User manual ALTIUM DESIGNER 6 - MODULE 4 - PCB DESIGN

PCB Design Training Module Software, documentation and related materials: Copyright © 2006 Altium Limited. All rights reserved. You are permitted to print this document provided that (1) the use of such is for personal use only and will not be copied or posted on any network computer or broadcast in any media, and (2) no modifications of the document is made. Unauthorized duplication, in whole or part, of this document by any means, mechanical or electronic, including translation into another language, except for brief excerpts in published reviews, is prohibited without the express written permission of Altium Limited. Unauthorized duplication of this work may also be prohibited by local statute. Violators may be subject to both criminal and civil penalties, including fines and/or imprisonment. Altium, Altium Designer, Board Insight, CAMtastic, CircuitStudio, Design Explorer, DXP, LiveDesign, NanoBoard, NanoTalk, Nexar, nVisage, P-CAD, Protel, SimCode, Situs, TASKING, and Topological Autorouting and their respective logos are trademarks or registered trademarks of Altium Limited or its subsidiaries. Microsoft, Microsoft Windows and Microsoft Access are registered trademarks of Microsoft Corporation. OrCAD, OrCAD Capture, OrCAD Layout and SPECCTRA are registered trademarks of Cadence Design Systems Inc. AutoCAD is a registered trademark of AutoDesk Inc. HP-GL is a registered trademark of Hewlett Packard Corporation. PostScript is a registered trademark of Adobe Systems, Inc. All other registered or unregistered trademarks referenced herein are the property of their respective owners and no trademark rights to the same are claimed. PCB Design training module ii PCB Design Training Module 1. 1. PCB design process ................................................................................................. 4-1 The PCB Editor workspace ...................................................................................... 4-3 1.1 PCB Panel ...................................................................................................... 4-3 1.2 Using the PCB Editor panel to browse........................................................... 4-4 1.3 PCB Editor Preferences ................................................................................. 4-9 1.4 Board Options dialog.................................................................................... 4-25 1.5 Board Layers and Colors.............................................................................. 4-26 1.6 The PCB coordinate system......................................................................... 4-27 1.7 Grids ............................................................................................................. 4-27 Browsing footprint libraries ................................................................................... 4-29 Creating a new PCB ................................................................................................ 4-30 3.1 Creating the Blank PCB ............................................................................... 4-30 3.2 Defining a sheet template.............................................................................4-30 3.3 Defining the Board Shape, and Placement / Routing Boundary................ 4-31 3.4 Exercise ­ Creating a board outline & placement / routing boundary.......... 4-32 Transferring design information to the PCB............................................................. 4-34 4.1 Design synchronization ................................................................................4-34 4.2 Resolving synchronization errors ................................................................. 4-35 4.3 Design transfer using a netlist ...................................................................... 4-36 4.4 Exercise ­ Transferring the design .............................................................. 4-37 Setting up the PCB layers ...................................................................................... 4-38 5.1 Enabling Layers............................................................................................ 4-38 5.2 Layer definitions ........................................................................................... 4-39 5.3 Defining the Electrical Layer Stackup .......................................................... 4-41 5.4 Defining Mechanical layers .......................................................................... 4-43 5.5 Internal power planes ................................................................................... 4-43 5.6 Exercise ­ Setting up layers......................................................................... 4-45 Design rules and design rule checking ................................................................ 4-46 6.1 Adding design rules...................................................................................... 4-46 6.2 Design rules concepts .................................................................................. 4-47 6.3 How rules are checked.................................................................................4-49 6.4 Where rules apply ........................................................................................ 4-50 6.5 Object classes .............................................................................................. 4-52 6.6 From-tos ....................................................................................................... 4-53 6.7 Exercise ­ Setting up the design rules......................................................... 4-53 6.8 Design Rule Checking..................................................................................4-54 Component Placement tools.................................................................................. 4-56 7.1 Placing components ..................................................................................... 4-56 7.2 Finding components for placement .............................................................. 4-56 7.3 Moving components .....................................................................................4-57 7.4 Interactive Placement commands ................................................................ 4-58 7.5 Auto Placement ............................................................................................ 4-59 7.6 Re-Annotation .............................................................................................. 4-59 7.7 Exercise ­ Component Placement............................................................... 4-60 Routing..................................................................................................................... 4-61 2. 3. 4. 5. 6. 7. 8. PCB Design training module iii 8.1 8.2 9. Interactive routing......................................................................................... 4-61 Automatic routing ......................................................................................... 4-67 Polygons .................................................................................................................. 4-69 9.1 Placing polygons .......................................................................................... 4-69 9.2 Exercise ­ Working with polygons ............................................................... 4-72 Output Generation .................................................................................................. 4-73 10.1 Creating a new Output Job file..................................................................... 4-73 10.2 Setting up Print job options ..........................................................................4-74 10.3 Creating CAM files ....................................................................................... 4-75 10.4 Running the Output Generator ..................................................................... 4-78 10.5 Exercise ­ adding an OutJob file to the project............................................ 4-78 10. PCB Design training module iv 1. PCB design process The PCB Design training day covers how to use the PCB Editor to create a PCB from setup, through component placement, routing, design rule checking and CAM output. This first section looks at the overall PCB design process. The diagram below shows an overview of the PCB design process from schematic entry through to PCB design completion. Figure 1. Overview of the PCB Design Process PCB Design training module 4-1 Once the PCB design is completed and verified, the Create Manufacturing Output process is used to generate the PCB output files. This process is outlined below in Figure 2. Figure 2. Work flow for generating PCB output files PCB Design training module 4-2 2. The PCB Editor workspace This section investigates how to browse through a PCB design and how to set up the workspace preferences and other document options, such as layers and grids. 2.1 PCB Panel The PCB panel provides a powerful method of examining the contents of the PCB workspace. Clicking on an entry in the panel will filter the workspace to highlight that object ­ the highlighting will depend on the settings of the options at the top of the panel. To begin with, enable all the options. 2.1.1 Browse mode selection list The drop down list at the top of the panel allows you to list, locate or edit the following PCB object types in the active PCB document: · Components (and then Component Classes) · Nets (and then Net Classes) · From-Tos · Split Planes · Design Rules & Design Rule Violations. · Differential Pairs When you select an object in the panel, it will be highlighted in the workspace, according to the options at the top of the panel. Each Browse function is described in the following pages. 2.1.2 MiniViewer The MiniViewer is located at the bottom of the panel and provides an overview of the workspace. The double-lined rectangle indicates the current region being displayed in the workspace. The MiniViewer also has the following display control functions: · Click and drag in the rectangle to pan around the workspace. · Click and drag on a corner of the rectangle to change the magnification of the workspace. Figure 3. PCB Editor panel PCB Design training module 4-3 2.2 2.2.1 Using the PCB Editor panel to browse Browsing nets and net classes · To browse nets, select Nets from the dropdown list in the PCB panel. · Click on All Nets in the Net Classes region of the dialog to browse all nets on the PCB. The nets are listed in the region below and they are also highlighted on the PCB. · If the design includes Net Classes these are also listed. Net classes such as D[0..7] have been generated automatically from busses in the design. · Click on a net name in the Nets region to choose it ­ all the objects that belong to that net are listed in the Net Items region. Also, the net is highlighted on the PCB. · Click on an item in the Net Items region and note that it is highlighted on the PCB. Also note that the object that you clicked on is selected. · Multi-select keys are supported. Hold SHIFT or CTRL as you click on entries in the list. · Right-click in the Net Items section and note that you can control which net items are displayed. · Double-click on a net name to open the Edit Net dialog. Here you can change the net name, add or remove nodes from the net and define the color of the connection lines for this net. · The Nets and the Net Items region have multiple columns. Note that you can control the sorting by clicking the heading on a column. · Type-ahead is supported. You can type on the keyboard to jump through the lists. Press Esc to abort the current type-ahead search and start another. Figure 4. Browsing nets from the PCB panel PCB Design training module 4-4 2.2.2 Browsing components and component classes · To browse components, select Components from the drop-down list. · When the panel is being used to filter (highlight) components, you might find it better to have the Select option at the top of the panel switched off. · Click on All Components in the Components Class region to browse all components on the PCB. The components are listed in the Components region, as well as being highlighted on the display. · If the design includes component classes, these are listed too, when you click on a component class only the components in that class are listed and highlighted. · Click on a component name in the Components region to choose it. All the objects that belong to that component are listed in the Component Primitives region. Also, the component is highlighted on the PCB. · Click on an item in the Component Items region, Note that it is highlighted on the PCB. Also note that the object that you clicked on is selected. · Multi-select keys are supported. Hold SHIFT or CTRL as you click on entries in the list. · Right-click in the Component Items section. Note that you can control which component primitives are displayed. · Double-click on a component name to open the Component dialog where you can modify any attribute of the component. · The Components and the Component Items region have multiple columns. Note that you can control the sorting by clicking the heading on a column. · The order of the columns can also be changed; click and drag a column to change the column order. This is handy when you wish to use the type-ahead feature on a different column. · Type-ahead is supported. You can type on the keyboard to jump through the lists. Press ESC to abort the current type-ahead search and start another. The type-ahead is always performed on the left-most column, so drag any column to make it the left-most. Figure 5. Browsing components from the PCB panel PCB Design training module 4-5 2.2.3 Browsing design rules and rule violations To browse design rules, select Rules from the drop-down list. All Rules classes are listed. · Click on a Rule Class and all rules defined for that class are listed in the Rules list. · Click on a rule in the Rules list to highlight all objects targeted by that rule. · Double-click on the rule to display a dialog to edit that rule. · If the selected rule is in violation, all violating objects are listed in the Violations region. To check all rules for violations, select [All Rules] in the Rule Classes section. · Click on a violation to highlight the object causing the violation. · Double-click on a violation to display the Violation Details dialog which details the rule that is being violated and the parameters of the primitive that is causing the violation. · For more information about design rule checking and violations, refer to 7.3 How rules are checked. Figure 6. Browsing design rules from the PCB panel PCB Design training module 4-6 2.2.4 From-To editor · Choose From-To Editor from the drop-down field at the top of the PCB panel. The top list section of the panel will fill with all nets currently defined for the design. · As you click on a net entry, all of the nodes on that net will be loaded into the middle list section of the panel. Filtering will be applied and a mask automatically used in order to leave just the nodes (pads) on the net fully visible. All other objects are dimmed. · Double-click on a net entry to open the Edit Net dialog where you can edit the properties of the net. · To add a new from-to, select the Nodes on Nets to which you want to add the from-to and click the Add From To button. The new from-to appears in the From-Tos on Net section. Click on the from-to in the From-Tos on Net section and click on Generate and select a from-to topology, e.g. Shortest, Daisy varieties or Starburst. · The From-To editor can only be used to create fromtos. To browse for existing from-tos, create a query in the Filter panel using the IsFromto keyword. · Note that all connection lines, other than those that have been defined as From-Tos on the currently selected net, will remained dimmed. Switch the panel back to Nets to restore the display of connection lines. Figure 7. The From-To Editor in the PCB panel 2.2.5 Split Plane editor · You can review and edit split planes in the PCB panel by selecting the Split Plane Editor from the drop-down list at the top of the panel. · Select the plane you want to display by clicking on the Plane name. The split planes and their nets on that power plane are listed. · Click on a split plane name in the Split Planes and Nets section to show the pads and vias on that split plane. · Double-click on a split plane name to edit the net associated with the split plane. · Right-click on a split plane name to select an option from the menu. Figure 8. Use the Split Plane Editor to display split planes PCB Design training module 4-7 2.2.6 Differential Pairs Editor · You can review and edit Differential Pairs in the PCB panel by selecting the Differential Pairs Editor from the drop-down list at the top of the panel. · Select the Differential Pair Class you want to display by clicking on the Differential Pair Class name. The Differential Pair Designators will then be listed. · Click on a Differential Pair name in the Differential Pair section to show the constituent nets of the pair, both positive and negative. · Double-click on a Differential Pair name to edit the nets associated with the Pair and view the options. · Right-click on any Differential Pair Class listing (Excepting the default class of All Differential Pairs) and the Object Class Explorer dialog will open allowing you to modify your Classes. Figure 9. Use the Differential Pairs Editor to display Differential Pairs. 2.2.7 Exercise ­ Browsing a PCB document In this exercise, you will examine the various ways to browse through a PCB document. 1. Open the document 4 Port Serial Interface.PcbDoc located in the \Altium Designer 6\Examples\Reference Designs\4 Port Serial Interface folder. 2. Choose the Fit Board view command. Try the other view control options in the View menu. 3. Use the MiniViewer to move around the board. 4. Browse each object type and observe how the display changes as you click in the different sections of the panel. As you do, try the Mask, Select and Zoom options. PCB Design training module 4-8 2.3 PCB Editor Preferences The Preferences dialog allows you to set up parameters relating to the PCB Editor workspace. This dialog is displayed using the Tools » Preferences menu command. Settings in this dialog are stored with the Altium Designer environment, so they remain the same when you change active PCB files. The options in each of the pages are described below. 2.3.1 General page Figure 10 General page of the PCB preferences Editing options Online DRC When checked, any design rule violations are flagged as they occur. The design rules are defined in the PCB Rules & Constraints Editor dialog (select the Design » Rules menu command). Snap to Center When checked, the cursor snaps to the centre when moving a free pad or via, snaps to the reference point of a component, or snaps to the vertex when moving a track segment. Smart Component Snap When enabled, cursor jumps to center of nearest component pad rather than the component reference. PCB Design training module 4-9 Double Click Runs Inspector When enabled, double-click opens the Inspector instead of the object's traditional dialog. Remove Duplicates With this option enabled, a special pass is included when data is being prepared for output. This pass checks for and removes duplicate primitives from the output data. Protect Locked Objects When checked, locked objects cannot be moved. If they are part of a selection that is being moved, you will be asked to confirm the action. Confirm Selection Memory Clear Eight selection memories are available ­ click the button at the bottom of the workspace to display the Selection Memory controls (press F1 over the panel for details of the shortcuts for using the selection memory). The Selection Memories work just like a calculator -- the selection state of objects can be stored, recalled and added to on storage or recall. Enable this option to display a warning dialog when the contents of a section are to be cleared. Click Clears Selection The selection behavior in Altium Designer is like all other Windows applications, i.e. when you click on an object, it is selected and when you click away from that object, it is deselected. If this option is disabled, clicking away from an object no longer deselects it. If this option is off, you use the Deselect options in the Edit menu. Shift+Click to Select Rather than simply clicking on an object to select it, you can configure Altium Designer to require that the SHIFT key must be depressed when clicking to select it. Press the Primitives button to choose which objects will require Shift+Click to select. Popular choices include rooms, polygons and components. Preserve Angle When Dragging Enable this option so that when the tracks are being dragged on the PCB document, the angles of these track segments are preserved, maintaining the routing quality. You can also create new segments by dragging the drag handles, while holding down the Alt key before performing the drag operation will revert to the previous behavior. The new drag method also has an avoid obstacle mode which is toggled with the Shift + R short cut. Smart Track Ends If this Smart Track Ends option is enabled the net analyzer will attempt to keep connection lines attached to the ends of the tracks. For example, if you start routing from a pad, and then stop the routing (leaving the track end in free space), the net analyzer will attach the connection line to the track end rather than the originating pad. Note: The connection line can be either as a solid or dotted line in this mode. A solid line denotes that there is no routing topology rule assigned, and the net analyzer simply connects the various sub nets at their nearest locations. A dotted connection line denotes that there is a routing topology rule for this net and the net analyzer attempts to obey this topology rule by drawing a partially routed connection. PCB Design training module 4 - 10 Other section Undo/Redo This sets the undo stack size, i.e. the number of undo/redos available. Note that the higher the number, the more memory required. For object intensive operations, like autorouting or copying and pasting the entire board, the memory usage can be significant. Rotation Step When an object that can be rotated is floating on the cursor, press the SPACEBAR to rotate it by this amount in an anti-clockwise direction. Hold the SHIFT key while pressing the SPACEBAR to rotate it in a clockwise direction. Cursor Type Set the cursor to a small or large 90-degree cross, or a small 45-degree cross. Component Drag This option determines how connected tracks are dealt with when moving a component. When Connected Tracks is selected, tracks drag with the component; otherwise, they do not. If the Connected Tracks option for components is set, components cannot be rotated while being moved. Autopan options Style If this option is enabled, Autopan becomes activated when there is a crosshair on the cursor. There are six Autopan modes: · Re-Center -- re-centers the display around the location where the cursor touched the window edge. It also holds the cursor position relative to its location on the board, bringing it back to the centre of the display. · Fixed Size Jump -- pans across in steps defined by the Step Size. Hold the SHIFT key to pan in steps defined by the Shift Step Size. · Shift Accelerate -- pans across in steps defined by the Step Size. Hold the SHIFT key to accelerate the panning up to the maximum step size, defined by the Shift Step Size. · Shift Decelerate -- pans across in steps defined by the Shift Step Size. Hold the SHIFT key to decelerate the panning down to the minimum step size, defined by the Step Size. · Ballistic -- pans at maximum speed. · Adaptive -- pans at the rate set in the Speed field. Speed When Adaptive is enabled, the panning speed for Autopanning is set in mils/sec or pixels/sec. Step and Shift Step Size Some of the Autopan styles require step sizes. These options set the distances that define the autopanning step distance and the step distance when you hold down the SHIFT key while autopanning. The default distances are in mils or mms and the larger the number, the faster the panning speeds. Polygon Repour This has three options for determining whether a polygon repours when edited: · Never -- no automatic repour. PCB Design training module 4 - 11 · Threshold -- if selected, polygons with more than the Threshold Number of primitives will prompt to confirm repour, before performing the repour. · Always -- polygon always repours. 2.3.2 Display page Figure 11 Display page of the PCB preferences Display options section Convert Special Strings When enabled, special strings that can be interpreted on screen are converted and displayed, rather than simply displaying the special string text. Regardless of this setting, all special strings are converted when output is generated, e.g. printed. Redraw Layers Forces a screen redraw as you toggle through layers with the current layer being redrawn last Transparent Layers Gives layer colors a `transparent' nature by changing the color of an object that overlaps an object on another layer, allowing objects that would otherwise be hidden by an object on the current layer to be readily identified. The background color changes to black for easier viewing. PCB Design training module 4 - 12 Use Alpha Blending Toggle this option if your video card does not support Alpha Blending or if you suspect your Video Card Drivers are having difficulty using this graphic feature. Highlighting Options section Highlight in Full Completely highlights the selected object in the current selection color. With this option disabled, the selected object is outlined in the current selection color. Use Net Color for Highlight This option is used on power plane layers to shade the plane in the net color. Use Transparent Mode When Masking Turn this option on to enable transparent object behavior for masked objects. Show All Primitives in Highlighted Nets Enable this option to display all primitives in a highlighted net, even if layers that net objects are on are not currently enabled. Useful for a board with high layer count, requiring you to design with only a few layers enabled at a time. Apply Mask During Interactive Editing Use masking (fading of objects that are not of interest) during interactive editing. Apply Highlight During Interactive Editing Highlight, or brighten objects of interest during interactive editing. Show section The check boxes in this section perform the following when checked. Testpoints Origin Marker Status Info Displays testpoints Displays the Origin Marker Displays information about the object under the cursor in the status bar Draft Thresholds section Tracks Tracks of the width entered in the check box (or narrower) will be displayed as a single line; tracks of a greater width will be displayed as an outline (when tracks are displayed in Draft Mode). Strings The number entered in this field determines which strings are displayed as text and which are displayed as an outline box. Strings that are placed at or greater than the height entered in pixels (default 11) will be displayed as text; strings that are placed at a lesser value will be represented by an outline box. Plane Drawing section These options control the display of power planes. The first two options present the plane layers in the negative where objects on the layer represent no-copper. The Solid Net Colored option shades each region on the plane in a semi-transparent shade of the current net color. If this mode is selected and Single Layer Mode is enabled, pad and via plane connections are drawn in the positive. PCB Design training module 4 - 13 Layer Drawing Order button The PCB Editor allows you to control the order in which layers are re-drawn. Click on the Layer Drawing Order button to pop up the Layer Drawing Order dialog. The order that the layers appear in the list is the order in which they will re-draw. The layer at the top of the list is the layer that will appear on top of all other layers on the screen. 2.3.3 Board Insight Display page Figure 12 Board Insight Display page of the PCB preferences Pad and Via Display Options section Pad Nets Enable this option to show the Net name for all pads Pad Numbers Enable this option to show the pin numbers for all pads Via Nets Enable this option to show the Net name for all vias. Use Smart Display Color Enable this option for Altium Designer to control the font characteristics for the display of the pad and via details. If this option is disabled you can set the font characteristics below. PCB Design training module 4 - 14 · Font Color · Transparent Background 1. Enable this option to use the background ground color surrounding the pad/via details. Disable this option and set the Background Color. · Background Color Min/Max Font Size · The minimum font size to be used to display the Pad and Via details, regardless of the zoom level. This setting is not used if the Smart Display Color option is enabled. · The maximum font size to be used to display the Pad and Via details, regardless of the zoom level. This setting is not used if the Smart Display Color option is enabled. Font Name The font to be used to display the Pad and Via details. This setting is not used if the Smart Display Color option is enabled. Font Style The font style to be used to display the Pad and Via details. This setting is not used if the Smart Display Color option is enabled. Minimum Object Size The minimum size used to display the Pad and Via details, regardless of the zoom level. So at low levels of zoom you can still maintain visibility of the pad and via details. This setting is not used if the Smart Display Color option is enabled. Net Names on Tracks section Display Enable this option to control the display of the net name on tracks. You can choose from: · Do Not Display - the net name is not displayed on the track · Single and Centered - the net name is displayed once, in the center of the track · Repeated - the net name is displayed all along the track Single Layer Mode Options section Current Shows which Single Layer Mode option is currently in use. You can cycle through all available modes while in PCB by pressing the SHIFT+S hotkey. Available Select which Single Layer Modes to cycle through when pressing SHIFT+S in the PCB editor. · Hide Other Layers 2. Enable this option to include the Hide Other Layers as an available single layer mode option. The SHIFT+S keyboard shortcut cycles through the available layer modes. · Gray Scale Other Layers 3. Enable this option to include the Grey Scale Other Layers as an available single layer mode option. The SHIFT+S keyboard shortcut cycles through the available layer modes. · Monochrome Other Layers PCB Design training module 4 - 15 4. Enable this option to include the Monochrome Other Layers as an available single layer mode option. The SHIFT+S keyboard shortcut cycles through the available layer modes. Note: The available Single Layer Modes here are shared with and set the same for the Board Insight Lens although they maintain a separate setting for the current mode they are in. 2.3.4 Board Insight Modes page Figure 13 Board Insight Modes page of the PCB preferences Display Section Display Heads Up Information Enable this option to display context-sensitive information in your workspace. The information that is displayed can be controlled with the Browse Mode settings. Most of this information is already displayed in the status bar, however you can now raise your head up and look at this information in the same area that you are working. Use Background Color Enable this option so that the Heads Up information is displayed with its background transparent. Disable this options the Background Color setting is used. Insert Key Resets Heads Up Delta Origin Enable this option to reset the Delta Origin to the current mouse coordinates when the Insert Key is pressed. The distance horizontally and vertically the mouse is moved from the Delta Origin can PCB Design training module 4 - 16