コンポーネント配置とボードの配線

現在、バージョン 22. をご覧頂いています。最新情報については、バージョン コンポーネント配置とボードの配線 の 24 をご覧ください。
 

Parent page: Tutorial - A Complete Design Walkthrough with Altium Designer

Positioning the Components on the PCB

There is a saying that PCB design is 90% placement and 10% routing. While you could argue about the percentage of each, it is generally accepted that good component placement is critical for good board design. Keep in mind that you may need to also tune the placement as you route.

Component Positioning and Placement options

When you click and hold on a component to move it, if the Snap to Center option is on, then the component will be held by its reference point. The reference point is the 0,0 coordinate of the component as it was built in the library editor.

The Smart Component Snap option allows you to override this snap to center behavior and snap to the nearest component pad instead, which is handy when you need to position a specific pad in a specific location.

Enable Snap To Center to always hold the component by its reference point. Smart Component Snap is helpful when you need to align by a specific pad.
Enable Snap To Center to always hold the component by its reference point. Smart Component Snap is helpful when you need to align by a specific pad.

Positioning Components

You can now position the components in suitable locations on the board.

To move a component either:

  • Click, Hold&Drag to move the component to the required location, rotate it with the Spacebar, then release the mouse button to place it, or
  • Run the Edit » Move » Component command, then single click to pick up a component, move it to the required location, rotate it if required, then click once to place it. When you are finished, right-click to drop out of the Move Component command.
The connection lines are automatically re-optimized as you move a component. Use them to help orient and position the components to reduce the number of connection line cross-overs.

Components positioned on the board.
Components positioned on the board.

  • Selected objects can also be moved using the keyboard rather than the mouse. To do this, hold Ctrl, then each time you press an Arrow key, the selection will move 1 grid step in the direction of that arrow. Include the Shift key to move selected objects in 10x Snap Grid steps.
  • As you move a component with the mouse, you can constrain it to an axis by holding the Alt key. The component will attempt to hold the same horizontal axis (if moving horizontally) or vertical axis (if moving vertically); move it further from the axis to override this behavior or release the Alt key.
With the components positioned, it's time to do some routing!

Interactively Routing the Board

Main page: Interactive Routing

Routing is the process of laying tracks and vias on the board to connect the component pins. The PCB editor makes this job easy by providing sophisticated interactive routing tools, as well as ActiveRoute, which optimally routes selected connections with the click of a button.

In this section of the tutorial, you will manually route the entire board single-sided, with all tracks on the top layer. The Interactive Routing tools help maximize routing efficiency and flexibility in an intuitive way, including cursor guidance for track placement, single-click routing of the connection, pushing obstacles, automatically following existing connections, all in accordance with applicable design rules.

Preparing for Interactive Routing

Preferences page: PCB Editor – Interactive Routing

Before starting to route, configure the Interactive Routing options in the PCB Editor – Interactive Routing page of the Preferences dialog.

Configure the interactive routing options.
Configure the interactive routing options.

Time to Route

  • Interactive routing is launched by clicking the Route button PCB editor, Interactive Routing button, or by selecting the routing command (Route » Interactive Routing, shortcut: Ctrl+W).
  • Since the components are mostly surface mount and the design is simple, the board can be routed on the top layer. As you place tracks on the top layer of the board, use the ratsnest (connection lines) to guide you.
  • Tracks on a PCB are made from a series of straight segments. Each time there is a change of direction, a new track segment begins. Also, by default, the PCB editor constrains tracks to a vertical, horizontal, or 45° orientation, allowing you to easily produce professional results. This behavior can be customized to suit your needs, but for this tutorial, you can use the defaults.
  • When the routing reaches the target pad, the software will automatically release that connection and you will remain in Interactive Routing mode, ready to click on the next connection line.

A simple animation showing the board being routed. Many of the connections are finished using Ctrl+Click to autocomplete.

Interactive Routing Modes

The PCB editor's Interactive Routing engine supports a number of different modes, with each mode helping you deal with particular situations. Press the Shift+R shortcut to cycle through these modes as you interactively route. Note that the current mode is displayed on the Status Bar and in the Heads-Up display.

Interactive Routing modes that are not required can be disabled in the PCB Editor – Interactive Editing page of the Preferences dialog.

Routing Tips and Tricks

The PCB editor includes a range of features to help make the interactive routing process more efficient, including in-command shortcuts that you use during routing, detailed feedback via the Status Bar and the Heads Up display, and the ability to display clearance boundaries as you route.

Routing Shortcuts

Useful shortcuts during routing:

Keystroke Behavior
Shift+F1 Pop up a menu of interactive shortcuts – most settings can be changed on the fly by pressing the appropriate shortcut or selecting from the menu.
* or Ctrl+Shift+Mouse Wheel Switch to the next available signal layer. A via is automatically added in accordance with the applicable Routing Via Style design rule. Learn more about changing layers and adding a via as you route.
Tab Open the Interactive Routing mode of the Properties panel, where you can change the routing settings.
Shift+R Cycle through the enabled routing conflict resolution modes. Configure your preferred modes in the PCB Editor – Interactive Routing preferences page.
Shift+S Cycle through the available Single Layer Modes. This feature is ideal when there are many objects on multiple layers. Configure the available modes in the PCB Editor – Board Insight Display page.
Spacebar Toggle the current corner direction.
Shift+Spacebar Cycle through the various track corner modes. The styles are any angle, 45°, 45° with arc, 90°, and 90° with arc. There is an option to limit this to 45° and 90° on the PCB Editor – Interactive Routing preferences page.
Ctrl+Shift+G Cycle through the three Gloss strength (Gloss Effort (Routed)) settings. The current setting is displayed in the Heads Up display and on the Status Bar.
Ctrl+Click Auto-complete the connection being routed. Auto-complete will not succeed if there are unresolvable conflicts with obstacles.
1 Toggle the Look-ahead mode on/off.
3 Cycle through the routing width choices: Rule Minimum / Rule Preferred / Rule Maximum / User Choice. Learn more about changing the width as you route.
4 Cycle through the routing via style choices: Rule Minimum / Rule Preferred / Rule Maximum / User Choice. Learn more about changing the via style as you route.
6 Cycle through available Via Types.
Shift+E Cycle through the three object Hotspot Snap modes: off / on for current layer / on for all layers.
Ctrl Temporarily suspend object snapping feature while routing.
End Redraw the screen.
PgUp / PgDn Zoom in / out, centered around the current cursor position. Alternatively, use the standard Windows mouse wheel zoom and pan shortcuts.
Backspace Remove the last-committed track segment.
Right-Click or Esc Drop the current connection and remain in Interactive Routing mode.

Feedback During Interactive Routing

It is essential to know the name of the net or the current width setting as you route a net. This information, along with a wealth of other useful details, is available in the Heads-Up display and on the Status Bar during routing. An excellent feature to help visualize the amount of space available for routing is the ability to display clearance boundaries around all other net-objects. The image below demonstrates this; as the 12V net is being routed, all other net objects display a clearance boundary defined by the applicable Electrical Clearance Constraint (which was defined earlier in the tutorial). It is not possible to cross this boundary during routing.

  • Press Shift+H to toggle the Heads-Up display off and on. Configure the display content, color, and fonts in the PCB Editor – Board Insight Modes page of the Preferences dialog.
  • Press Ctrl+W to toggle the clearance boundaries off and on.

Routing the board with the Clearance Boundaries feature enabled, image also highlights the Status Bar and Heads Up display


Modifying and Rerouting Existing Routes

To modify an existing route, there are two approaches, either: reroute, or re-arrange.

Reroute an existing Route

  • There is no need to un-route a connection to redefine its path. You can click the Route button PCB editor, Interactive Routing button and start routing the new path.
  • The Loop Removal feature will automatically remove any redundant track segments (and vias) as soon as you close the loop and right-click to indicate you are finished (the Loop Removal feature was enabled earlier in the tutorial).
  • You can start and end the new route path at any point, swapping layers as required.
  • You can also create temporary violations by switching to Ignore Obstacle mode (as shown in the animation below), which you later resolve.

Simple animation showing the Loop Removal feature being used to modify existing routing.

Loop Removal is enabled on the PCB Editor – Interactive Routing page of the Preferences dialog. Note that there are situations where you may want to create loops, for example, power net routing. If necessary, Loop Removal can be disabled for an individual net by editing that net in the PCB panel. To access the option, set the panel to Netsmode, then double-click on the net name in the panel to open the Edit Net dialog.

During Loop Removal, you will find situations where you return to the existing routing but are not yet finished defining the new path. When the Automatically Terminate Routing option is enabled, as soon as the new route overlays the existing route, the routing process will terminate and the old, redundant routing will be removed. In this situation, it can be more efficient to disable the Automatically Terminate Routing option.

Rearrange Existing Routes

  • To interactively slide or drag track segments across the board, click, hold and drag as shown in the animation below. The default dragging behavior is configured on the PCB Editor – Interactive Routing page of the Preferences dialog as shown in the animation below.
  • The PCB editor will automatically maintain the 45/90º angles with connected segments, shortening and lengthening them as required.

Simple animation showing track dragging being used to modify existing routing.

Interactive Sliding Tips

  • Change the default select-then-drag mode using the Unselected via/track and Selected via/track options on the PCB Editor – Interactive Routing page of the Preferences dialog.
  • During dragging, the routing conflict resolution modes also apply (Ignore, Push, HugNPush). Press Shift+R to cycle through the modes as you drag a track segment.
  • Existing pads and vias will be jumped, or vias will be pushed if necessary and possible if Push mode is enabled.
  • To convert a 90º corner to a 45º route, start dragging on the corner vertex.
  • While dragging, you can move the cursor and hotspot snap it to an existing, non-moving object such as a pad (shown above). Use this to help align the new segment location with an existing object and avoid very small segments being added.
  • To break a single segment, select the segment first, then position the cursor over the center vertex to add in new segments.
  • Press Tab during sliding to access the Interactive Sliding mode of the Properties panel, where you can change any of the sliding settings.

An example of dragging multiple tracks by setting the routing conflict mode to Push.
An example of dragging multiple tracks by setting the routing conflict mode to Push.


Viewing Your Board in 3D

The PCB editor requires a graphics card that supports DirectX, refer to the System Requirements page for more details.

A powerful feature of Altium Designer is the ability to view your board as a 3-dimensional object. To switch to 3D, run the View » 3D Layout Mode command or press the 3 shortcut. The board will display as a 3-dimensional object. The tutorial board is shown below.

You can fluidly zoom the view, rotate it, and even travel inside the board using the following controls:

  • ZoomingCtrl+Right-Click, Hold&Drag, or Ctrl+Mouse Wheel, or the PgUp / PgDn keys.
  • PanningRight-Click, Hold&Drag, or the standard Windows mouse-wheel controls.
  • RotationShift+Right-Click, Hold&Drag. Note that when you press Shift a directional sphere appears at the current cursor position, as shown in the image below. Rotational movement of the model is made about the center of the sphere (position the cursor before pressing Shift to position the sphere) using the following controls. Move the mouse around to highlight the required control, then:
    • Right-Click, Hold&Drag sphere when the Center Dot is highlighted – rotate in any direction.
    • Right-Click, Hold&Drag sphere when the Horizontal Arrow is highlighted – rotate the view about the Y-axis.
    • Right-Click, Hold&Drag sphere when the Vertical Arrow is highlighted – rotate the view about the X-axis.
    • Right-Click, Hold&Drag sphere when the Circle Segment is highlighted – rotate the view about the Z-plane.

Hold Shift to display the 3D view directional sphere then click and drag the right mouse button to rotate.
Hold Shift to display the 3D view directional sphere then click and drag the right mouse button to rotate.

Tips for Working in 3D

  • Press L to open the View Configuration panel when the board is in 3D Layout Mode, where you can configure the 3D view display options (on the View Options tab in the General Settings and 3D Settings sections).
  • The 3D display colors can use Realistic, or By Layer, which are the layer colors defined in the 2D Layout Mode. There are a number of 3D Configurations defined. Explore these in the General Settings of the View Options tab of the View Configuration panel. For example, the Altium 3D Dk Green configuration is applied in the image above.
  • There are controls to configure the layer colors as well as the board thickness (vertical scaling), which is handy for examining the internal layers and interconnect structures in the PCB. 3D layers have a transparency setting; slide this to "see through" the objects on that layer.
  • You can choose to Show 3D bodies or hide them.
  • To display the components in 3D, each component needs to have a suitable 3D model included in its footprint. Refer to the Working with 3D Bodies page to learn more about including 3D models, and refer to Additional Tools for Working with 3D Bodies page to learn techniques for positioning a model on its footprint.
  • Apart from the component manufacturer's website, 3D models are also available on:
    • Community portal websites, such as 3D Content Central and GrabCAD, where designers share models.
    • A growing number of commercial 3D sites, including PCB 3D.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
注記

利用できる機能は、Altium 製品のアクセスレベルによって異なります。Altium Designer ソフトウェア サブスクリプション の様々なレベルに含まれる機能と、Altium 365 プラットフォーム で提供されるアプリケーションを通じて提供される機能を比較してください。

ソフトウェアの機能が見つからない場合は、Altium の営業担当者に連絡して 詳細を確認してください。

Content