Improvements in Beta

This page includes detailed information for features and functionality that are currently available to Beta users.

Altium Agile and Altium Designer users: When you update your Altium Designer Agile or Altium Designer installation to a newer version and you use a Standalone or Private Server license, you may need to reactivate/refresh the license to be able to access and use new features and functionality. For more information, refer to the following pages:

 
 

Version 26.12

Altium Designer Develop – Released: 10 November 2026 – Version 26.12.1 (build 7) Beta 2
Altium Designer Develop – Released: 30 October 2026 – Version 26.12.0 (build 6)

Altium Designer Agile – Released: 10 November 2026 – Version 26.12.1 (build 40) Beta 2
Altium Designer Agile – Released: 30 October 2026 – Version 26.12.0 (build 29)

Altium Designer – Released: 10 November 2026 – Version 26.12.1 (build 8) Beta 2
Altium Designer – Released: 30 October 2026 – Version 26.12.0 (build 7)

Beta Release Notes for Altium Designer

Harness Design Improvement

Updated Default Pin Length

The default value of the Pin Length for a pin has been increased from 0.5mm to 7.5mm in the Harness Design - Defaults Preferences page.

For more information about preferences for a harness design, refer to the Harness Design Preferences page.

Platform Improvement

Switching to .NET 10

With this release, Altium Designer switches from using .NET 8 to .NET 10. This is bundled as a part of Altium Designer. This change enables Altium Designer to take advantage of later functionality and developments with .NET, including general performance enhancements. This is especially relevant as part of preparation for the future release of Altium Designer 27.0.

Any Third Party extensions that were found to be incompatible with .NET 10 have been removed from the software, starting with this release. If later, updated versions of these extensions are made to be compatible with Altium Designer/Altium Designer Develop/Altium Designer Agile 26.12 (or beyond), contact beta.program@altium.com to get them reviewed and added back to the installation.

Data Management Improvement

New Fields When Creating a Jira Issue

When creating a Jira issue through a placed comment in the design space, additional fields are now available for specifying Components, Fix versions, and Labels.

For more information about working with Jira tasks, refer to the Document Commenting page.

Features Made Fully Public in Altium Designer 26.12

The following features are now officially Public with this release:

Features in Closed Beta

  • To access beta features you must have the Beta User Program extension installed. If it is not currently installed, you can install it from the Available tab of the Extensions and Updates page.

  • The information about each beta feature remains on this page until the feature becomes open beta/public at which time its description is moved to the New in Altium Designer page.

 
 

Existing Closed Beta Features Improved in Altium Designer 26.12

The following existing Closed Beta features have been improved further in this release:

Tabbed Routing

This feature is available when the PCB.TabbedRouting option is enabled in the Advanced Settings dialog.

The concept of Tabbed Routing to the PCB editor has been introduced. Tabs are used to achieve required trace impedance in areas where width is restricted, for example, in dense BGA pin fields. Tabbed routing is a critical feature required to support DDR5 interfaces.

The functionality provides the ability to generate tabs, with given parameters, on selected arc traces, and the ability to choose tab positioning and, if required, force tab application.

Once the required arc traces are selected, choose the Tools » Tabbed Routing command from the main menus. Configure tab geometry and tab positioning in the Properties panel that opens.

  • Choose which of the four parameters of the tab geometry to calculate (Height, Top Width, Bottom Width, or Area) based on values entered manually for the other three.

    When the defined tab shape is applied to an arc segment, the tab will follow the arc’s geometry – the Top Width, Height and Area are preserved, while the Bottom Width may vary.

  • Two modes of tab positioning are available: Arc Midpoint (generates tabs on the midpoints of each arc) and Angle Grid (generates tabs on the intersections of the arc and radial lines from the arc center; the angles of these lines are defined by the Angle Step (α) and Angle Offset (β) parameters).

    The Angle Grid mode is particularly useful for positioning the tabs evenly in relation to a via array defined by a BGA footprint.

You can also use additional options:

  • Force tabs – force placement of tabs (i.e., place tabs that will violate applicable design rules).

  • Show preview on PCB – enabled tab preview in the design space.

Once the parameters are configured as required, click the  button at the top of the panel to generate tabs. A dialog will present the results of how many tabs were generated or omitted (in adherence to defined design rules).

In this example, tabs will be added to outer arcs of three diff pairs. Arcs in the area where tabbed routing should be applied have been selected. 

The PCB Filter panel was used to filter out unnecessary arcs and select only the arcs to which tabs should be added.

Select the Tools » Tabbed Routing command from the main menus.

Configure tab geometry, tab positioning, and other options in the Properties panel that opens.

Once the properties are configured, click the  button to generate tabs on the selected arcs.

 
  • You can use the PCB Filter panel to select arcs of a specific radius. For example, if you would like to select arcs with a radius larger than 0.5 mm, use the IsArc And (AsMM(ArcRadius) > 0.5) query.

  • You can select and deselect arcs when configuring tabbed routing. After running the Tabbed Routing command, click an arc that is currently not selected to select it or click an arc that is currently selected to deselect it (clicking anything else will not change the select/deselect state of objects) –  .

If no tabs were generated due to DRC violations, you can either interrogate and modify applicable design rules or use the Force tabs option available in the Properties panel. 

In the current implementation, if you try to generate tabs on arcs that already have tabs, new tabs are generated over the top of existing ones. Also, generating tabs on straight traces is not supported.

For more information, refer to the Adding Tabs to Routing page.

Diff Pair Auto-shrinking

This feature is available when the PCB.Routing.EnableDiffPairAutoShrinking option is enabled in the Advanced Settings dialog. Note that the PCB.Routing.EnableAutoShrinking option must also be enabled, which adds an Auto Shrinking option to the PCB Editor – Interactive Routing page of the Preferences dialog. The setting of the option in Preferences will be reflected in the option on the Properties panel and vice versa.

Note: The PCB.Routing.EnableDiffPairAutoShrinking advanced settings option simply controls the visibility of the option relating to this feature on the Properties panel when interactively routing differential pairs. If only the PCB.Routing.EnableAutoShrinking option is enabled, the Interactive Differential Pair Router will not auto-shrink, regardless of the setting for the Auto Shrinking option in Preferences.

The auto-shrinking functionality is now available when routing differential pairs using the Interactive Differential Pair Router (Route » Interactive Differential Pair Routing), allowing diff pairs to be narrowed to the applicable width/gap in tight places as you route.

In cases when a differential pair being routed using the interactive router cannot be routed between obstacles with the currently chosen routing width and gap, this new feature allows to automatically shrink the width and/or gap to a value that would allow routing (provided that this shrunk diff pair would not violate the minimum allowed width/gap from the corresponding constraint). Enable the Auto Shrinking option in the Interactive Routing Options region of the Properties panel when interactively routing a differential pair to enable the feature.

Note that auto-shrinking is not applied in Ignore Obstacles and Stop At First Obstacle routing conflict resolution modes. Learn more about Available Routing Conflict Resolution Modes.

For more information, refer to the Differential Pair Routing page.

Dynamic Symbols

This feature is available when the HarnessDesign.DynamicSymbol option is enabled in the Advanced Settings dialog.

The concept of Dynamic Symbols has been introduced for use with harness design, facilitating the ability to have a ‘placeholder component’ within your wiring diagram(s), an entity that has no predefined link to a standard component in your connected Workspace Library (no defined Design Item ID) and, importantly, no pins defined. This allows you to conveniently work with bulkhead connectors involving a large pin count, breaking the connector into multiple parts on the same diagram or over multiple wiring diagrams – complete with break symbols – and ordering the pins across those parts as you need, on the fly.

A dynamic symbol is available in two ways:

  • By placing a truly ‘generic component’ into a harness wiring diagram, using a new Generic Component control, available from the main Place menu, the Active Bar, and from the bottom of the Components panel (when its filter is set to All).

  • By placing a standard component directly into a harness wiring diagram from the Manufacturer Part Search panel or Components panel, using a new Place with Dynamic Symbol menu command.

     

The notion of truly ‘generic component’ for use with harness design should not be confused with the predefined generic components (based on component templates) that are available for placement in a PCB design and located as tiles above in the Components panel.

A generic component appears with a red-colored symbol, signifying that it is using a ‘dynamic symbol’ at this point and is not referencing an actual component in your Workspace Library. Once a graphic (a rectangle) of a generic component is placed, pins can be added to the symbol, with smart auto-suggestion to quickly populate sides of the symbol. Alternatively, pins can be added to the symbol at any point after graphic placement using the Place Pins command from the Part Actions right-click context menu of the symbol.

Pins can also be added directly to the symbol while placing wires. When in wire placement mode (Place » Harness Wire), move the cursor close to the generic component's graphic. When a 'phantom' pin appears, click its hotspot to place the pin and attach a wire to it.

When ready, a component with a dynamic symbol (generic or placed from the Manufacturer Part Search panel) can be saved to your connected Workspace as a standard Workspace Library component. A control becomes available in the design space, next to the component when it is selected, with which to do so.

  • For a generic component, the control to save to the Workspace becomes available once the generic component has been given a value for its Comment.

  • For a component placed from the Manufacturer Part Search panel, the  button is also available in the Properties panel when the component is selected.

Once a Comment is added to a generic component, use the control that appears to save the component to your connected Workspace.

Save a component with a dynamic symbol placed from the Manufacturer Part Search panel using the control in the design space or the button in the Properties panel.

 

You can turn a generic component into a standard component by choosing that component in the Workspace Library (choosing its Design Item ID). You will have the option of using the library component’s standard symbol, or to keep using the dynamic symbol – useful for when you still do not want to fully lock down the symbol at that stage. In the case of the latter, the symbol turns from red to blue, signifying that a dynamic symbol is still in-play, but for a real, associated Workspace Library component.

Replace a generic component with a standard one by clicking the control at the right of the Design Item ID field in the Properties panel when the component is selected.

Search for and select the required component in the Select Component dialog that opens. 

You can choose between using the selected component's linked symbol or keeping the dynamic symbol.

If you keep the dynamic symbol, it will be shown blue in the design space.

 

With a connector selected, configuration of the pins, their order and splitting pins across new parts, can be performed from the Pins tab in the Properties panel. Use 'drag and drop' controls on the left-hand side of a selected pin's entry () to rearrange pins within the same part, across parts, and to move unplaced pins into a part.

Where a connector has been split into two or more parts (using the Split Symbol command from the Part Actions right-click context menu of the symbol), a break symbol can be presented in the design space by ensuring a new option to do so – Show Breaks for Split Symbols – is enabled on the Harness Design – General page of the Preferences dialog.

Various useful commands are also available on the right-click context menu, for placing additional pins and splitting/merging parts.

While on the logical side, a connector can be split up for better readability within one or more wiring diagrams, once the data is pushed through to the layout drawing, the connector is a single entity again.

For more information, refer to the Working with Dynamic Symbols page.

Connection Table in Layout Drawing

This feature is available when the Harness.ConnectionTable option is enabled in the Advanced Settings dialog.

Connection tables are now available for placement in a harness design layout drawing document (*.LdrDoc). A connection table is an automatically generated table that shows the wires connected to every connection point in the harness. The table gives you immediate pin-level visibility by showing the connections between connectors and wires inside the layout. It also gives you the ability to easily trace wires from connectors rather than needing to inspect the bundle and unravel which wires go to the connector. Design reviewers can use the connection table to cross-check routing, pin assignments and component relationships rather than switching between multiple documents, allowing them to make immediate changes.

To place a connection table, click the Add Connection Table control in the Connector Terminations section of the Model region in the Properties panel when a component is selected in a harness layout drawing. The Connector Terminations region displays the name of the table (which can be edited in the panel), and the table appears in the design space with a list of the cavities and associated parts displayed below the table. When the table is selected in the design space, you can use the Cavity Parts Summary and Associated Parts Summary regions of the Properties panel to configure the displayed list (font, etc.,), including disabling the display.  

The table can be deleted by clicking the Delete Table control in the Properties panel when a component is selected in the design space. The table is immediately deleted.

With a component selected, click Add Connection Table to place a table.

The table is placed in the design space, with the list of cavities and associated parts below it. 

Use the controls to configure the font, etc., of the displayed list; disable Display Summary to remove the list.

 

As part of this functionality, a new Wiring tab has been added to the Properties panel when a harness connector is selected in the design space of the layout drawing document. The tab displays the wiring list for the selected harness component.

For more information about the new connection table, refer to the Creating the Harness Layout Drawing page.

Advanced Via Fencing

This feature is available when the PCB.AdvancedViaFencing option is enabled in the Advanced Settings dialog. Note that the PCB.Performance.InteractivePropertyPanel.Optimization option must also be enabled.

This release delivers advanced support when using via fencing (adding shielding and stitching vias) in a PCB design and is especially relevant to RF and High-Speed designs which, due to their inherent complexity, require a stronger, more accommodating and robust, via fencing tool.

The commands to add stitching (Via Stitching) and shielding (Via Shielding) to a net are available from the PCB editor’s Tools » Via Stitching/Shielding menu, as before, with a keyboard shortcut sequence now added for shielding (T, H, S), complementing that already available for stitching (T, H, A). In addition, dedicated commands for removing stitching/shielding are no longer provided, because you can now simply select a stitching/shielding union and use the Delete shortcut.

Enhanced shielding and stitching support is delivered through the Properties panel, which presents controls for Via Fencing in ’Shielding’ or ‘Stitching’ modes, depending on the selected existing fencing entity in the PCB design space (or chosen entity if adding new fencing for the first time).

 

The panel provides all the controls needed to configure fencing exactly as you need it:

  • Apply different shielding via patterns to the same net on different layers. This caters for the common case of adding different via patterns on traces on layers between signal transition vias.

  • Place stacked vias into the shielding.

  • Shield with staggered vias using a new, configurable ‘via offset’.

  • Fence by geometry edge (polygonal-shaped objects or the board outline) in a selected area. Expanding on the previous ability to follow the ‘outer’ side of the selected geometry, you can now set up to follow the 'inner' side as well. This enables you to surround different RF-sensitive areas, such as Faraday cage, Coplanar Waveguides, RF walls perimeter (to limit the fringing fields along the board outline), etc.

  • Fencing obeys Clearance, Short Circuit, Hole to Hole, and Board Outline Clearance design rules.

  • With respect to shielding, advanced via fencing calculates the Via Pitch from via centers, rather than via annular rings, unifying it with the current stitching via approach. You also have the added ability to configure a pattern for ‘equalized’ (maintain equal via pitch between staggered rows, where possible) or ‘optimal’ (automatically adjust pitch to distribute vias more evenly, where possible) pitching. In the latter case, this calculates a distance between vias that follows the shielding contour, rather than shortest distance (as was the case before).

The Properties panel also guides you through the various states that can be encountered, with relevant messaging and action controls for:

  • Generating an initial via shielding/stitching pattern. If there is existing shielding for a net, you will have the choice to add the newly defined shielding or replace the existing shielding completely.

  • Pending changes, where modifications to an existing shielding/stitching pattern have been made in the panel and have yet to be applied to the design itself.

  • Board changes, where objects/geometry within the design have changed and the associated shielding/stitching has become ‘out of date’.

You also have the convenience of seeing a preview of the shielding/stitching pattern, prior to its generation, though be aware that the final pattern generated in the design may change slightly to accommodate DRC.

 

Whether generating a new shielding/stitching pattern or updating an existing one, a dialog will present the results of how many shielding/stitching vias were generated or omitted (in adherence to defined design rules). If no vias were generated, you can either interrogate and modify applicable rules or use a Force vias control, available in the Properties panel (which places vias that will violate those design rules).

  • When applying a via shielding pattern in Inner mode to polygon pours, shielding vias are placed only near a polygon's outline or edge of the board ().

  • When applying a via shielding pattern to hatched polygon pours, a stitching via will automatically be placed if its center is located on copper within the polygon ().

  • When applying a via shielding pattern, it is possible to have overlapping annular rings for the shielding vias. Set the Via Pitch value less than the via Diameter but greater than the via Hole Size ().

  • When applying a via shielding pattern, the last via in the shielding contour will be removed if it would otherwise violate the Via Pitch constraint.

  • When applying a via shielding pattern, the Optimize Pitch option will only automatically reduce the Via Pitch as far as the minimum pitch allowed by the applicable Hole To Hole Clearance rule. If the current shielding configuration is such that further pitch reduction would actually result in a rule violation, then the existing Via Pitch value is preserved, instead of being automatically decreased.

  • When applying via stitching, you have an option to enable/disable adding of stitching vias that will 'punch through' other-net polygon pours on other layers, provided those polygons are unlocked. The option – Stitch through other-net polygons – is located in the Advanced collapsible region of Stitching Parameters in the Properties panel.

    In the example shown here, polygon pours of net GND are placed on outer layers of the PCB while a polygon pour of net 3V3 (gold) is placed on an inner layer. 

    When via stitching is applied to the GND net and the Stitch through other-net polygons option is disabled, stitching vias are not placed in the area where the 3V3 net polygon pour overlaps GND polygon pours.

    When via stitching is applied to the GND net and the Stitch through other-net polygons option is enabled, stitching vias are placed in the area where the 3V3 net polygon pour overlaps GND polygon pours, punching through the 3V3 polygon pour.

     
  • You will be prevented from applying shielding/stitching parameters that are not valid for the applicable objects/geometry within the design.

  • The advanced via fencing feature and properties are observed by the PCB List panel, PCB panel (in its Unions mode) and the PCB CoDesign feature.

  • The following compatibility report entry has also been added when opening a project in a previous version of the software:

    “CAUTION: This document contains enhanced via shielding/stitching functionality supporting optimized via placement for more uniform spacing, shielding along region edges, repeated shielding of the same nets, with via stacks, and improved adherence to settings and design rules. These will be lost when opening the document and regenerating shielding/stitching in a version of Altium Designer that does not support this functionality.”

For more information, refer to the Adding Via Stitching & Via Shielding page.

Modern Comment Markers

This feature is available when the Comments.ModernMarkers option is enabled in the Advanced Settings dialog.

In this release, a new design has been introduced for comment markers placed in the design space. The new markers are available wherever comments are supported. This feature also includes new coloring when placing comments in an ActiveBOM document.

 

For more information about the commenting functionality, refer to the Document Commenting page.

Advanced Diff Pair Retrace

This feature is available when the PCB.Routing.AdvancedDPRetrace option is enabled in the Advanced Settings dialog.

This release adds enhanced support for retracing a selected differential pair when the Hugging Style is set to Rounded mode in the Gloss And Retrace panel. The Set Diff Pair Gap field is now provided in the Retrace Parameters region of the panel that allows you to select one of the rule-based gap options (Min / Max / Preferred) of an applicable Differential Pairs Routing design constraint when the Retrace Selected command is run, or retrace using the Current gap between the differential pair tracks. Alternatively, enter a desired custom gap value directly in the field.

For more information, refer to the Interactive Routing page.

Harness Library Components

This feature is available when the EDMS.HarnessEntityModel option is enabled in the Advanced Settings dialog.

This release brings support for a range of harness-related component types that can be defined as part of your Workspace Library. At the heart of this support is a new model type that can be created and defined – the Harness Entity. When creating a new component, choosing the Harness Entity model type will take you through to creating one of the following supported models:

  • Harness Connector – a physical, pluggable termination point for bundled wires, providing interconnection to/between electronics modules/circuits in an overall harness loom. Configure its gender, crimp gender and sealing type and whether it has built-in crimping. A ‘cavity view’ of the connector can also be defined (see below).

  • Crimp – a metal terminal where the contact barrel is compressed around the stripped electrical wire. Configure its gender and finish, along with associated, industry-standard parameters.

  • Seal – an environmental barrier around a crimped wire to prevent moisture, dust and debris from entering a connector cavity. Configure the min/max outer diameter (OD). A seal can have an associated plug (a cavity plug or dummy plug), which is used to seal an unused/empty cavity in a sealed connector. So when a sealed connector has a cavity where no wire/crimp is inserted, a plug fills that cavity to ensure the environmental sealing integrity of the whole connector is maintained.

  • Accessory – a physical component used in the routing and organization of harnesses, such as a peg, band, corner post or tie-wrap.

  • Splice – a crimped and insulated mechanical joint used to extend, fork or connect circuits in a harness loom. Configure its type: Butt, Parallel, Reducer, Tap or IDC, along with associated, industry-standard parameters. Note that this is only for mechanical splices.

  • Covering – a length of protective sleeving over a harness bundle to physically protect the bundle against heat and abrasion, for example. Configure its type: Tubing (Standard, Slit or Shrinkable), Corrugated Tubing (Standard or Slit), Spiral Wrap, Tape or Braiding, along with coloring and associated, industry-standard parameters. Note that defining a harness covering is currently supported at the Workspace Library level only.

For all but the Covering entity type, you upload a 3D model, which is used as the basis for defining a range of physical model views (projections) for use when placed in the layout drawing. For each defined view, you can configure whether it is solid or wireframe, its projection side, zoom level, and rotation, and whether it is added as default when importing data from a wiring diagram into the layout drawing.

In this example, a Harness Connector harness entity type is being defined. On the General tab, upload a 3D model of the connector and define the connector's parameters.

On the Views tab, define physical model views based on the uploaded 3D model.

 

In addition, for a Harness Connector model entity, you can use the uploaded 3D model as a backdrop in the definition of a Cavity Model, which is essentially a graphical view of the connector – a Cavity View, if you will – with its numbered cavities and associated crimps and seals. The model is defined through a new Cavity Model (or Cavity View) editor, with the Properties panel reflecting options and controls at both the model level (with no cavity selected) and the selected cavity level.

On the Cavity Model tab, you can manage the connector's cavity model and view its details.

When editing the cavity model, define properties of individual cavities using the Properties panel.

 

Various new component rule checks have been added with respect to saving a new harness component involving a defined connector model and its cavity model/view, which you can find on the Data Management - Component Rule Checks page of the Preferences, under the new section Violations Associated with Harness Entities.

An additional Workspace item type is also available – the Harness Entity Template – allowing for a more streamlined reuse of a defined harness entity model. A harness entity model or template can be referenced through a component template (using the new HarnessEntity parameter). This allows you to quickly create harness components based on specific component (and harness) templates.

Select a Harness Entity saved in your Workspace as the Default Value of the HarnessEntity parameter in a component template.

Alternatively, select a Harness Entity Template as parameter's Model Template.

 

A range of predefined harness entity templates can be deployed to your connected Workspace from the Library - Components page of its browser-based interface (learn more). As part of this, a range of predefined component templates are also added referencing these, which will appear on the Data Management - Component Types page of the Preferences (and also in the listing of available types when creating a new component). Take them for a spin and modify them as necessary as you explore the area of harness components.

When browsing harness components in your Workspace Library through the Components panel, a preview of the related harness entity model is provided ().

The Harness Library Components feature is available for a connected Workspace on the Altium Platform and supported by the Altium On-Prem Enterprise Server starting from version 8.1.4.

For more information, refer to the Creating a Harness Component page.

Related Components

This feature is available when the EDMS.RelatedComponents option is enabled in the Advanced Settings dialog.

This release brings support for specifying components at the Workspace Library level that are related to a defined PCB or Harness component. A new section is presented – Related Components – with which to do so when defining a component through the Component editor (in Single Component Editing and Batch Component Editing modes).

Add one or more of the following entries as required:

  • Alternate – a replacement component that can be used in place of this defined component (driven by the BOM).

  • Mating Half – this entry is in place for future use when defining two halves of an inline harness connector defined on a multi-board schematic.

  • Associated Component – a component associated with the component being defined. When defining a PCB component for example, this could be a nut, screw, spacer, etc. When defining a Harness component, this could be a backshell, wedgelock, etc. You also have the ability to specify quantity/length and inclusion into the BOM as either Optional or Mandatory.

When browsing components in your Workspace Library through the Components panel, a new section for Related Components is provided.

The Related Components feature is only available for a connected Workspace on the Altium Platform. It is currently not supported by the Altium On-Prem Enterprise Server.

For more information, refer to the Single Component Editing and Batch Component Editing pages.

Design Reviews

This feature is available when the EDMS.DesignReviewsCreation option is enabled in the Advanced Settings dialog.

This feature adds the ability to create a design review from within Altium Designer. To create a design review, select Create Design Review in Web from the Project menu or the right-click menu of a project entry in the Projects panel. When the option is clicked, the interface opens in which you can access the Design Reviews page for the project in the Workspace's browser-based interface. The Create Design Review window opens in which you can define reviewers, description and which checklist template is to be used.

Once created, in Altium Designer your active design reviews – for which you are a defined reviewer – will be accessible from a new Design Review page within the project’s Share dialog. You can also initiate design review creation from here.

In addition, if a design review process (with workflow) has been defined and made active through the Workspace, it will become available to you under Altium Designer’s Project » Project Activities sub-menu. If such a process-based workflow is available, you will not be able to initiate design review creation from the Share dialog.

For more information about design reviews, refer to the Sharing a Design page.

Selectable Harness Source within Multi-board Design

This feature is available when the MBS.HarnessSource option is enabled in the Advanced Settings dialog.

This feature gives you the ability to select the harness design project to be used as the source for a harness connection in a multi-board design, bringing logical connectivity to the latter. With a harness connection selected on a multi-board schematic, you can now choose the required project from the Harness Project drop-down in the Source region of the Properties panel.

Additionally, you can use the same source harness project for multiple harness connections in the multi-board design. In other words, you can freely define one or more instances of the same harness in your multi-board design. Note that this is analogous to multi-channel in a PCB design, but this is multi-harness in a multi-board design! You no longer need to create a separate harness project per connection with all BOM-related information efficiently taken from one wiring diagram in a single harness design source.

Also, support for the seamless bidirectional synchronization of information between the multi-board schematic and the harness wiring diagram allows the two domains to be worked on independently. Changes can be propagated from one domain to the other through a generated ECO using the Design » Import from Child Projects and Design » Update Child Projects commands in the multi-board schematic and the Design » Import Changes From <Multi-board Project> command in the harness wiring diagram.

When first synchronizing (i.e., importing data from the harness source to multi-board schematic or vice versa), you will be prompted to match components on the two sides to create the ‘Component Links’ through which synchronization can be performed. You can choose to do this automatically or manually, the latter performed using the Edit Component Links Between Harness Project and MultiBoard Document dialog.

Once links have been created, the initial ECO will be generated.

For more information, refer to the Working with Connections page.

Interactive Dynamic Phase Tuning

This feature is available when the PCB.TraceTuning.InteractivePhaseTuning option is enabled in the Advanced Settings dialog.

This release adds dynamic phase matching support when manually length tuning a net within a differential pair using the Interactive Length Tuning tool. This facilitates maximum efficiency of differential signal transmission by enabling you to manually equalize the length of the two sides in a differential pair, while also matching the phase along the entire length of the pair.

When interactively building the tuning pattern (Tools » Interactive Length Tuning used on a net of a diff pair), the applicable Matched Lengths rule (with the Within Differential Pair Length option enabled and Dynamic Phase Matching enabled and configured) will be listed in the Target region of the Properties panel (Source – From Rules). Whether the pattern is generated or not depends on the position along the track, with the Clip to Target option also observed if enabled (clipping the length to be slightly below the target but within the rule’s defined Dynamic Phase Tolerance), as well as the Length Gauge functioning as expected.

In this example, a Matched Length rule is configured to constraint dynamic phase matching within differential pair BMDI3. 

A violation of the Matched Length rule is flagged and highlighted in the design space.

When interactively tuning a net within the diff pair, the Matched Length rule is considered as a source when the From Rules option is selected.

Using the Interactive Length Tuning tool and the Matched Length rule as the source, you can tune the diff pair net to maintain the phase along the length of the pair.

 

For more information, refer to the Length Tuning page.

Improved Return Path Via Detection

This feature is available when the PCB.Rules.ReturnPathViaDetection option is enabled in the Advanced Settings dialog.

This release adds improved detection of return path vias during design rule checking of a Return Path rule. Stacked and staggered microvias are now considered for use as return path vias.

For a high-speed signal, such vias may be considered for a return path if they connect reference layers for that signal, flowing between layers (if there is only one reference layer for the high speed signal there is nothing to stitch and no return path via is needed), and if the distance between the return path vias, and return path vias and the signal, is not more than the Max Stitch Via Distance defined in the rule.

In the example shown below, a stacked microvia is used as a stitch via that connects polygon pours on two reference layers. Since the via electrically connects reference planes where polygon pours exist to facilitate the return path, no Return Path rule DRC violation is detected.

 

When defining a Return Path rule, additional fields are now available to determine the Reference net or net class. These are supported by the Constraint Manager, DRC and the PCB CoDesign feature.

Determining the Reference in the PCB Rules and Constraints Editor dialog
Determining the Reference in the PCB Rules and Constraints Editor dialog

Determining the Reference in the Constraint Manager
Determining the Reference in the Constraint Manager

For more information, refer to the High Speed Design page.

Streamlined Approach for Overlapping Polygon Pours

This feature is available when the PCB.Polygon.AdvancedPour.NoDiffusion and PCB.Polygon.AdvancedPour options are enabled in the Advanced Settings dialog.

This release introduces a streamlined approach for resolving overlapping polygon pours. A lower-priority polygon will only be poured outside of the boundary of a higher-priority polygon that is either completely nested within it or partially overlaps it, resulting in a significant performance using less time to repour polygons.

In the example shown below, a polygon that belongs to net IO_2V5 (green) is a higher-priority polygon and a polygon that belongs to net GND (pink) is a lower-priority polygon, and the IO_2V5 net polygon was poured before the GND net polygon. While there are voids formed by densely placed vias in the IO_2V5 net polygon and the GND net polygon fully overlaps it, these voids are not filled by the GND net polygon because it is a lower-priority polygon.

For more information about the configuring the pour order, refer to the Polygons on Signal Layers page.

Rounding for Diff Pair Gap/Width Transitions

This feature is available when the PCB.Routing.RoundedDPTransitions option is enabled in the Advanced Settings dialog.

This release brings support for automatically adding rounded miters at gap/width transitions during Any Angle diff pair interactive routing or rounded diff pair glossing, particularly at room boundaries.

An example of several Any Angle diff pairs that change their gap and width values at the room boundary.

A closer look at a transition.

 

For more information about diff pair routing, refer to the Differential Pair Routing page.

Sawtooth Rounding

This feature is available when the PCB.TraceTuning.Sawtooth.Rounding option is enabled in the Advanced Settings dialog.

You now can apply rounded corners to sawtooth patterns when interactive length tuning and interactive diff pair length tuning. In the Rounding field of the Properties panel, enter the desired rounding percentage between 0% (default) and 50% or use the  buttons to decrease or increase the Rounding value per the fixed 5% interval provided in the Step field.

The rounding feature can also be accessed when using the automatic length tuning feature (Route » Automatic Length Tuning). In the Auto Tuning Process dialog that opens after initiating the command, the Rounding and Step options are available on the Within Pair Matching tab.

For more information about sawtooth patterns, refer to the Length Tuning page.

3D-MID Export of Tracks to Centerline Curves

This feature is available when the 3DLayout.Export.TracksAsLines option is enabled in the Advanced Settings dialog.

To support 5-axis production processes, tracks on the 3D substrate can now be exported as centerline curves when exporting the 3D-MID design into STEP format.

Tracks in the 3D-MID design can be exported into a STEP file as centerline curves. The 3D-MID document is shown on the left and the exported STEP file is shown on the right, with track centerlines highlighted in green.
Tracks in the 3D-MID design can be exported into a STEP file as centerline curves. The 3D-MID document is shown on the left and the exported STEP file is shown on the right, with track centerlines highlighted in green.

Also, when exporting a 3D-MID design into any available format, a text file (<3DMIDDocumentName>_tracks.txt) is generated in the same folder as the exported 3D-MID file. This text file includes information about the location of each of the tracks in the design, as well as their width and net attributes.

This feature applies only to tracks. Other copper objects (pads, regions, etc.) are exported as surfaces, as before.

For more information, refer to the 3D-MID Design page.

Automatic Face Filling

This feature is available when the 3DLayout.FaceFilling option is enabled in the Advanced Settings dialog.

This release delivers a first-step implementation of the ability to fill the faces of the 3D substrate in a 3D-MID design document with a geometric pattern. This functionality is especially aimed at those wanting to quickly create a geometric covering for security purposes, such as a protective mesh for secure payment terminals.

To use this feature, choose the Route » Automatic Face Filling command from the main menus when a trace is selected. Use the Face Filling dialog that opens to configure the geometry properties of the pattern and the number of traces to be used in the creation of the geometric pattern, and then click OK. The surface will be filled with a pattern whose overall height equals the length of the initial track and which extends perpendicular to the track up to surface boundaries while avoiding obstacles.

  • While multiple placed tracks could be selected before running the automated filling, use of a single track is more stable at this time.

  • In order to have the ability to use the automatic face filling feature on any surface, the 3DLayout.FaceFilling.AllowAllSurfaces option must be enabled in the Advanced Settings dialog. When this option is disabled, the feature can be used on flat surfaces only.

For more information, refer to the 3D-MID Design page.

Dynamic Re-route on Component Drag

This feature is available when the PCB.ComponentDrag.EnableDynamicReroute option is enabled in the Advanced Settings dialog.

Additional options are available in the PCB Editor – Interactive Routing page of the Preferences dialog that help to better control re-routing. When the Component re-route option is enabled, in the fields below, you can define the maximum number of connections that a moving component can have before the routing engine will no longer attempt to re-route. The up to xx pins dynamic field is used to specify the maximum number during movement (i.e., dynamically re-route as the component is being moved). Use the up to xx pins on drop field to specify the maximum number at final placement (i.e., when the component is 'dropped' into final position). 

For more information, refer to the Modifying Existing Routes page.

Using Polygons on Power Planes

This feature is available when the PCB.SplitPlanes.Pouring option is enabled in the Advanced Settings dialog.

Traditionally, a PCB power plane is designed as a negative, that is, the objects placed on a power plane layer become voids in the copper when the board is fabricated. This approach is used because it is more efficient to generate the output data this way, as the bulk of a plane layer is normally copper; voids in the copper are only needed in specific locations such as around non-connected pads, or as separation voids when the plane is divided into different voltage regions.

As part of improving support for more complex power plane design, it is now possible to define power planes as polygons. Working in this mode does not affect the approach to designing a power plane; they are still defined in the negative – so placing an object creates a void in the copper, and they continue to be split into separate regions by placing a split line.

The advantage of using polygons is that copper islands, narrow necks and dead copper can automatically be detected and removed.

Although the layer appears the same, using polygons on the plane layers allows for more comprehensive checking of the integrity of the copper.
Although the layer appears the same, using polygons on the plane layers allows for more comprehensive checking of the integrity of the copper.

Notes about the Polygons on Plane mode:

  • After enabling the option, review each plane layer and repour the plane polygon(s) with the polygon options configured to suit your design needs.
  • Connections and Clearances for plane layers are defined by the PlaneConnect and PlaneClearance design rules.
  • After modifying a plane (connect or clearance) design rule, repour at least one polygon on each plane layer, to update the connections/clearances on that layer.
  • Edits made on a plane layer, such as modifying the location of a split line, cause an automatic repour of polygons on that plane layer.

For more information, refer to the Internal Power & Split Planes page.

Via Annular Rings on Terminating Plane Layers

This feature is available when the PCB.SplitPlanes.ViaShapes and PCB.SplitPlanes.Pouring options are enabled in the Advanced Settings dialog.

An annular ring has always been included on a signal-terminating layer. This release includes the introduction of an annular ring shape when the terminating layer (the first and/or last layer of the via) is a plane layer, regardless of whether the via on that layer is being connected.

Terminating plane layers now include an annular ring for all vias.Terminating plane layers now include an annular ring for all vias.

For more information, refer to the Internal Power & Split Planes page.

Compact Parameter Auto-Positioning for Discrete Parts

This feature is available when the Schematic.CompactAutopositionForDiscreteParts option is enabled in the Advanced Settings dialog.

This release improves the positioning of parameters for components placed on a schematic sheet by introducing a compact auto-positioning option for 2-pin discrete components (when horizontally oriented). Enabled using the new Compact Autoposition for Discrete Parts option on the Schematic – General page of the Preferences dialog, this feature acts solely on the Designator and Value parameters to place them tightly around the second pin of the device symbol. All other parameters remain untouched in their placed locations.

For components placed from a Workspace library, parameter visibility is determined by properties of the Workspace folder where corresponding Component Items reside. Refer to the Working with Component Folders and Items page to learn more about controlling parameter visibility when placing Workspace library components.
For more information, refer to the Searching for & Placing Components page.

Same-Net Clearance Rule Between Polygon Pours and Pads/Vias

This feature is available when the PCB.PolygonSameNetClearance option is enabled in the Advanced Settings dialog.

Added support to Design Rule Checking (DRC) for applying and observing a defined same-net clearance constraint in the following cases:

  • between polygon pours

  • between polygon pours and pads/vias (where the pad/vias do not have a direct physical connection to the pour and are located in or outside of the pour area).

Also, the pouring of polygons now adheres to defined same-net clearance rules between a polygon pour and a pad/via. When there is a clearance constraint between a pad/via and a polygon pour of the same net, the polygon pour will be poured to maintain this constraint (provided the pour is in Don't Pour Over Same Net Objects or Pour Over Same Net Polygons Only pouring mode).

Javascript ID: SameNetPolygons_AD24_5

A PCB with polygon pours in Don't Pour Over Same Net Objects pouring mode. The polygons are poured to maintain the clearance constraint between polygons of the same net and between polygons and pads/vias of the same net.

The same PCB with polygon pours in Pour Over All Same Net Objects pouring mode. The polygons are poured without maintaining the clearance constraint, and constraint violations are detected between polygons of the same net and between polygons and pads/vias of the same net.

The same PCB with polygon pours in Pour Over Same Net Polygons Only pouring mode. The polygons are poured to maintain the clearance constraint only between polygons and pads/vias of the same net, and a constraint violation is detected between polygons of the same net.

For more information, refer to the Polygons on Signal Layers page.

Export an Image of the Power Network Tree – Power Analyzer by Keysight

The Power Analyzer by Keysight release 1.0.7 includes a new feature that helps to document the analysis of the power network in your design. 

When you are examining the Tree View in the Power Analyzer by Keysight document (<ProjectName>.pdnaK), click the  button to export a PNG-format image of the entire network tree to a new schematic document. The schematic is automatically titled Power Delivery Tree.SchDoc.

Javascript ID: PABK_ExportTree

To help with the documentation process, an image of the entire Power Network can be exported directly to a schematic sheet.

To help with the documentation process, an image of the entire Power Network can be exported directly to a schematic sheet.

For more information, refer to the Power Analyzer by Keysight QuickStart Guide.

Defining Clearance By Layer

This feature is available when the PCB.Rules.ClearanceByLayer option is enabled in the Advanced Settings dialog.

When designing a PCB, you may need to adjust the clearances between primitives differently (track, via, polygon, etc.) depending on the layer. For example, the clearance between copper tracks on inner layers must be 35 µm, and only 18 µm is needed for outer layers. Another example is the clearance between a via or through-hole (multi-layer) pad and other copper objects – if the pad/via has shapes of different sizes on layers, you might need to define different clearances for these layers.

Beginning with this release, you can define the clearances by layer using controls below the clearance matrix in the Constraints region of the Clearance design rule. By default, the All Layers tab is shown, and the matrix is used to configure clearances between objects on all signal layers. Click the Add control, then select an entry of the specific signal layer or the group of layers (outer/inner layers) for which you want to configure the clearances and then configure the values of clearances on the added tab as required.

 

If a cell in the clearance matrix has different values on added layer tabs, an asterisk will display next to the value in that cell on all tabs. Hover the cursor to display a tooltip listing the values of this cell for different layers.

To provide backward compatibility with earlier versions of Altium Designer, a new Clearance rule is created according to each layer/layer group tab added using the new functionality when the PCB document is opened in a version of Altium Designer where the functionality has not yet been implemented.

For more information, refer to the Electrical Rule Types page.

Altium Performance Monitor

This feature is available when the System.Performance.Monitor option is enabled in the Advanced Settings dialog.

This release includes the Altium Performance Monitor, which monitors your installation of Altium Designer and collects important debugging data in the event of a system freeze (when a process takes longer than it should to execute). Running in the background (Altium.Performance.Monitor) as a distinct process under the main application (X2.exe), if the software ‘hangs’ at any point, the Monitor will gather call stack information, package it to a temporary file, and send the data to Altium for investigation.

Note: This new functionality is part of the Altium Product Improvement Program. Therefore, the Participate option on the System – Product Improvement page of the Preferences dialog must also be enabled.

Additional Features/Functionalities

  • Primitive Delay Cache: A new advanced settings option – PCB.Performance.UseNetDelayCalculationCache – is available in the Advanced Settings dialog with this release that saves/loads the calculated relative delay for each type of primitive to/from cache. This improves the performance in calculating the delay when reopening a design and selecting a primitive for the first time.

  • Git Fast Clone: A new advanced settings option – VCS.GitFastClone – is available in the Advanced Settings dialog with this release which, when enabled, improves the speed when opening a Git-based project from a connected Workspace. A special server endpoint is used to make the underlying 'git clone' operation faster (to obtain the local repository for an existing (remote) Git repository). In tests with a design project of 500 MB, the opening time was less than a minute with the option enabled (compared with 4-5 minutes with the option disabled).

  • Open CASCADE Library for 3D-MID Documents: A new advanced settings option – 3DLayout.OpenCascade – is available in the Advanced Settings dialog with this release which, when enabled, switches from using the C3D library for geometric modeling of a 3D-MID document (*.PcbDoc3D) to using the Open CASCADE library.

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

The features available to you depend on which Altium solution you have – Altium Develop, Altium Agile Teams, Altium Agile Enterprise, or Altium Designer (on active term).

If you don’t see a documented feature in your actual software, contact Altium Sales to find out more.

Legacy Documentation

Altium Designer documentation is no longer versioned. If you need to access documentation for older versions of Altium Designer, visit the Legacy Documentation section of the Other Installers page.

Contents