and

much easier to reference the datasheet.

Creating a Schematic Part

Now that we have verified

that the pins all match the

ones in the datasheet (with

the correct pin numbers!) we

can move pins around and

make it look more like the

application schematic given

This usually allows for a

cleaner looking schematic

drawing and much easier to

reference the datasheet.

NOTE: You can also hide pins

from the schematic

document. Double click on

the pin and check ‘hide’

Creating a Schematic Part

Now we need

to associate the

PCB Footprint

we created

with the

schematic

drawing

Click the ‘add

footprint at the

bottom of the

page

Click ‘browse’

in the ‘footprint

model’ section

Creating a Schematic Part

Select your EE495 Library from the dropdown list

There is only one part inside your custom EE495 library, so the

choice is easy. Select your part and click ‘OK’

Creating a Schematic Part

In your schematic library, you

should now see the footprint

you created along with the

schematic drawing you made

Finally the part is complete!!

NOTE: This gets much faster

as you do it more, but you can

see the value of the large list

of integrated libraries included

with Altium

Creating a Schematic Part

One last check is to look at

the left side of the screen. The

first three columns in this case

all refer to data you entered

when creating the schematic

document

The last column (FT232RL) is

the name that you gave the

PCB Footprint

Check and compare that pin 1

on the schematic is linked to

pin 1 on the PCB footprint

Repeat for the rest. If

something doesn’t match,

something went wrong!!

Save the Project

Now is a good time to save

the project and all the

changes you made.

Follow the menu sequence

to the right to save the

project

Insert The FTDI Chip

Select your EE495 library, and place the only component in your

library (so far). You should see the schematic drawing and also the

PCB footprint. If not something is wrong

Insert The FTDI Chip

Notice how the rotated and mirrored USB-B connector matches up

perfectly with the FT232 chip. (D- goes to USBDM, D+ goes to

USBD+) This did not happen by chance

Current Schematic

Programming Interface

We need a device

that will send our

compiled HEX

code to the

microcontroller.

This type of

device is called a

programmer

Sparkfun sells

many decent

programmers that

are cheap ($13)

Programming Interface

If you want, you

can see the

schematic of the

programmer, and

integrate it onto

your development

board

As you can see,

this is a simple

device which

would only add a

few components

to your project

Programming Interface

The specification for the

2x5 header, spaced 0.1”

apart perfectly matches

the connection for the

programmer.

Although you may not

know what these pins

are, we will assign them

to the programmer

header

Placing a Connective Wire

Find the icon that looks like the one above, and

click it to place a wire, it will be blue in appearance

WARNING!!: Make sure not to use the

‘place line’ from the drawing box. This

will draw a line that LOOKS like a

connective wire, but a connection

won’t be made

Placing a Connective Wire

Draw wires on the

2x5 header as shown

on the right

Click the GND and

VCC icons from the

wiring menu (shown

below) and make it

look like the diagram

to the right

Net Labels

A net label is a method of electrically connecting nets

of the same name

This allows a method to make a connection without

requiring placing a wire

So what’s wrong with running wires ?? It is far more

difficult and more confusing to run wires, especially

when routing a large bus.

Net Labels

Here is a schematic which is very confusing and would benefit from using

net labels

Net Labels

This is a design

that uses direct

wires for short

connections, and

net labels for long

connections.

Notice how the

schematic looks

more clean and

professional.

NOTE: Even if

direct wire

connections are

used, it’s still a

good idea to give

the net a name for

PCB reasons

Net Labels

Another example

Using Net Labels

Click on the net label

icon and place the net

label on each of the

wires.

Double click the

rename the net. You

can type in a new net,

or select one from the

drop down list.

Using Net Labels

Rename the nets to

match the diagram on

the right

WARNING: When

placing netlabels, make

sure there is a red X

at the connection

point. If it is a gray X,

there is no electrical

connection

Good Bad

Using Net Labels

Our programming

connector now

exactly matches the

pinout of the

programmer we

selected to buy

Using Net Labels

Make the same net labels on the microcontroller as you did on

the programming connector

Connect the Power and Ground nets as shown below.

The programmer is now electrically connected to the

microcontroller

Using Net Labels

Make the same net labels on the microcontroller as you did on

the programming connector

Connect the Power and Ground nets as shown below.

The programmer is now electrically connected to the

microcontroller

Reset Pin

The reset pin on the microcontroller is an active low

pin, indicated by the bar above the name

This means the device functions normally as long as the

reset line is held high, and will go into reset mode

when brought low (like rebooting a computer)

Looking at the datasheet, we can see characteristics on

each pin and how it works.

Passive Components

Now we need to add capacitors, resistors, and the LEDs.

Place a part, select the Miscellaneous Devices library, and scroll down to

CAP

Place this part (Don’t worry that the footprint isn’t SMD 0805)

Passive Components

Change the comment to =Value, and uncheck the

visible

Change the value to 0.1uF

Passive Components

In the footprint section,

click the ‘add’ button to

add our 0805 footprint to

this capacitor

Passive Components

Click ‘browse’

and make sure

‘any’ PCB library

is selected

Select the ‘Chip

Capacitor’

library, and

choose

CC2012-0805

This is code for:

CC= Chip Cap

2012- metric

0805 - empirical

Passive Components

Place the capacitor down. It should look

something like this:

This is now our template for a capacitor,

just copy & paste whenever you need

capacitors and they will all have the same

footprint and settings we set for this

capacitor

Do not worry about the ‘C?’ , we will deal

with labeling the parts at the end. For now

it is a waste of time.

Passive Components

Repeat the same process with resistors and

LEDs (all in same miscellaneous devices

library)

Modify the settings and change the

footprints

◦Diodes are from the Chip Diode library

◦Resistors are from the Chip Resistor library

Complete the Schematic

Copy and paste the

parts as needed to

finish this schematic

◦Highlight, CTRL-C (copy),

CTRL-V (paste)

The parts to the left are

in the miscellaneous

connectors library and

are called HDR1X10

NOTE: I moved the pin

locations on the top

connector, this does not

change functionality at all,

it just allows for a

cleaner schematic. To do

this you must first unlock

the pins. Double click the

part and uncheck the

‘lock pins’ to move the

pins around

Complete the Schematic

It is common

practice to

add a 0.1uF

decoupling

capacitor to

EVERY

power pin

per IC

Complete the Schematic

The reset line must be

held high with external

circuitry.

Using a 10k pull-up

resistor we can keep

this out of reset

NOTE: Try adding a

switch from the reset

line to ground. This is a

hardware reset switch

Complete the Schematic

Pins 19 and 22 are INPUT pins on the

microcontroller. These pins are both 10-bit

analog to digital converters. It is necessary to pull

these pins high with pull-up resistors if they are

going to be unused (or possibly unused)

Complete the Schematic

Don’t forget we cannot apply 5V across the LED’s. We must use current limiting resistors

To ensure maximum functionality of the development board, rather than hardwiring the LEDs to a

specific port, we will make it so a user can connect any of the three 8-bit ports

Complete the Schematic

Notice how RXD on the microcontroller connects to TXD on the FT232 chip, This is because two

transmitting signals cannot appear on the same line. One pin is an OUTPUT and one is an input.

Because these pins are correctly defined with both parts, The DRC would catch that if we made

the mistake of connecting TXD to TXD

The LED’s here are optional and light when data is being sent or received

Complete the Schematic

I have altered the typical application circuit for this in two ways:

◦I have added terminating resistors on the differential pair

◦I have not included the ferrite bead , you should include this . You can include a 0805 footprint as a

placeholder for the ferrite bead which comes in a chip

Complete the Schematic

Now that all the

parts are added, we

must label all the

components

Follow the menu

sequence to the right

to label all the parts

automatically

Click ‘Yes’ when

asking to update the

changes

Complete the Schematic

All the parts are

now properly

numbered

NOTE: This step

is necessary

before working

with simulations

or PCB Layout

Finished Schematic

Smart PDF

I have included a Smart PDF of the

schematic for this development board in

the downloads section of the website.

In this PDF file you can select and zoom

in to see parts, nets, etc …

Compiling the Project

Compiling the project is fancy

terminology for error checking.

Error checking, although not required, is a

must before converting the schematic

drawing into a PCB document.

We can’t error check without setting up

rules, so first we must setup rules

Compiling the Project

Click

◦Project > Project

Options

Compiling the Project

Under the Error Reporting tab, you can

set options for which level of report you

will get.

◦Some errors are serious

◦Some are not a big deal

Compiling the Project

A setting of ‘no report’ is the same as the

software ignoring it

A warning will allow an action, but won’t

be happy about it

Set the ‘Error’ level or above to see

immediate feedback

Fatal error will not allow compilation of

the project

Compiling the Project

If we set ‘floating net labels’ to error, when we

compile the document, a red squiggly line will

appear beneath the floating label and it will

appear in the compilation report

Compiling the Project

If we set ‘floating net labels’ to fatal error,

when we compile the document, a red squiggly

line will appear beneath the floating label and it

will appear in the compilation report.

Compiling the Project

If you double-

click the error

in the messages

box, it will

show you

compile errors

From there you

can select the

offending error

and it will dim

the schematic

except for the

error

Compiling the Project

I recommend reading through and setting whatever rules

you think will be appropriate.

Keep in mind it is better to have a compilation report

with a lot of information that you don’t care about than to

have an important error slip past

If there are no errors, you will not get a popup screen

when the compilation is complete

Connection Matrix

The next

tab over is

connection

matrix. This

is a quick

way to

allow

certain

connections

to be made

or denied.

Usually this

doesn’t

need to be

changed

PROJECT UPDATE

DUE WED. 06/04/08 !!

Single page report with the following

◦What have you done for your project- (Be Specific!!) I expect

this to be mostly schematic design and research at this point

◦What do you have left to complete

◦Who is responsible for each part of the design

Schematic Entry

PCB Layout

Implementing Technology (Ex: Mike will be in charge of interfacing the transmitter with a

microcontroller)

◦Exam 1 will be based on this report.

Do not think that if you have done no work yet that you are not responsible for the project or

that your test will be easy. The more work you have done by the 9th, the easier the test should be.

Every group member is responsible if someone is trying to get out of doing work. Do not cover

for anyone else. If I find out that the work was not done by an individual, I will hold the entire

group responsible

If there is a problem with someone not working, you have until the 7th to split from the group and

work on the same project by yourself if you let me know.

Creating the PCB

One of the reasons why it is important to define the PCB footprints

while entering in the schematic is to be able to provide a good estimate

of how much board area you will need.

Generally speaking the following things make production more

expensive

◦Larger area

◦More layers

◦Smaller holes

◦Closer tolerances

◦Closer traces and spacing

◦Thinner or Thicker PCB

Our goal is to keep cost as low as possible while still being able to

transfer a schematic to a functioning PCB.

There are no special characteristics of this design that require any

exotics, and we can use a 2 layer PCB for low cost

Creating the PCB

From the project tab in the

bottom left corner, click the ‘Files’

tab and click the upward facing

arrows until you can see

NEW FROM TEMPLATE

Select PCB Board Wizard

Creating the PCB

You will get a very friendly wizard screen, click next to continue

Creating the PCB

Choose the board units as Imperial for this since that is what most of us are

most familiar with

NOTE: You are not stuck with the choice of units that you choose here. The

units specified are ONLY used for the PCB wizard

Creating the PCB

There are many predefined templates for exotic designs or standard PCB

computer interface forms, such as AT Bus, PCI bus, Eurocard, and many

others.

Choose CUSTOM (at the top)

Creating the PCB

Leave the default settings (Rectangular, 5000 mils x 4000 mils )

The dimensions of the board will be on a generic, information layer

(Mechanical layer) which is used to give information to the board house.

Creating the PCB

We want to have a two layer board. This is two signal layers (top of board,

bottom of board) and zero internal plane layers, make this change

Do you remember what a power plane is ? How does it differ from a signal

layer? (HINT: you can have signal layers internal or external, and you can have

power planes internal and external)

Creating the PCB

Make sure the hole type is set on thruhole vias only

Do you remember what a via is ??

Creating the PCB

Our board contains mostly surface mount components, so check this option

Choose that both sides of the board can contain components.

NOTE: These settings really don’t matter. They exist for the autorouter which

we will not be using

Creating the PCB

Change track size

(10mils) and trace

clearance (8 mils)

What is the metric

length of 8 mils ????

Change the minimum via

hole size to 15 mils, and

the min. via width to 30

mils

NOTE: ALWAYS be sure

your settings can be

fabricated at a

reasonable price before

setting these values

Creating the PCB

The wizard is now complete and your PCB is created based on the values you

have given.

Creating the PCB

Right click on

the PCB >

Click ‘Options’

Click ‘Board

Options

Creating the PCB

Uncheck ‘Display Sheet’ (this has a use, but for now we want to reduce

clutter)

Change the markers from lines to dots and click OK.

NOTE: The snap grid and component grid are very important, we will get

into this later though.

Creating the PCB

The PCB has been added to the

list of documents, but has NOT

been added to the project (Notice

it is listed as a free document)

Click and drag the PCB to your

project

Right click on the PCB1.PcbDoc

file and save the file in your project

directory.

Save the file as ‘Dev Board’

Creating the PCB

If you get the following warning, just click OK. It is telling you there may be

compatibility issues if you try to open the PCB document in an older version

of Altium.

Creating the PCB

If you select your schematic again, click the Design button up top and then

click on ‘UPDATE PCB DOCUMENT DEV BOARD.PcbDoc’

This will begin the process to turn your schematic into a PCB

Creating the PCB

This will open the ECO (Engineering Change Order)

This is asking which changes to make.

Validate changes will check for errors in the process

Execute will actually perform the change

Creating the PCB

Click ‘Validate’ at the bottom. This may take a while depending on the

complexity of the project.

Notice the green check boxes to the right. This means that each step with the

green check mark can be performed sucessfully.

I have deliberately removed the library for the USB connector to show what

will happen if there is an error for a step (red x) Adding the library will fix

this error

Creating the PCB

Because there are usually many different steps to creating the ECO, it is

usually helpful to check the box that says ‘Only show errors’ at the bottom.

You are in good shape when no errors occur and this list is empty

Creating the PCB

When no errors appear during the validation step, you can click the ‘execute

changes’ to actually import the schematic to the PCB

You will see a second row of green check boxes when you execute the

changes. Again, check for errors by checking the ‘Only show errors’

Creating the PCB

NOTE: Every time you perform an ECO, the results are saved in a text file in

your project directory

Creating the PCB

Export the NETLIST following the menu sequence below (You must be on

the PCB document, not the schematic document

This will export the Netlist to your project directory

Creating the PCB

The Netlist contains information such as parts,

footprint, and value (as shown below)

Creating the PCB

It also contains connection

information as shown to the right

Each Netlabel (either assigned by

you or the software, every net

has a netlabel) shows which

component and pin number

connects to that node

Obviously a connection like GND

will have many connections, and

netlabels such as MISO might only

have a few (3 in this case)

Creating the PCB

◦Netlist Connections for Net MISO:

P3 pin 9

P1 pin 5

U1 pin 16

◦A quick look at the schematic shows

that this net is properly connected

Creating the Netlist

Fortunately, Altium handles the Netlist transparently to

the end user, but it is important to at least be familiar

with the term and how the schematic is transferred to

the PCB and vice versa

Any changes that are made must be made to the Netlist.

The Netlist is the ‘link’ between the PCB and the

schematic. It is important that the schematic and PCB

agree on connections, nets, footprints, etc..

Creating the PCB

After executing changes. If there are errors or not,

whatever the software can import into the PCB it will do

Notice how the software just sort of ‘dumps’ all your

parts (PCB Footprints) off to the side of the board.

Does anyone know why the software doesn’t place

the parts ???

Creating the PCB

You may have

noticed the words

on the right on

your design. Leave

it where it is and

don’t mess with it.

We will get to that

later what it does

This is called a

Special String

Creating the PCB

Notice how all the parts are placed inside a colored

rectangle box called ‘Main’. This is called a ROOM.

Rooms are used to group common circuit types. A room

is created for each schematic page we have

Since we only have one page, called ‘MAIN’, there is only

one room

Creating the PCB

Rooms are like borders for your parts. An item inside a

room cannot escape without an error message.

Since we only have one room, we can delete the room

without affecting our layout at all.

Click anywhere in the room and hit the DEL key

The room will disappear and the components will remain

NOTE: You can disable the use of rooms in project

options

Creating the PCB

If you hit the ‘L’ key on the PCB page, it will bring up the

following prompt.

Change the option under mechanical layers that says ‘Used

Layers Only’

Creating the PCB

Notice the different tabs at the bottom of the screen. The selected

layer will look different than the others (in this case, top layer)

Unlike a schematic, which is 2D, a PCB is a 3D entity with a whole

bunch of layers on top of each other. These layers are all combined to

form your PCB.

NOTE: These layers are all color coded!!!!

Creating the PCB

If we zoom in, notice that U2 (The FT232 chip) has

several green pads, and several red pads.

The red pads represent something on the top layer. But

why are some of the pads green ??

Creating the PCB

If we type ‘L’ again, it

will bring up the board

layer lists.

Since the layers are

color coded, we can

quickly look for the

green one and notice

that this is a DRC error

marker (Design Rule

Check)

For some reason Altium

has a problem with our

FT232 Chip

Check the boxes for

pad holes and via holes

Creating the PCB

If we put the mouse over one of the green pads, it will tell us

information about the pad, most importantly it will tell us what the

error is

For these pads, there is a clearance constraint error between a pad on

the top layer, and another pad on the top layer

NOTE: It is up to you to decide is this is a real error, or an improperly

set rule

Creating the PCB

Like the schematic, there are rules we need to set.

Click Design > Rules (or) Rules wizard to create/modify rules

NOTE: The software only creates errors based on your rules. It is up

to you to know if something is OK or not. If you tell the software that

2 mil traces are OK, the software will enforce that.

Creating the PCB

The DRC

expects a

minimum

spacing

between

different

nets of 8

mils.

Creating the PCB

Make the following rule changes (from top of list down):

◦Max Trace Width= 200 mils

◦Minimum Via Size = 15 mils, Min Via diameter = 30 mils

◦Maximum Via size = 50 mils, Max Via diameter = 80 mils

◦Minimum hole size = 15 mils, Max hole size = 200

Creating the PCB

Try using trial and error

and change the setting to

7 mils and you’ll notice

the error markers go

away.

NOTE: There are many

better ways of

determining the actual

spacing, but we want to

keep things simple for

now

Creating the PCB

Notice the small

lines, these are

collectively referred

to as a Ratsnest.

It is a way of

telling you which

connections need

to be made still

Example: You can see

pin 2 of R12 needs

to connect to Pin 2

of the USB

connector

Creating the PCB

Components are moved in the PCB the same way they

are moved in the schematic.

Notice how the Ratsnest connections remain and will

dynamically change based on how a component is

rotated.

Creating the PCB

There is usually a tradeoff when placing components.

This USB connector might be easier to route if it is in

the middle of the board, but will be difficult for a user to

use a connector in the middle of the board.

For this design, do the best you can to make it easier to

route, for your project, it should make physical sense to

an end user, even if it means harder routing

Creating the PCB

EVERYONE’S PCB WILL BE DIFFERENT!!!

Do not try to make yours exactly like mine or anyone

else’s.

This design I went out of my way to create a more

dense design for clarity and to resize the board. Feel

free to use the entire board area.

Creating the PCB

Usually, components that are close together in the

schematic are placed close together in the PCB.

NOTE: If you have two monitors, keep the schematic

open on one side, and the PCB on the other side. If you

have one monitor, just write down the components

Creating the PCB

For the USB circuit,

we will group the

following components

◦C7- C11

◦R12 – R16

◦U2

◦D9, D10

Creating the PCB

Next group the

components as they

are arranged in the

schematic.

Prioritize the

placement by

organizing the high

speed or critical

components first at

closest length

Creating the PCB

Usually the more time you take in component

placement, the less time you will need for routing

Which placement is better and why ??? (L or R)

Creating the PCB

Which placement is better and why ??? (L or R)

Creating the PCB

Which placement is better and why ??? (L or R)

PCB Inspector

Start the PCB

Inspector.

This is one of the

most useful and

time saving

features in Altium

PCB Inspector

Hold down

control and

click both R14

and C10

The PCB

inspector

shows two

objects are

displayed/selec

ted.

PCB Inspector

Change the layer

from TOP to

BOTTOM, and all

selected objects are

immediately changed

to the bottom layer

This change moved

the component pads

from the top of the

board to the bottom

of the board and

mirrored them

PCB Inspector

We can now place R14 and

C10 underneath the USB

connector and make the

connection from the bottom of

the board.

Notice the pads are BLUE

(color code bottom layer), This

lets you know that these

components are on the bottom

of the board

Component Placement

Place the three

decoupling

capacitors on the

bottom layer, and

position them as

close to the power

pins as possible as

shown below

Component Placement

The current limiting

resistors can be

place on the bottom

of the board (under

the FT232 chip)

The RX and TX

indicator LEDs

should be placed on

the top of the board

Component Placement

This is beginning to

look very cramped

and hard to see

things which are

overlapping.

We don’t care

where the

component labels

(top overlay) go, and

will position them

last, so they are just

getting in the way

right now

Component Placement

Click on the LS at

the left of the list of

layers. This is to

change the active

Layer Set (Visible

layers)

This will bring up a

screen like that on

the right. Change

the setting to ‘Signal

Layers’

Component Placement

This shows only

SIGNAL LAYERS or

layers that conduct

electricity and hides

the rest of the layers

that we don’t care

about at the

moment.

Most of routing is

best done with the

Signal Layers

layerset active

Component Placement

It is much easier to look

for lines that cross over

here and make changes

with component

placement.

NOTE: Be careful when

placing components in

this mode. The top

overlay (silkscreen) is

sometimes used for

component boundaries

and you might place a

component inside the

boundary of another

part

Component Placement

Place the rest of the

components however you

want to

Routing

Now we need to make electrical connections

between the components

Click the icon to interactively route connections

NOTE: Whichever layer is active, the trace will

being on that layer

Routing

Make a connection

between two

components as

shown to the right.

Notice that the wire

itself is associated

with the net VCC

Routing

By lowering the ‘Masked Objects Factor’ in

the ‘Mask Level’ in the bottom right corner,

when you click on a pad to wire, such as VCC, it

will dull out the other connections to make it

easier to see where the connections need to go

Routing

You should

adjust this so

you can easily

see the

highlighted net,

but still see the

outlines of the

other pads

Routing

Press the TAB key while routing and you can

change the width of the trace for that particular

net, and specific hole sizes. Make VCC 15 mils

Routing

Notice the new VCC trace is 15 mils thick

Routing

Try to route this board using mostly perpendicular traces.

For example, use the bottom layer for horizontal traces, and the top

layer for vertical traces. This will make the routing much easier (at

the expense of more holes)

Routing

The connection on the

right is a differential pair at

a high frequency.

Differential pairs should be

kept closer together

Although you are using an

orthogonal method of

laying out the board,

Critical nets do not need

to apply.

Try to keep the layer

changes and discontinuities

to a minimum for critical

lines

Routing

As a general rule for right now, you want to make the traces about as

large as you can make them.

Why ?

Routing

When the USB

connector is

complete, there

should be four

traces coming

from the USB

interface to the

rest of the circuit

◦VCC

◦GND

◦TX

◦RX

Routing

The TX and RX

traces from the

FT232 Chip to

the rest of the

chip can be

relatively high

speed (1 MB/s)

For reasons we

will go over later,

this means we

should try to

maintain the same

geometry

throughout the

trace. (Don’t vary

the width)

Routing

When the routing is complete, you should

have something that looks like the picture

to the right.

VCC and GND connections are not all

complete though.

We will work on VCC first

Routing

In the left-hand drop down box at the top, select VCC. This will

highlight the VCC net

NOTE: The box to the right will highlight and jump to a particular

component.

Routing

The VCC net is highlighted

and there are three ‘ratsnest’

wires that need to be

connected.

Make the connections to

connect all the VCC’s

together

Routing

The VCC net is highlighted

and there are three ‘ratsnest’

wires that need to be

connected.

Make the connections to

connect all the VCC’s

together

Repeat the process for GND

Routing

When the routing is complete, there

should be no more ‘ratsnest’ wires

We must run a DRC (Design Rule

Check) to make sure there are no

errors.

Click TOOLS > Design rule check

Routing

Uncheck the box to create

a report file

Click Run Design Rule

Check

If there are no errors, you

should get an empty

message box like below

Routing

Change the Layer Set back to ALL LAYERS and view the entire board.

As you can see, we have a lot of wasted area, so this gives us a chance to

resize the board

Routing

Click and drag

the pink line to

the right to the

left, leaving

about 50 mils

spacing

between the

pink line and

the

traces/compon

ents

Routing

Notice the

dimensions are

automatically

fixed to the

new distance

between the

arrows

Repeat this

process with

the bottom

pink line

Routing

The board should look something like this.

Shift and click to select all four pink lines

Routing

Click

◦Design > Board Shape > Define from selected objects

Routing

The board should now be resized to the

new dimensions

NOTE: The pink line is a special line called

a Keep-Out layer. This is to prevent placing

components too close to the edge of the

board

This is technically not the smartest way to

change the board size, but the simplest to

see how it works.

If you want to change the board size on a

real board please let me know and I’ll show

you better methods

Cleaning Up The Design

Now we should clean up the design. The top overlay (silkscreen) are

overlapping VIAs so they wont show up well, the fonts are too big, and the

spacing is too close together

Cleaning Up The Design

Right click on any of the

top overlay (such as D1)

and click ‘Find Similar

Objects

Under String Type-

DESIGNATOR, change

from ANY to SAME. This

will select all designators

on the board

Cleaning Up The Design

You can see that all the

component designators are

selected, and nothing else

The PCB inspector shows

that 99 objects are selected

Change the ‘Text Kind’

from ‘Stroke Font’ to ‘True

Type’

Cleaning Up The Design

The changes are

immediately made and all

99 designators are changed

from stroke font to true

type font.

The reduced size and

cleaner font type already

makes the board look a lot

better

Cleaning Up The Design

P4 and P5 are not very intuitive to the end user and should probably be

changed to something more descriptive.

Also, the 8-bit LED display can also be changed to Bit0, Bit1, etc… or

1,2,4,8,… so a user can easily add the binary numbers

Cleaning Up The Design

Go back to the

schematic, and change P5

to ‘LED INPUT’

Change P1 to PORTB

Change P4 to PORTD

Change P2 to PORTC

Change P3 to ISP (In

circuit serial

programming)

Change D9 to TX

Change D10 to RX

We are making 7

changes to component

names here

Cleaning Up The Design

Click DESIGN > Update PCB Document

Dev Board

As a result of changing the component

names, some nets changed also. Apply all

changes except adding the room

Cleaning Up The Design

The changes have taken place and now we each connector is more descriptive

This method can also be used to change PCB footprints, etc…

Cleaning Up The Design

You can make the font larger or in bold, or change the font itself if you want to, just

double click the text to bring up the menu

These connectors will have pin headers on them once assembled, so the Pin 1

indicator with the rectangular pad will be invisible to us. We need to add a better

Pin 1 indicator.

Cleaning Up The Design

Click the place arc by edge

Place an arc anywhere on the board

Double click on the arc to get the

prompt below, change:

◦Radius = 5 mil

◦Width = 10 mil

◦Start Angle = End Angle = 0

◦Layer = Top Overlay

Cleaning Up The Design

Copy & Paste the arc and place next to

the Pin 1’s for the 10 pin headers

Cleaning Up The Design

We should create two new board layer

sets.

One where only items on the TOP of

the board are visible

One where items on the BOT of the

board are visible

Click the ‘LS’ at the bottom of the

screen and click ‘Board Layer Sets’

Cleaning Up The Design

Click ‘New Set’ in the bottom left

Click ‘Make Empty

Cleaning Up The Design

Name the set

‘TOP BOARD’

Check the

following boxes:

◦To p L ay e r

◦To p O v e r l ay

◦Multi-Layer

Cleaning Up The Design

Create another

new set called

‘BOT BOARD’

Check the ‘View

from bottom side’

Check the

following boxes:

◦To p L ay e r

◦To p O v e r l ay

◦Multi-Layer

Cleaning Up The Design

Select the TOP BOARD from the layer

set.

This is what the real board will look

like from the top looking down

without the default Superman ability to

see through all the layers

Cleaning Up The Design

This is the best view to

move the top

overlay/silkscreen layers

around to make sure it will

look good when you are

done.

NOTE: You should avoid the

holes with the top overlay,

but do not worry if the top

overlay is on top of a trace

Cleaning Up The Design

I have moved R10 and

R11 indicators to a

location with less

clutter and without

being blocked by a via.

Cleaning Up The Design

I have moved R10 and

R11 indicators to a

location with less

clutter and without

being blocked by a via.

Cleaning Up The Design

This is also the time

where you should

optimize your traces.

The trace on the top

image looks silly and

was probably done

because of optical

interference with the

bottom layer

Viewing ONLY the top

layer can help spot

errors easily and make

a clean and professional

looking PCB

Cleaning Up The Design

Set the active layer set to the BOT LAYER you made

Perform the same optimizations as with the top layer

Cleaning Up The Design

The image to the left shows a DRC error because the polarity marking for

the capacitors are too close together. This is not a real error and we don’t

care about it

The image on the right does not flag for an error, but the bottom overlay for

C1 will not show up properly because of the location of the via.

Does anyone notice anything else wrong with the image to the right ???

Cleaning Up The Design

Is anything wrong with the bottom overlay in this picture ?

Cleaning Up The Design

Our board looks OK, but there is a lot of

unused space

We will add what is called a ‘copper pour’ or

‘polygon pour’ to fill in the empty areas

Cleaning Up The Design

Click the polygon plane icon as

shown to the right

Change net to GND

Cleaning Up The Design

Click about 50-100 mils away from

the each corner and then right click

This will begin the polygon

calculation and placement.

NOTE: For large designs this can

take hours

Cleaning Up The Design

Notice how the polygon pour will

avoid a net that is different than

the net assigned to it.

It will put copper everywhere

possible that doesn’t create a

violation

Cleaning Up The Design

On nets that there

is a connection

(GND), you can

see it handles it

exactly the same

as any other net,

but has a few

short connectors

that connect the

pad/hole to the

pour

Cleaning Up The Design

Repeat this

process on the

bottom layer of

the board, also

connecting to

GND

PCB Complete!

Rather than trying to manually figure out what to

order, we can extract a bill of materials from the

design

This is why it was so important to enter all the

details in correctly earlier

Click ‘Bill of Materials’ as shown below

PCB Complete!

Check the box to ‘Open Exported’ and click

‘Export’

PCB Complete!

An Excel spreadsheet of the B.O.M. will open with

all the information you need to quickly order the

parts

PCB Complete!

From the PCB, click

File > Assembly

Outputs > Assembly

Drawings

PCB Complete!

This will create

Assembly

Drawings that are

helpful when

assembling the

parts.

Usually I print

these and write

the value of each

component where

the component

goes

PCB Complete!

To get the PCB

fabricated the

board house needs

two things:

◦Gerber Files

◦NC Drill Files

Follow the menu

sequence to obtain

the NC Drill files

first

PCB Complete!

Leave these values

as default unless

you know what

you are doing

Click OK

PCB Complete!

Leave these values

as default unless

you know what

you are doing

Click OK

PCB Complete!

A PCB with only

holes in it should

appear.

These holes match

the holes of your

design

Go back to the

PCB

PCB Complete!

Follow the menu

sequence to create

the output Gerber

files

PCB Complete!

Leave the values

intact under the

‘General’ tab

PCB Complete!

Under the Layers

tab, click ‘Plot

Layers’ and you

can either choose

ALL ON or USED

ON.

If you choose

USED ON you

should manually

check the bottom

two layers called

◦GPT – Top Pad

Master

◦GPB – Bottom Pad

Master

PCB Complete!

Under ‘Drill

Drawing’ (This is

different than NC

Drill files) check

the ‘plot all used

layer pairs’ in the

two locations at

the left

PCB Complete!

Under ‘Apertures’

make sure

Embedded Apertures

are selected

(RS274X)

NOTE: Before

RS274X, there was

RS274D, which did

not contain the

embedded

Apertures, most

everyone requires

RS274-X format

Ignore the Advanced

tab and click OK

PCB Complete!

Again, depending on

the complexity of

the design and the

capabilities of your

computer, this could

take hours.

This design should

take around 10

seconds

Notice how two

new files have been

created, These are

CAM files

PCB Complete!

The PCB Document is a single

document

The Gerber files are a list of

around 10-40 individual files

with information on each layer

This standardized format of

Gerber files means the board

house does not need to own

every software package

imaginable

CAM Viewers are required to

open these ‘generic’ Gerber

files. CAMtastic is Altiums

included CAM viewer

PCB Complete!

Highlight the CAMtastic file

with your board layout on it

Click the CAMtastic tab

PCB Complete!

Inside the CAM viewer, you

can see a rather crappy

rendition of your board and

a bunch of color coded files.

You may also notice there

are new buttons in the menu

screen. This is so you can

modify the output files

(Gerber files) directly.

PCB Complete!

You may notice a new chart that appears

in the Gerber files.

If you remember the .LEGEND from the

PCB layout, that is known as a SPECIAL

STRING which performs a special

function.

This particular one creates information

about the holes and represents this

information with symbols

PCB Complete!

Although it looks like

someone did graffiti on your

work, these patterns

represent the type of hole it

is, and the size of the hole

The + is the center of the

hole, and the pattern reveals

drill information from the

.LEGEND special string

NOTE: There are much

better CAM viewers than

Altium’s, Some are included

in my syllabus

PCB Complete!

When you

created the

Gerber files

and NC Drill

files, a new

folder is

automatically

created in

your project

folder called

‘Project

Outputs’

All these files

are what you

send to get

your board

made

Altium is nice

enough to

file extensions

with Windows

so you can

see which

each file is

PCB Complete!

Click Report > Board information for a quick

summary of your board

Click ‘REPORT’ and include this report file in

any project files you send me. POINTS

WILL BE TAKEN OFF IF IT IS NOT

INCLUDED

PCB Complete!

Click the ‘All On’ box and click ‘Report’

PCB Complete!

An HTML report file is created

(file path is given) and you can

select the units.

This HTML file has hyperlinks so

you can quickly view areas

PCB Complete!

Be careful with this one, The annular ring

size from board vendors is defined

differently. The Ring size is this

number divided by 2

PCB Complete!

What’s wrong with this ????

We specified a minimum trace width of

10 mils, yes we have 81 tracks with a

more narrow width. Is the DRC Broken ?

Special Strings

Type ‘L’ from the PCB screen and click the ‘View

Options’

Check the box that allows you to Convert Special

Strings

Special Strings

Click the Text Entry icon from the PCB menu

Double click on the text you placed to get the

following menu

Special Strings

Shown to the right

are all the available

Special Strings that

can be placed in

PCB Entry.

NOTE: This list

usually changes

with each revision

Part 2: Intermediate Guide

This portion of the guide contains more

advanced features as is geared towards:

◦Hardware Engineers

◦Signal Integrity Issues

◦Advanced Altium Designer features

Logos

The image you want to create a logo out of MUST be saved

as a MONOCHROME BITMAP file. This can be done by

opening the file in MS Paint and saving the file as shown in

the box below

Logos

The most requested feature people want

to know is how to implement a logo in

their design. There is a script located in

this directory

C:\Program Files\Altium Designer 6\Examples\

Scripts\Delphiscript Scripts\Pcb\PCB Logo Creator

Add Converter.Pas to your project. This

script will convert any Black and white

image to a PCB footprint.

Logos

Notice the different menu icons when

you have a script selected. From here, you

can click the small triangle button to

execute the script or press F9

Logos

Make sure to change the layer to TOP OVERLAY

(Silkscreen) and load the .BMP image. Notice there is an

option for scaling factor, and it shows image size.

Image size will be the dimensions of the logo in mils

once the conversion is complete. Using the scaling

allows you to make the exact dimensions you want for

the image

Logos

Depending on many factors, such as complexity,

and processing power, the converting time may

vary

When complete, there will be a new PCB

document added to your project containing your

logo. It is a good idea to copy & paste the logo

into your footprint library for future use

Logos

Logos can also include:

◦Compliance icons such as FCC, ROHS, CE,

etc..

◦Warnings such as ESD, High Voltage, Etc

◦Make sure you can legally use any logos you

place on your PCB

Multiple Monitor Setup

Schematic/PCB Interaction with

Multiple Monitors

Circuit Simulation

Version Control System

Snippets

Snippets allow for quick reuse of existing

designs.

Schematic, PCB, Routing can all be saved as

snippets.

Easily found by clicking the ‘System’ bar in

the bottom right corner, then enabling

‘Snippets’

Snippets

To create a snippet,

simply highlight the

schematic/pcb

information you

would like to reuse,

right click, then

select ‘Add to

Snippet’

Snippets

You can create multiple subfolders to keep your snippets

organized.

To place a snippet, simply highlight the snippet of your choice,

and click the ‘PLACE’ button at the top of the snippets box.

Snippets

When placing a snippet, you will see a rectangular boundary outline of the object. Once the location is

held, you will place the ENTIRE snippet as shown below.

Notice that nodes, net labels, differential pairs, and component ID’s are all pasted from the snippet.

When pasting a PCB snippet, the footprint, layer information, traces, etc.. Are all pasted from the

snippet

This powerful, simple to use feature is a great timesaving tool when creating multiple projects

Inspector Tools

The PCB and Schematic Inspector tools

for some reason are hidden a little deep

inside the software.

This feature allows you to easily and

quickly make project-wide changes to

components, nets, etc.

Serious users will be amazed at how

much time is saved by using the Inspector

tools

Schematic Inspector

Start out by

docking the

Schematic

Inspector. I

usually keep it

in the side

dockbar

which is

useful for a

multiple-

screen display.

Schematic Inspector

By selecting multiple objects (shift & left

click), you can see the Schematic

Inspector update the display for all

selected parts.

Items showing <…> have varying values

for more than one component (Such as

location X/Y coordinates)

Schematic Inspector

In this example,

Three

capacitors are

selected

Schematic

Inspector

shows that 3

objects are

selected in the

bottom of it’s

taskbar.

From this stage,

any value

changed inside

the inspector

will

immediately be

changed in ALL

SELECTED

OBJECTS

Schematic Inspector

Changes such as changing the part comment from 0.1uF

to 1uF are immediately visible in the schematic

Schematic Inspector

Allows changing a field with different values (Showing <…>) to make all values uniform

In the example below, component orientation is changed from <…> to 90 Degrees.

Immediately each component is rotated to the 90 degree position.

For this example, the lower two capacitors are unchanged, as their value was already 90 degrees,

and the top capacitor is rotated from 0 degrees to 90 degrees.

Find Similar Objects

The perfect complimentary tool used

with Inspector is the ‘Find Similar

Objects’ right click menu.

Find Similar Objects

To find ALL

capacitors with

a part comment

of 1uF we

change the

following

objects from

‘ANY’ to

‘SAME’

◦Description:

Capacitor

◦Part

Comment: 1uF

Click OK when

finished

Schematic Inspector- Find Similar

Objects

After hitting

‘Apply’ or ‘OK’,

the Schematic

Inspector

immediately finds

all matching parts.

In this case the

three capacitors

we changed

earlier to 1uF are

highlighted over

the rest of the

schematic, and

selected in the

Inspector.

PCB Inspector

PCB Inspector works similar

to the Schematic Inspector.

Shown below is an example of

finding and selecting all traces

that are 7 mils width on the

top layer only

Notice how quickly we

selected and can modify 744

objects meeting this criteria!!

PCB Inspector

We can almost immediately find any

group of objects on the PCB and change

values.

This is an important feature because it

will allow you to quickly adhere to

changes in project requirements, such as

fabrication trace-width parameters

Project Report

A quick detour from

the PCB Inspector

allows us to see a

general report on the

project

From the main

toolbar, click

‘Reports’ then Board

information

You will see a general

summary as shown

to the right, click on

the ‘Report’ button

Project Report

Select the

information you

want included in the

report.

Usually it is best to

select all and then

navigate to when you

want in the report

with hyperlinks

Click ‘Report’ when

done selecting

objects

Project Report

An HTML based

report will be

generated with a

table of contents

and hyperlink

navigation available

Project Report

The report

will probably

give more

information

than you will

ever want to

know, such as

a detailed

breakdown

of the

routing, layer

information,

vias, tracks,

etc..

Project Report

Shown below

is a part of the

report on

board holes.

This contains

EVERY hole

on the board,

and includes

the drill size

of the hole.

Report and PCB Inspector

Scenario: Your PCB Manufacturer tells you that your hole size must

be 20 mils in diameter, and that the holes in your submitted project

are 15 mils (As shown in the previous slide)

Go to the report to see a detailed analysis of the holes. For this

board we can see the smallest hole size we need to change is 15 to

20 mils, every other hole is larger

◦Use ‘Find similar objects’ to find pads/vias that match 15 mil hole size

◦In the PCB Inspector, we know from the report that we need to change

351 Vias, and 10 pads from 15 mils to 20 mils. We can see in the

Inspector window how many objects are selected.

◦Change the hole size from 15 to 20 mils using PCB Inspector

◦Find any clearance conflicts with the online DRC and quickly fix

◦Regenerate output files with smallest hole size = 20 mils

A process like this, to quickly find and modify 361 holes might take

just a few minutes rather than hours of finding and modifying each

pad/via manually.

Output Job File

Scale Print (1:1Footprint Verification)

PCB Tab

The Return Path

Bandwidth

Microstrips

Differential Pairs

Signal Integrity Introduction

Fourier Series and Transform

Physical Resistance

Physical Inductance

Physical Capacitance

Reflections

Multi-Layer Boards

The term ‘Multi-Layer board’ usually

refers to more than two layers.

A multi-layer board contains a lot more

information such as

◦Layer Stack

Layer Stack

A Layer Stack is a detailed report that contains information

on:

◦Physical Layers and ordering of layers

External signal layers

Internal signal layers

Internal planes

◦Copper thickness per layer (1oz = 1.4 mil, ½ oz = 0.7 mil)

◦Dielectric material and permittivity constant

◦Prepreg thickness

◦Core thickness

◦Total board thickness

This information is crucially important when implementing

transmission lines, microstrips, striplines, etc.

Internal Planes

Internal Signal Layers

Layer Stack

Design > Layer Stack

manager will show a

3D representation of

the layer stack

Layer Stack

Impedance Controlled Routing

Transmission lines usually required if:

Microstrip

Stripline

Reflections

Cross Talk

EMI

Output Files

CAM Viewers

CAM Viewers allow the re/viewing of Gerber files.

CAMTastic: Basic, Included in Altium Designer

http://www.altium.com/files/learningguides/AR0119%20CAMtastic%20Introduction.pdf

ViewMate- Pentalogix FREE Gerber Viewer

http://www.pentalogix.com/Download/download.html

CAMMaster- Pentalogix

http://www.pentalogix.com/Products/CAMMaster/cammaster.html

CAM350- Downstream Technology

http://www.downstreamtech.com/cam350.html

GC Prevue- FREE Gerber Viewer

http://www.graphicode.com/

GerbTool- Wise Software

http://www.wssi.com/index.php?option=com_content&task=section&id=16&Itemid=1

IPC: Formerly known as

Institute of Interconnecting and Packaging Electronic Circuits

IPC Guides the electronic

interconnection industry through

dramatic changes. IPC brings together

designers, board manufacturers, assembly

companies, suppliers, and OEM’s.

IPC is responsibly for creating over 200

standards

IPC: Certification

IPC also has a certification program which

allows one to be certified as:

◦Certified Interconnect Designer (C.I.D.)

Proves a designer’s knowledge of how to transform

a schematic into a reliable rigid PCB design.

◦Advanced Certified Interconnect Designer

(C.I.D.+)

Recognition of a designer’s accomplishments. Exam

covers forty key objectives which go beyond the

C.I.D. certification.

IPC: C.I.D. Certification

Interested individuals who wish to be

certified should obtain the following articles:

◦IPC-2221A: Generic Standard on Printed Board

Design ($30 members/$60 nonmembers)

◦IPC-2222: Sectional Standard on Rigid Organic

Printed Boards ($20/$40)

◦IPC-D-325A: Documentation Requirements for

Printed Circuit Boards ($25/$50)

◦IPC-T-50G: Terms and Definitions for

Interconnecting and Packaging Electronic

Circuits ($40/$80)

◦PWB-CRT-SGA: PWB Designer Certification

Study Guide ($35/$70)

IPC: C.I.D. Certification

Shown to the right

are some of the

sample questions

available on the IPC

Website

IPC: For More Information

IPC Homepage

http://www.ipc.org/

Online Store – Purchase Articles

http://webvision.ipc.org/scripts/mgrqispi.dll?APPNA

ME=IPCWEB&PRGNAME=TOCFRAME&ARGUME

NTS=-N,-N,-A,-A,-N50

Certification

http://dc.ipc.org/certification.htm

Keyboard Shortcuts

References

Bogatin, Eric. Signal Integrity- Simplified. Upper

Saddle River, NJ: Prentice Hall, 2006

Schmitt, Ron. Electromagnetics Explained.

Boston, MA: Newnes, 2002

Johnson, Howard, and Graham, Martin. High

Speed Signal Propagation- Advanced Black

Magic. Upper Saddle River, NJ: Prentice Hall,

2003

Altium Designer Learning Guides

http://www.altium.com/community/support/lea

rningguides/altiumdesigner6learningguides/

Microsoft Altium_Designer_Intermediate_Guide [Compatibility Mode] Altium Designer Intermediate Guide

Altium_Designer_Intermediate_Guide

Altium_Designer_Intermediate_Guide

Altium_Designer_Intermediate_Guide

Navigation menu

Versions of this User Manual:

Views

Navigation