PCB_Cmd-ConvertSelectedConvertSelected_AD

Created: Juli 27, 2017 | Updated: Juli 13, 2018 | Applies to versions: 18.0 and 18.1

Now reading version 18.0. For the latest, read: PCB_Cmd-ConvertSelected((ConvertSelected))_AD for version 22

The following pre-packaged resources, derived from this base command, are available:

Applied Parameters: Action=PadsToVias

Summary

This command is used to change free pads into vias. A free pad is one that is not part of a parent component object. Changing free pads to vias can be useful when manually converting imported Gerber files back into PCB format.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Convert Selected Free Pads to Vias command from the main menus.

Use

First, ensure that all free pads that you wish to convert are selected in the main design workspace.

After launching the command, the free pads will be converted to vias. The properties for a via can be edited through the Properties panel.

Tips

A free pad will be converted to a via with the same hole size. The highest value found across all available XY size pairs for the pad (corresponding to the pad size on different layers) will be used for the via's diameter.

Convert Selected Vias to Free Pads

Applied Parameters: Action=ViasToPads

Summary

This command is used to change vias into free pads. A free pad is one that is not part of a parent component object. Changing vias to free pads can be useful when importing PADS-PCB and PADS 2000 files, where vias are used to connect to power and ground layers. This allows proper connection to internal power planes, using editable pads.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Convert Selected Vias to Free Pads command from the main menus.

Use

First, ensure that all vias that you wish to convert are selected in the main design workspace.

After launching the command, the vias will be converted to free pads. The properties for a pad can be edited through the Properties panel.

Tips

The vias will be converted to free pads of the same style (Simple, Top-Middle-Bottom, or Full Stack) and with the same hole size. The via's diameter size is used for the pad's XY sizing on the applicable layers. The shape of the pad will be set to Round.

Create Polygon from Selected Primitives

Applied Parameters: Action=TO_POLYGON

Summary

This command allows you to define a polygon pour object using a closed boundary made up of selected track and/or arc objects.

As well as defining areas of electrical copper on a board, polygon pours are also used to define other polygonal-shaped design objects, such as a special symbol or a company logo. If an outline of the required shape has been defined in another design tool, such as AutoCAD, it can be exported as DXF and then imported into Altium Designer. That outline can then be converted into a polygon pour using this command.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Create Polygon from Selected Primitives command from the main menus.

Use

First, ensure that all constituent track and arc primitives of the closed boundary are selected in the main design workspace.

For Altium Designer to be able to perform a track to polygon conversion, the outline must be correctly defined. That means the outline must form a closed shape, with the ends of touching track segments correctly meeting (starting/ending in the same X, Y location).

After launching the command, a polygon pour will be created from the closed boundary formed by the track primitives. The polygon pour is drawn in outline only mode and is not selected. Select and move the polygon to its required location in the workspace. Select the polygon to access its properties through the Properties panel (double-click on it if the panel is not visible), from where you can change its fill mode (to solid or hatched) and other associated properties, as required.

Tips

The polygon pour will be created on the current (or active) layer, not the layer that the selected tracks are on. This means you can define the shape on a mechanical Layer, then create the polygon pour on a signal layer.
The selected tracks will still exist after the polygon pour has been created and will remain selected.

Create Room from Selected Primitives

Applied Parameters: Action=TO_ROOM

Summary

This command allows you to define a room object using a closed boundary made up of selected track and/or arc objects. A room is a primitive design object. It is a region that assists in the placement of components.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Create Room from Selected Primitives command from the main menus.

Use

First, ensure that all constituent track and arc primitives of the closed boundary are selected in the main design workspace.

For Altium Designer to be a able to perform a track to room conversion, the outline must be correctly defined. That means the outline must form a closed shape, with the ends of touching track segments correctly meeting (starting/ending in the same X, Y location).

After launching the command, the Edit Room Definition dialog will open. Use this dialog to define the room's associated Room Definition design rule, including which components (or class of components) are targeted by (associated with) the room and related constraints. After clicking OK, a room will be created from the closed boundary formed by the track primitives. The room's boundary follows the center line of the bounding track objects and it is not selected. Select and move the room to its required location in the workspace. Double-click on it to access the Edit Room Definition dialog, from where you can further change scope and/or constraints for the associated room definition rule as required.

Tips

The room will be created on the layer specified in the associated rule's constraints, not the layer that the selected tracks are on. This means you can define the shape on a mechanical Layer, then create the room on the required signal layer.
The selected tracks will still exist after the room has been created and will remain selected.

Create Region from Selected Primitives

Applied Parameters: Action=TO_REGION

Summary

This command allows you to define a solid (copper) region object using a closed boundary made up of selected track and/or arc objects. This is a region object that has its Kind property set to Copper.

As well as defining areas of electrical copper on a board, solid regions are also used to define other polygonal-shaped design objects, such as a special symbol or a company logo. If an outline of the required shape has been defined in another design tool, such as AutoCAD, it can be exported as DXF and then imported into Altium Designer. That outline can then be converted into a solid region using this command.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Create Region from Selected Primitives command, from the main menus.

Use

First, ensure that all constituent track and arc primitives of the closed boundary are selected in the main design workspace.

For Altium Designer to be a able to perform a track to region conversion, the outline must be correctly defined. That means the outline must form a closed shape, with the ends of touching track segments correctly meeting (starting/ending in the same X, Y location).

After launching the command, a solid region will be created from the closed boundary formed by the track primitives. The region's boundary follows the center line of the bounding track objects and it is not selected. Select and move the region to its required location in the workspace. Select the region to access its properties through the Properties panel (double-click on it if the panel is not visible), from where you can change its properties as required.

Tips

The region will be created on the current (or active) layer, not the layer that the selected tracks are on. This means you can define the shape on a mechanical Layer then create the region on a signal layer.
The selected tracks will still exist after the region has been created and will remain selected.

Create Cutout from Selected Primitives

Applied Parameters: Action=TO_CUTOUT

Summary

This command allows you to define a polygon pour cutout region object using a closed boundary made up of selected track and/or arc objects. This is a region object that has its Kind property set to Polygon Cutout.

A polygon pour cutout region represents a void area in any polygon pour object (on the same layer) that it overlaps.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Create Cutout from Selected Primitives command from the main menus.

Use

First, ensure that all constituent track and arc primitives of the closed boundary are selected in the main design workspace.

After launching the command, a polygon cutout region will be created from the closed boundary formed by the track primitives. The region's boundary follows the center line of the bounding track objects and it is not selected. Select and move the region to its required location in the workspace. Select the region to access its properties through the Properties panel (double-click on it if the panel is not visible), from where you can change its properties as required.

Tips

The region will be created on the current (or active) layer, not the layer that the selected tracks are on. This means you can define the shape on a mechanical Layer then create the region on a signal layer.
The selected tracks will still exist after the region has been created and will remain selected.

Create Board Cutout from Selected Primitives

Applied Parameters: Action=TO_BOARDCUTOUT

Summary

This command allows you to define a board cutout region object using a closed boundary made up of selected track and/or arc objects. This is a region object that has its Kind property set to Board Cutout.

A board cutout region defines an area that becomes a hole through the finished board. Board cutout regions are transferred to Gerber and ODB++ files for manufacturing purposes.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Create Board Cutout from Selected Primitives command from the main menus.

Use

First, ensure that all constituent track and arc primitives of the closed boundary are selected in the main design workspace.

After launching the command, a board cutout region will be created from the closed boundary formed by the track primitives. The region's boundary follows the center line of the bounding track objects and it is not selected. Select and move the region to its required location in the workspace. Select the region to access its properties through the Properties panel (double-click on it if the panel is not visible), from where you can change its properties as required.

Tips

The region will be created on the Multi-Layer, regardless of the layer that the selected tracks are on. This means you can define the shape on a mechanical Layer.
The selected tracks will still exist after the region has been created and will remain selected.

Druckversion

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

PCB_Cmd-ConvertSelectedConvertSelected_AD

Summary

Access

Use

Tips

Summary

Access

Use

Tips

Summary

Access

Use

Tips

Summary

Access

Use

Tips

Summary

Access

Use

Tips

Summary

Access

Use

Tips

Summary

Access

Use

Tips

Was this page helpful?