Altium NEXUS Documentation

ConvertSelected

Modified by Susan Riege on Dec 18, 2018

Parent page: PCB Commands

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

  1. 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.


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

  1. 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.


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 NEXUS. 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 NEXUS 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

  1. 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.
  2. The selected tracks will still exist after the polygon pour has been created and will remain selected.


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 NEXUS 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

  1. 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.
  2. The selected tracks will still exist after the room has been created and will remain selected.


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 NEXUS. 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 NEXUS 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

  1. 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.
  2. The selected tracks will still exist after the region has been created and will remain selected.


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.

For Altium NEXUS 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 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

  1. 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.
  2. The selected tracks will still exist after the region has been created and will remain selected.


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.

For Altium NEXUS 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 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

  1. 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.
  2. The selected tracks will still exist after the region has been created and will remain selected.


Applied Parameters: Action=TO_3DBODY

Summary

This command allows you to create 3D bodies from selected tracks, arcs and solid regions.

Access

This command is accessed from the PCB Editor by choosing the Tools » Convert » Create 3D Body From selected primitives command from the main menus.

Use

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

For Altium NEXUS 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 3D Body will be created from the closed boundary formed by the primitives. The 3D Body's boundary follows the center line of the bounding track objects and it is not selected. Select and move the 3D Body to its required location in the workspace. Select the 3D Body 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

  1. The 3D Body will be created on the Top Layer, regardless of the layer on which the selected tracks are located. This means you can define the shape on a mechanical layer.
  2. The selected primitives will still exist after the region has been created and will remain selected.

 

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

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.