PDF Archive

Easily share your PDF documents with your contacts, on the Web and Social Networks.

Share a file Manage my documents Convert Recover PDF Search Help Contact



Altium Notes .pdf



Original filename: Altium_Notes.pdf

This PDF 1.4 document has been generated by LaTeX with hyperref package / pdfTeX-1.40.3, and has been sent on pdf-archive.com on 17/03/2018 at 01:54, from IP address 142.3.x.x. The current document download page has been viewed 536 times.
File size: 5 MB (75 pages).
Privacy: public file




Download original PDF file









Document preview


Introduction to Altium Designer
Unified Design Environment

EEESAU
March 2010

ii

c
Copyright 2010
by Gabriel Haines

Written by Gabriel Haines

iii

Preface
This document is intended to provide an introduction to Altium Designer, suitable for
users with little or no experience in the use of EDA tools or CAD software. The content
of this document has been arranged in a consecutive order, presenting information when
it is needed and reflecting how the design process progresses (design flow). Although
reading in a consecutive order is recommended, chapters or sections may be read in any
order.
This document has been written for the Altium Designer Summer 09 release. Whilst
the majority of topics and functionality discussed should be applicable to previous versions, not all features may be present or operate in the same exact way. For example, the
user interface and basic structure has not changed much if at all, but certain functions and
features like 3D PCB, FPGA Instruments, and online supplier linking may have changed
since previous versions. Content contained in this document based on the authors experience, Altium help files & manuals, and content found in the Altium Training Manuals [1]

Contents
1

2

Introduction

1

1.1

Overview of the Altium Designer Environment . . . . . . . . . . . . . .

1

1.2

Workspace Panels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1

1.3

Shortcut Keys, Pop-up & context Sensitive Menus . . . . . . . . . . . . .

2

1.4

Creating & Using Projects . . . . . . . . . . . . . . . . . . . . . . . . .

3

1.4.1

Project Types . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3

1.4.2

Creating a Project . . . . . . . . . . . . . . . . . . . . . . . . . .

4

1.4.3

Project Workspace Panel . . . . . . . . . . . . . . . . . . . . . .

4

1.4.4

Adding and Removing Files From a Project . . . . . . . . . . . .

4

1.4.5

Project Packager . . . . . . . . . . . . . . . . . . . . . . . . . .

5

1.5

Help System . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5

1.6

Version Control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6

1.6.1

Getting Subversion . . . . . . . . . . . . . . . . . . . . . . . . .

6

1.6.2

Subversion Servers & Repositories . . . . . . . . . . . . . . . . .

7

1.6.3

Interfacing SVN with Altium Designer . . . . . . . . . . . . . .

7

1.6.4

Using Subversion in Altium Designer . . . . . . . . . . . . . . .

7

1.6.5

Further Reading on Version Control . . . . . . . . . . . . . . . .

9

Schematic capture

10

2.1

Introduction to the Schematic Editor . . . . . . . . . . . . . . . . . . . .

10

2.1.1

Navigating around schematics . . . . . . . . . . . . . . . . . . .

11

2.1.2

Schematic Objects . . . . . . . . . . . . . . . . . . . . . . . . .

11

2.1.3

Filling in the Title Block . . . . . . . . . . . . . . . . . . . . . .

11

2.1.4

Using Templates with Existing Title Blocks . . . . . . . . . . . .

13

Library System . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13

2.2.1

Browsing & Adding Libraries . . . . . . . . . . . . . . . . . . .

14

2.2.2

Library Panel . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15

2.2.3

Searching for a Component . . . . . . . . . . . . . . . . . . . .

15

Component Placement . . . . . . . . . . . . . . . . . . . . . . . . . . .

17

2.3.1

Placing Components . . . . . . . . . . . . . . . . . . . . . . . .

17

2.3.2

Annotation . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17

2.3.3

Editing Component Parameters . . . . . . . . . . . . . . . . . .

18

2.2

2.3

CONTENTS
2.3.4
2.4

2.5

3

Linking Components to Suppliers . . . . . . . . . . . . . . . . .

20

Component Connections, Buses & Harnesses . . . . . . . . . . . . . . .

21

2.4.1

Wires & Nets . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21

2.4.2

Power Ports . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22

2.4.3

Buses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22

2.4.4

Harnesses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

23

Multi Sheet Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

24

2.5.1

Flat and Hierarchical Design Structure . . . . . . . . . . . . . . .

24

2.5.2

Multi Sheet Connectivity . . . . . . . . . . . . . . . . . . . . . .

25

2.5.3

Connecting Sheets in a Hierarchical Design . . . . . . . . . . . .

26

2.5.4

Synchronising Sheets in a Hierarchical Design . . . . . . . . . .

26

Design Verification

28

3.1

Compiling Schematics and Projects . . . . . . . . . . . . . . . . . . . .

28

3.1.1

Setting Compiler Options . . . . . . . . . . . . . . . . . . . . .

28

3.1.2

Compiling and Compiler Errors . . . . . . . . . . . . . . . . . .

29

Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

30

3.2.1

Simulation Models for Components . . . . . . . . . . . . . . . .

30

3.2.2

Simulation Sources and Objects . . . . . . . . . . . . . . . . . .

30

3.2.3

Simulation Settings . . . . . . . . . . . . . . . . . . . . . . . . .

31

3.2.4

Running and Viewing Simulation Data . . . . . . . . . . . . . .

32

3.2.5

Creating a Bode Plot . . . . . . . . . . . . . . . . . . . . . . . .

33

Signal Integrity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

35

3.3.1

Before Starting Signal Integrity . . . . . . . . . . . . . . . . . .

35

3.3.2

Starting Signal Integrity for the First Time . . . . . . . . . . . . .

36

3.3.3

Signal Integrity Panel . . . . . . . . . . . . . . . . . . . . . . . .

36

3.3.4

Signal Integrity Settings and Stimulus . . . . . . . . . . . . . . .

37

3.3.5

Setting Design Rules . . . . . . . . . . . . . . . . . . . . . . . .

37

3.3.6

Simple Signal Integrity Example . . . . . . . . . . . . . . . . . .

39

3.2

3.3

4

v

PCB Design

41

4.1

Creating a PCB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

41

4.2

PCB Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

43

4.2.1

Board Options and Grids . . . . . . . . . . . . . . . . . . . . . .

43

4.2.2

PCB Layers . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

43

4.2.3

Layer Stack Manager . . . . . . . . . . . . . . . . . . . . . . . .

45

4.2.4

Design Rules . . . . . . . . . . . . . . . . . . . . . . . . . . . .

46

4.3

Transferring a Schematic Design to a PCB . . . . . . . . . . . . . . . . .

47

4.4

Rooms and Component Placement . . . . . . . . . . . . . . . . . . . . .

48

4.5

Holes and Board Cutouts . . . . . . . . . . . . . . . . . . . . . . . . . .

49

4.6

Routing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

49

vi

5

CONTENTS
4.6.1

Routing Tracks . . . . . . . . . . . . . . . . . . . . . . . . . . .

49

4.6.2

Placing Vias . . . . . . . . . . . . . . . . . . . . . . . . . . . .

51

4.6.3

Polygon Pours . . . . . . . . . . . . . . . . . . . . . . . . . . .

52

4.6.4

Impedance Controlled Routing (Microstrip) . . . . . . . . . . . .

53

4.7

Signal Integrity from PCB . . . . . . . . . . . . . . . . . . . . . . . . .

54

4.8

3D PCB Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

55

Creating and Editing Libraries

57

5.1

Schematic library editor . . . . . . . . . . . . . . . . . . . . . . . . . . .

57

5.1.1

Creating a Component Symbol . . . . . . . . . . . . . . . . . . .

57

5.1.2

Pin Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . .

59

5.1.3

Component Properties . . . . . . . . . . . . . . . . . . . . . . .

59

5.1.4

Linking a Symbol to a Footprint . . . . . . . . . . . . . . . . . .

59

5.1.5

Linking to Suppliers . . . . . . . . . . . . . . . . . . . . . . . .

60

5.1.6

Updating Changes from a Library . . . . . . . . . . . . . . . . .

60

PCB library editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

60

5.2.1

Creating a Footprint Manually . . . . . . . . . . . . . . . . . . .

61

5.2.2

Creating a Footprint using the Footprint Wizard . . . . . . . . . .

62

5.2.3

Creating Simple 3D Bodies . . . . . . . . . . . . . . . . . . . .

63

5.2

6

Project Outputs

65

6.1

Bill Of Materials . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

65

6.2

Smart PDF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

66

6.3

Output Jobs and Cam Output . . . . . . . . . . . . . . . . . . . . . . . .

66

6.3.1

67

Gerber Output . . . . . . . . . . . . . . . . . . . . . . . . . . .

Chapter 1
Introduction
1.1

Overview of the Altium Designer Environment

Altium Designer is an advanced electronic design automation (EDA) software tool. Unlike traditional EDA software that has functionality split into discrete modules/ programs
(for tasks such as schematic capture & PCB design), Altium offers a complete design
solution from one integrated software platform. The platform is focused on uniting and
integrating all aspects of electronic product development into one application, hence the
term “Unified Design Environment”.
Altium Designer has always featured schematic capture and PCB design, but also contains a wide range features to assist in many aspects of electronic design. This includes
circuit simulation, signal integrity analysis, FPGA & HDL integration, embedded software tools & compilers, bill of materials, formal report generation and CAM output to
name a few.
When starting Altium Designer, by default the home view is displayed, as shown below
in Figure 1.1. The home view itself displays the current license status, available updates,
and a task list to offer easy access to common functions and specific documentation. On
the left and right of the main window (and the bottom in the case of Figure 1.1) are the
workspace panels. The very top of the window contains the system menu and toolbar.
These menus and toolbars change depending on which type of document is being edited.
Sections of the toolbar can be enabled/disabled by right clicking the toolbar, then selecting the desired item in the popup menu. The top right corner contains the view navigation
toolbar. This toolbar shows the location of the current file, and also offers forward & back
buttons in a similar style to a web browser. Below the System menu & toolbar, but above
the home view window is the document bar. Every time a document is opened, a tab is
placed into the document bar.

1.2

Workspace Panels

The workspace panels provide a lot of the functionality in Altium Designer. They can be
dragged out into their own floating panels, or docked into the main window along one of
the four borders. Holding the CTRL key while dragging a panel will stop it from joining
a group of panels. The panel on the right hand side of the window is set to pop out by
default when one of the labels is clicked. Pop out functionality can be enable or disabled

2

Introduction

System Toolbar

View Navigation
Toolbar

Document Tab

System Menu

Workspace Panel
(set to popout)
Workspace Panel

Main Window /
Document Editing Area
Workspace Panel

Panel Controls

Figure 1.1: Altium Designer home view.
by clicking on the push pin icon in the top right hand corner of the respective panel or
group of panels.
There are two types of panels: system panels and editor panels. System panels are always available (e.g. Project, Files, Output). Editor panels (e.g. PCB library, schematic
library) are only available when certain types of documents are being edited.
In the bottom right corner are the panel controls. These buttons display menus listing
all available panels. If a certain panel has been closed, it can be opened again using
these controls. The panel controls can also be found in the system menu under View →
Workspace Panels. The workspace layout can be reset to factory default by clicking
View → Desktop Layouts → Default.

1.3

Shortcut Keys, Pop-up & context Sensitive Menus

The use of shortcut keys is quite intuitive and powerful. System menu commands can
be accessed simply by pressing the key that corresponds to the underlined letter in that
command name. Pressing a shortcut key will cause the corresponding system menu to
pop-up under the mouse cursor. For example, to create a new schematic file, click File →
New → Schematic, or simply press F N S. The panel control menus can also be accessed
by pressing k. Unlike most windows applications, the ALT key is not needed to activate
menu shortcuts when a document is opened in the document editor.

1.4 Creating & Using Projects

3

A panel containing a full list of shortcuts can be opened using the panel controls by
pressing K then clicking Help → Shortcuts. A list of shortcuts can also be found on the
Altium online wiki by clicking Help → Altium Wiki → Shortcut Keys
Context sensitive menus can be accessed in a document simply by right clicking an object, or the document itself. These menus are called context sensitive because the menu
that pops-up depends on what object if any was clicked. Many of the relevant commands
from the system menu appear in the context sensitive menu. Figure 1.2 shows the context
sensitive menu after right clicking on a component.

Figure 1.2: Component Context Sensitive Menu

1.4
1.4.1

Creating & Using Projects
Project Types

Projects are how Altium designer collects and organises all the source files & settings that
make up a physical project. There are 6 types of Projects available (shown with their file
extension):

• PCB Project (.PrjPcb)
• FPGA Project (.PrjFpg)
• Core Project (.PrjCor)
• Library Packages (.PrjPkg)
• Embedded Project (.PrjEmb)
• Script Project (.PrjScr)


Related documents


adoh workingwithpanels 040713 1023 23232
adoh tutorial gettingstartedwithpcbdesign 030713 1310 21746
adoh schematiceditingessentials 040713 0905 23120
adoh gettingreadytoroute 080713 1409 29052
altium notes
solar light tower harvey mudd


Related keywords