Altium Designer Documentation

Polygon Pour

Modified by Susan Riege on May 3, 2019


The Polygon Pour dialog

Summary

This dialog allows you to specify the settings for a polygon pour. A polygon pour is a group design object that is made up of simpler primitive objects. Polygon pours are used to create either a solid or a hatched (lattice) area on a PCB layer, using either region objects, or a combination of track and arc objects. Also referred to as copper pours, polygon pours are similar to a region, except that they can fill irregularly shaped areas of a board as they automatically pour around existing objects, connecting only to objects on the same net as the polygon pour.

On a signal layer, you can place a solid polygon pour to define an area for carrying large power supply currents, or as a ground-connected area for providing electro-magnetic shielding. Hatched polygon pours are commonly used for ground purposes in analog designs.
For information on how a placed polygon pour object can be modified graphically directly in the workspace, refer to Editing Polygonal Shaped Objects.

Access

This dialog is accessed in the following ways:

  • Click the Properties button in the Polygon Pour Manager dialog (Tools » Polygon Pours » Polygon Manager).
  • Click Create New Polygon from » Selected Polygon in the Polygon Pour Manager dialog (Tools » Polygon Pours » Polygon Manager).

Graphical Tab

The Polygon Pour dialog - Graphical tab displaying the various fill modes available.

Use the Graphical tab to modify graphical properties of the polygon pour object.

Options/Controls

Fill Mode

Click to choose the fill mode for the polygon pour. There are three modes available, each with their own advantages and options:

  • Solid (Copper Regions) - region based polygons result in far fewer objects being placed, making for: smaller files; faster redraws, file opening, DRC and net connectivity analysis; and smaller output files as the region object is fully supported in Gerber and ODB++. The dialog changes to present a graphical depiction of a solid polygon pour, with the following associated options:
    • Remove Islands Less Than - specify an area value, any islands of polygon whose area is smaller than this value, will be removed.
    • Arc Approximation - specify the maximum deviation from a perfect arc (curved edges are created from multiple short, straight edges).
    • Remove Necks When Copper Width Less Than - specify a width value, the polygon pour copper whose width is smaller than this value will be removed. Typically this is set to be no smaller than the smallest width track used in the design, or the smallest copper width supported by the fabricator.
  • Hatched (Tracks/Arcs) - track/arc based polygons allow a hatched polygon to be created, by setting the Track Width to be smaller than the Grid Size. Note that they can also be solid by setting the Track Width to be larger than the Grid Size. The dialog changes to present a graphical depiction of a hatched polygon pour, with the following associated options:
    • Track Width - specify the width of track used to create the polygon.
    • Grid Size - specify the spacing, or grid that the tracks are placed on for the hatched polygon.
    • Surround Pads With - specify the shape used to surround the pads: Arcs or Octagons.
    • Hatch Mode - there are four modes available: 90 Degree, 45 Degree, Horizontal, or Vertical. When a hatch mode is selected, the polygon preview is shown in the dialog.
  • None (Outlines Only) - outlines only polygons are simply track/arc polygons without the internal tracks and arcs. The dialog changes to present a graphical depiction of an outline only polygon pour, with the following associated options:
    • Track Width - specify the track width for polygon outline.
    • Surround Pads With - specify the shapes to surround the pads: Arcs or Octagons.

Properties

  • Name - specify a suitable name for the polygon. As well as helping identify each polygon, the name can be used to target a specific polygon (or family of polygons) in a design rule by using the IsNamedPolygon('YourPolyName') query keyword.
    • Auto Naming - enable this option to have automatic polygon naming applied to the polygon. Naming is based on the chosen naming scheme specified in the Polygon Naming Scheme field in the Other region of the Properties panel. The name is based on the layer, the connected net, and a unique numerical index.
Auto-assigned names are continually monitored and managed by the software. If an attribute changes, such as the net assignment or the position of the layer in the layer stack, then the auto-assigned name is automatically updated. Affected design rules are automatically updated.
  • Layer - specify the layer on which the polygon is placed.
  • Min Prim Length - specify how short the track/arc objects in the fill mode are allowed to be. This option is not accessible in the Solid (Copper Regions) mode.
  • Lock Primitives - enable this option to lock the primitives in the polygon. When this option is enabled, the polygon is treated as a group object, which allows you to manipulate it as a single object.
  • Locked - enable this option to protect the region from being edited graphically.
If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the PCB Editor – General page of the Preferences dialog and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double-click on the locked object and disable the Locked property or disable the Protect Locked Objects option to graphically edit the object.
  • Ignore On-Line Violations - enable this option to ignore on-line violation checks for this polygon. This option can be used when making design modifications that will create a violation (and potentially slow down the PC while performing on-line DRC). Alternatively, shelve the polygon before starting the design changes, then unshelve and repour the polygon when finished.

Net Options

  • Connect to Net - assign a net to the polygon pour. The polygon will automatically connect to pad and via objects that belong to the same net in accordance with the applicable Polygon Connect Style design rule. It will pour over other kinds of objects in that net according to the chosen setting from the drop-down:
    • Don't Pour Over Same Net Objects - select this option for the polygon to pour around all other objects regardless of the net to which they belong.
    • Pour Over All Same Net Objects - select this option for the polygon to pour over all objects on the same net as the polygon (that are within the polygon's area). For example, existing routes on that net will be completely covered by the polygon.
    • Pour Over Same Net Polygons Only - select this option for the polygon to only pour over existing polygon objects on the same net as this polygon. The polygon will pour around all other objects regardless of the net to which they belong.
  • Remove Dead Copper - enable this option to remove any isolated area of polygon copper that does not connect to the specified net. Note that a polygon that is not connected to a net is considered to be Dead Copper and it will be completely removed if this option is enabled.

Outline Vertices Tab


Polygon Pour dialog - Outline Vertices tab

Use the Outline Vertices tab to modify the individual vertices of the currently selected polygon pour 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. You also can adjust the position of the polygon pour object by globally applying delta-x/delta-y values to all vertex points.

Options/Controls

  • Vertices Grid - the main region of the tab lists all of the vertex points currently defined for the polygon pour 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 - 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 and 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 to the source vertex point with the arc being from this vertex to the subsequent vertex below in the list.
Multi-cell selection and editing is also supported (within the same column) using standard Ctrl+click, Shift+click, and click&drag techniques. To edit multiple selected cells, use the Edit command. The focused cell in the selection (distinguished by a dotted cell outline) will be in "in-place" editing mode. Type the required value then press Enter (or click away). All cells in the selection will be updated to that same value.
  • Menu - click to access a menu containing the following commands:
    • Edit - right-click on a coordinate cell (X or Y) for a vertex or its associated Arc Angle cell then use this command to edit the value in that cell. Alternatively, click directly on the cell.
Multi-cell selection and editing also is supported (within the same column) using the Edit command. The focused cells in the selection (distinguished by a dotted cell outline) will then be in "in-place" editing mode. Type the required value then press Enter (or click away). All cells in the selection will be updated to that same value.
  • Add - use this command to add a new vertex point. The new vertex will be added below the currently focused vertex entry (as distinguished by a dotted outline around a cell in its row) and will initially have the same coordinates as the focused entry.
  • Remove - use this command to remove the currently selected vertex entries in the list. This command will be unavailable if there are only two vertices present for the polygon pour.
  • Copy - use this command to copy the content of the selected cells in the list to the clipboard (alternatively, use Ctrl+C).
  • Paste - use this command to paste the content of the clipboard into the list, starting at the selected cell (alternatively, use Ctrl+V).
  • Export to CSV - use this command to export all vertices to a CSV-formatted file (*.csv). The full list will be exported. There is no need to select anything prior to launching this command. Use the subsequent Export Outline Vertices dialog to determine where and under what name the file is to be saved.
  • Import from CSV - use this command to import vertices from a CSV-formatted file (*.csv). Use the Import Outline Vertices dialog to browse to and open the required CSV file. The contents of the file will completely overwrite existing vertices.
The vertices can be modified as required externally in your chosen spreadsheet editor. Once modified, import the new vertex information using this command.
  • Select All - use this command to quickly select the entire grid contents of the list.
  • Select Column - use this command to quickly select the entire column in which the currently focused cell resides.
  • Move Up - use this command to move the selected vertex upward in the list.
  • Move Down - use this command to move the selected vertex downward in the list.
  • Move By XY - use this command to move the entire polygon pour object. The Move By dialog will appear in which you can enter the increment value to be applied to each vertex point X and Y coordinates.
Using the Select Column and Select All commands in conjunction with the Copy command, you also can quickly take vertex information into an external editor then use the Paste command to bring modified information back in.
All of the above Menu commands are also available from the right-click context menu associated to the main list region.

Quickly change the units of measurement currently used in the dialog between metric (mm) and imperial (mil) using the Ctrl+Q shortcut. This affects the dialog only and does not change the actual measurement unit employed for the board as determined by the Units setting in the Other region of the Properties panel in Board mode. 

  • Add - click this button to add a new vertex point. The new vertex will be added below the currently focused vertex entry (as distinguished by a dotted outline around a cell in its row) and will initially have the same X,Y coordinates as the focused entry.
Do not be concerned if the new vertex is inadvertently added at the wrong position in the overall list of vertex points. You can use the Move Up and Move Down commands on a menu to adjust as necessary.
  • Remove - click this button to remove the currently selected vertex entry(ies) in the list. This command will be unavailable if there are only two vertices present for the polygon pour.
To remove multiple vertices, select them as required using standard multi-select features (Ctrl+clickShift+click, drag-select) then click Remove.

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

联系我们

联系原厂或当地办公室

You are reporting an issue with the following selected text
and/or image within the active document:
Altium Designer 免费试用
Altium Designer Free Trial
我们开始吧!首先,您或者您的公司已经在使用Altium Designer了吗?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

既然您在使用Altium Designer,为何仍需要试用?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,实际上您无需下载一个试用版本。

点击下方按钮下载最新版本的Altium Designer安装包

下载Altium Designer 安装包

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

填写下方表格,获取Altium Designer最新报价。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

如果您是Altium维保期内客户,您不需要下载试用版本。

如果您不是Altium维保客户,请填写下方表格免费试用。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

您为何想要试用Altium Designer?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

那您来对地方了!请填写下方表格申请试用吧。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

听上去很棒!您知道我们为学生提供了特殊折扣么?欲知详情,请点击这里。.

同时,请填写下方表格申请免费试用吧。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好棒!创作是一件超酷的事情,我们可以为您提供完美的设计软件。

Upverter是一个社区导向的交流平台,专为您这样的创客量身定做。

点击这里看看吧!

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。