Defining Polygons & Copper Regions for a PCB in Altium NEXUS

Created: April 21, 2022 | Updated: August 27, 2022
このドキュメント ページは、廃止された Altium NEXUS/NEXUS Client (展開された NEXUS ソリューションの一部) を参照しています。PCB 設計、データ管理、共同作業の全ての要求は、Altium Designer (Altium Designer Enterprise サブスクリプション を含む) と、接続された Altium 365 Workspace で利用できます。詳細については、FAQs のページ をご覧ください。

A common requirement on a printed circuit board is large areas of copper. It could be a hatched region of grounding copper on an analog design, a large, solid region of copper for carrying heavy power supply currents, or a solid ground area for EMC shielding.

In Altium NEXUS, areas of copper can be defined using different design objects. In simple cases, Fills and Solid Regions can be used. These are rectangular and polygon-type objects that will not pour around other objects such as pads, vias, tracks, or text. Fill and Solid Region objects are described below on this page.

In more complex cases, Polygon Pours are used. The advantage of a Polygon Pour is that it automatically pours around copper objects that belong to another net in accordance with the applicable Electrical Clearance and Polygon Connect Style Design Rules. To learn more about Polygon Pours, see the Polygons on Signal Layers page.

To provide an electrically-stable ground or power reference throughout the PCB, power planes are used. To learn more about power planes, see the Internal Power & Split Planes page.

Fills and Solid Regions

An example of a selected solid region
An example of a selected solid region

A fill (Place » Fill) is a rectangular-shaped design object that can be placed on any layer, including copper (signal) layers. Fills are limited to a rectangular shape and will not avoid other objects, such as pads, vias, tracks, regions, other fills or text. If a Fill is placed on a signal layer, it can be connected to a Net.

A placed Fill A placed Fill

A fill is a rectangular object that can be placed on any layer. When placed on a signal layer, a fill becomes an area of solid copper that can be used to provide shielding or to carry large currents. Fills of varying size can be combined to cover irregularly shaped areas and can also be combined with track or arc segments and be connected to a net.

Fills also can be placed on non-electrical layers. For example, place a Fill on the Keep-Out layer to designate a 'no-go' area for auto-routing. Place a Fill on a Power Plane, Solder Mask or Paste Mask layer to create a void on that layer. In the PCB Library Editor, fills can be used to define component footprints.

Availability

Fills are available for placement in both the PCB and PCB Library editors in the following ways:

  • PCB Editor - the following methods of access are available:
    • Choose Place » Fill from the main menus.
    • Click the Fill button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
    • Right-click in the design space then click Place » Fill from the context menu.
    • Click the  button on the Wiring toolbar.
  • PCB Library Editor - the following methods of access are available:
    • Choose Place » Fill from the main menus.
    • Click the Fill button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
    • Right-click in the design space then select Place » Fill from the context menu.
    • Click the  button on the PCB Lib Placement toolbar.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter fill placement mode. Placement is made by performing the following sequence of actions:

  1. Click or press Enter to anchor the first corner of the fill.
  2. Move the cursor to adjust the size of the fill then click or press Enter to anchor the diagonally-opposite corner and complete placement of the fill.
  3. Continue placing further fills or right-click or press Esc to exit placement mode.

A fill will 'adopt' a net name if it touches an object that has a net name.

Additional actions that can be performed during placement are:

  • Press the Tab key to pause the placement and access the Fill mode of the Properties panel from where its properties can be changed on the fly. Click the pause button overlay () to resume placement.
  • Press the L key to flip the fill to the other side of the board – note that this is only possible prior to anchoring the fill's first corner.
  • Press the + and - keys (on the numeric keypad) to cycle forward and backward through all visible layers in the design to change placement layer quickly.
  • Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement. 
While attributes can be modified during placement (Tab to access the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Graphical Editing

This method of editing allows you to select a placed fill object directly in the design space and change its size, shape or location graphically.

When a fill object is selected, the following editing handles are available:

A selected Fill A selected Fill

  • Click and drag A to resize the fill in the vertical and horizontal directions simultaneously.
  • Click and drag B to resize the fill in the vertical and horizontal directions separately.
  • Click and drag C to rotate the fill about its center point.
  • Click anywhere on the fill away from editing handles and drag to reposition it. While dragging, the fill can be rotated or mirrored:
    • Press the Spacebar to rotate the fill counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step defined on the PCB Editor – General page of the Preferences dialog.
    • Press the X or Y keys to mirror the fill along the X-axis or Y-axis.

The Fill mode of the Properties panel.
The Fill mode of the Properties panel.

Location

The icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status.
  • (X/Y)
    • X (first field) - the current X (horizontal) coordinate of the reference point of the fill, relative to the current design space origin. Edit to change the X position of the fill. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default. 
    • Y (second field) - The current Y (vertical) coordinate of the reference point of the fill, relative to the current origin. Edit to change the Y position of the fill. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default. 
  • Rotation - the fill's angle of rotation (in degrees), measured counterclockwise from zero (the 3 o'clock horizontal). Edit to change the rotation of the fill. Minimum angular resolution is 0.001°.

Properties

  • Component – this field is shown in the PCB editor only when the selected Fill is a constituent part of a PCB Component and displays the designator of the parent PCB component. Select the clickable Component link to open the Component mode of the Properties panel for the parent component.
  • Net - use to choose a net for the fill. All nets for the active board design will be listed in the drop-down list. Select No Net to specify that the fill is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed. Alternatively, you can click on the Assign Net icon () to choose an object in the design space - the net of that object will be assigned to selected fill(s).
  • Layer - the layer on which the fill is placed. Fills can be placed on any layer other than the system layers. Use the drop-down to select a different layer.
  • Area - specifies the area value of the fill object.
  • Length - displays the length.
  • Width - displays the width.

Paste Mask Expansion

  • Rule - select to have the paste mask expansion for the fill follow the defined value in the applicable Paste Mask Expansion design rule. The associated expansion value will be disabled if this option is chosen.
  • Manual - select to override the applicable design rule and specify the paste mask expansion value for the fill in the field below. 

Solder Mask Expansion

  • Rule - select the checkbox to have the solder mask expansion for the fill follow the defined value in the applicable Solder Mask Expansion design rule. The associated expansion value will be disabled if this option is chosen.
  • Manual - select the checkbox to override the applicable design rule and specify the solder mask expansion value for the fill in the field below.

A region (Place » Solid Region) is a design object that is used for defining polygonal shapes. A Solid Region (commonly called Region) can be placed on any layer including signal (copper) layers. Like a Fill, a Region does not avoid other objects, such as pads, vias, tracks, fills, other regions or text. If a region is placed on a signal layer, it can be connected to a Net.

A region object has a number of special properties that allow it to be used for:

  • Polygon cutouts - where it is essentially a negative (empty) object that the surrounding polygon pours around.
  • Board shape cutouts - where it also acts as a negative (empty) object to define an irregular cutout or hole in the board.
  • Custom pad shapes - where it defines the copper area of an unusual pad, giving the ability to define automatically matched-shape solder and paste mask contractions/expansions.

Examples of the various types of placed region objects
Examples of the various types of placed region objects

Summary

A Region, also known as a Solid Region, is a polygonal-shaped primitive object that can be placed on any layer.

A region can have any number of sides and vertices (corners). It can be placed on a signal layer to define an area of solid copper to be used to provide shielding or to carry large currents. Positive regions can be combined with tracks or arc segments and be connected to a net. In the PCB Library editor, regions can be used to create custom pad shapes on copper layers or special mask shapes on the solder and paste masks. On non-electrical layers, regions can be used to define custom shapes for tasks such as logos.

When placed as a negative, a region can create a cutout (a void) in a polygon pour. In this mode, the region will not be filled with copper when the polygon is poured. When used as a negative region for a board cutout (by placing it on the multi-layer), it defines an area that becomes a hole through the finished board. Board cutout regions are transferred to Gerber and ODB++ files for manufacturing purposes through the use of a dedicated Rout layer.

Availability

Regions are available for placement in both the PCB editor and the PCB Library editors in one of the following ways:

  • PCB Editor:
    • Choose Place » Solid Region or Polygon Pour Cutout from the main menus.
    • Click the Solid Region button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
    • Right-click in the design space then click Place » Solid Region or Polygon Pour Cutout from the context menu.
  • PCB Library Editor:
    • Choose Place » Solid Region or Polygon Pour Cutout from the main menus.
    • Click the Solid Region button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
Note that Graphic objects placed in the PCB editor and PCB Library editors will automatically be converted to Region objects.

Placement

After launching the command, the cursor will change to a crosshair and you will enter region placement mode. Placement is made by performing the following sequence of actions:

  1. Position the cursor then click to anchor the starting vertex for the region.
  2. Move the cursor ready to place the second vertex. The default behavior is to place two edges with each click, with a user-defined corner shape between them. Refer to the Placement Modes topic below for more details on changing corner modes.
  3. Continue to move the mouse and click to place further vertices.
  4. After placing the final vertex, right-click or press Esc to close and complete placement of the region. There is no need to manually close the region as the software will automatically complete the shape by connecting the start point to the final point placed.
  5. Continue placing further regions or right-click or press Esc to exit placement mode.
A region will adopt a net name if it is placed over an object that is already connected to a net.

Additional actions that can be performed during placement include:

  • Press the Tab key to pause the placement and access the Region mode of the Properties panel from where its properties can be changed on the fly. Click the design space pause button overlay () to resume placement.
  • Press the + and - keys on the numeric keypad to cycle forward and backward through all layers currently visible in the design.
  • Press the * key to cycle through the visible signal layers.
While attributes can be modified during placement (Tab to bring up associated properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Graphical Editing

Move Region Vertices

Regions contain two points, or "handles", with which to edit the shape of the region.

  • Full Handles - located at the corners of the region.
  • Empty Handles - located in the centers of the segments created by the Full Handles.

An existing region can be re-shaped by moving these handles, or vertices, located at each corner or at the center of each edge.

To modify the region shape, click and select a region, which will highlight the vertices for the region and change the cursor to a crosshair.

  • Click on a Full Handle to move that corner.
  • Click along an edge to move the entire edge.
  • Click on an Empty Handle to move the whole side (for track and for arc).
  • Ctrl+Click on an Empty Handle to break that edge into two edges. Ctrl only needs to be held at the beginning of movement. The Shift+Spacebar hotkeys can then be used to cycle through modes (arc, miter, and any angle).

The various methods of moving region vertices.The various methods of moving region vertices.

Modify Region Border

In addition to vertex editing, you also can use the Modify Region Border command to easily change the shape of polygons. The command is run by right-clicking on the desired polygon then selecting Polygon Actions » Modify Polygon Border. Once the command is launched, the cursor becomes a crosshair. Each time you click, a new vertex is added. As during region placement, the Shift+Spacebar shortcuts can be used to change corner shapes.

Modifying a region border.
Modifying a region border.

The Region mode of the Properties panel.
The Region mode of the Properties panel.

Properties

  • Component – this field is shown in the PCB editor only when the selected Region is a constituent part of a PCB Component and displays the designator of the parent PCB component. Select the clickable Component link to open the Component mode of the Properties panel for the parent component.
  • Net - use to choose a net for the region. All nets for the active board design will be listed in the drop-down list. Select No Net to specify that the region is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed. Alternatively, you can click on the Assign Net icon () to choose an object in the design space - the net of that object will be assigned to selected region(s).
  • Layer - this field is available only when Kind is set to Copper, Polygon Cutout, or Cavity. Use it to specify the layer on which the region is placed. For Copper and Polygon Cutout, all defined (and enabled) layers for the active board design are listed in the drop-down list. For Cavity, only enabled mechanical layers are listed.
  • Kind - use the drop-down to select the function of the region:
    • Copper - a solid, positive area that can be placed on any design layer, such as a signal (copper) layer.
    • Polygon Cutout - functions as a polygon cutout defining a negative or no-copper area within a polygon. Repour the polygon after placing a Cutout.
    • Board Cutout - functions as a board cutout defining a negative area or hole within the board shape.
    • Cavity - used to define an embedded cavity within which a component will reside 'inside the board'. A region of this kind only can be placed on a suitable mechanical layer and must completely enclose the 3D body of the component with sufficient clearance on each side. Check with the fabricator to find out how much clearance is required.

      Note that the Cavity Kind is only available when in the PCB Library Editor.
  • Arc Approximation - enter the maximum deviation from a perfect arc.
  • Area - displays the area of the region object.
  • (X/Y)
    • X (first field) - this field shows the current X position of the center of the pad relative to the current origin. Edit the value in the field to change the position of the pad relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space), and are used if the unit is not specified. 
    • Y (second field) - this field shows the current Y position of the center of the pad relative to the current origin. Edit the value in the field to change the position of the pad relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space), and are used if the unit is not specified. 
The  icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status. 

Outline Vertices

This region is used to modify the individual vertices of the currently selected region object. You can modify the locations of existing vertices, add new vertices or remove them as required. Arc connections between vertex points can be defined and support is also provided for exporting vertex information to and importing from a CSV-formatted file. 

  • Vertices Grid - lists all of the vertex points currently defined for the region in terms of:
    • Index - the assigned index of the vertex (non-editable).
    • X - the X (horizontal) coordinate for the vertex. Click to edit.
    • Y - the Y (vertical) coordinate for the vertex. Click to edit.
    • Arc Angle (Neg = CW) - the angle of an arc that is drawn to connect this vertex point to the next. By default, connections are straight-line edges with this field remaining blank. Click to edit then enter an arc angle as required. Entry of a positive value will result in an arc drawn counterclockwise. To draw a clockwise arc, enter a negative value.
Straight-line edges are used to connect one vertex point to the next. If you would rather have an arc connection, enter a value for the required Arc Angle. Entry is made in the field associated with the source vertex point with the arc being from this vertex to the subsequent vertex below in the list.
  • Add - click to add a new vertex point. The new vertex will be added below the currently focused vertex entry and will initially have the same X,Y coordinates as the focused entry. Click  to remove the currently selected vertex.

Paste Mask Expansion

  • Rule/Manual - select the desired paste mask expansion configuration. When Manual is selected, you can enable and enter the desired measurement.

Solder Mask Expansion

  • Rule/Manual - select the desired solder mask expansion configuration. When Manual is selected, you can enable and enter the desired measurement.
Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

お問合せ

お近くの営業所にお問合せください。

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: