Improvements in Beta
This page includes detailed information for features and functionality that are currently available to Beta users.
Features in Closed Beta
Tabbed Routing
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.
-
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).
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).
For more information, refer to the Adding Tabs to Routing page.
Tabbed Routing – Enhancement in Altium Designer 26.12
Added Ability to Select and Deselect Arcs
It is now possible to select and deselect arcs when configuring tabbed routing. After running the Tabbed Routing command, click an arc that is not currently 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).
Diff Pair Auto-shrinking
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.
For more information, refer to the Differential Pair Routing page.
Dynamic Symbols
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.
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.
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.
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.
Dynamic Symbols – Enhancement in Altium Designer 26.12
Updated Drag-and-Drop on the Pins Tab
When working with the pins of a selected connector component (with dynamic symbol) in the wiring diagram's design space, the Pins tab of the Properties panel has been enhanced to provide 'drag and drop' controls on the left-hand side of a selected pin's entry , to allow faster rearrangement of pins within the same part, across parts, and to move unplaced pins into a part.
Connection Table in Layout Drawing
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.
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.
Wiring List – Enhancement in Altium Designer 26.12
Highlight Bundle When Wire Entry Selected in Wiring List
In a harness layout drawing (*.LdrDoc), when a wire entry is selected in a wiring list on the Wiring tab of the Properties panel for a selected harness connector component, the associated bundles are now highlighted in the design space.
Advanced Via Fencing
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.
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.
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).
For more information, refer to the Adding Via Stitching & Via Shielding page.
Via Fencing – Enhancements in Altium Designer 26.11
Shielding Now Follows Board Outline
When applying a via shielding pattern, Inner shielding support has been enhanced for polygon pours, to ensure shielding vias are placed only near a polygon's outline or edge of the board.
Ability to Overlap Annual Rings of Shielding Vias
When applying a via shielding pattern, it is now 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).
Last Shielding Via Removal
When applying a via shielding pattern, the last via in the shielding contour will now be removed if it would otherwise violate the Via Pitch constraint.
Advanced Via Fencing – Enhancements in Altium Designer 26.12
Enhanced Via Shielding Pitch Optimization
When configuring a via shielding pattern, the Optimize Pitch option has been enhanced to 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.
Improved Via Stitching on Hatched Polygon Pours
Via stitching on hatched polygon pours has been improved. Now a stitching via will automatically be placed if its center is located on copper within the polygon.
Added Option for Stitching Through Other Net Polygon Pours
When configuring via stitching, you now 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 addition of this option removes the dependency of this functionality on having to enable the Force Vias option (as was the case previously). The new option – Stitch through other-net polygons – is located in the Advanced collapsible region of Stitching Parameters in the Properties panel.
Enhanced Via Stitching Preview
The preview for a configured via stitching pattern has been enhanced to more accurately represent the final pattern that will be generated.
Modern Comment Markers
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 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 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 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.
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.
When browsing harness components in your Workspace Library through the Components panel, a preview of the related harness entity model is provided
For more information, refer to the Creating a Harness Component page.
Harness Library Components – Enhancements in Altium Designer 26.10
Additional Validation Checks for Harness Connectors
Additional validation checks associated with a defined cavity view for a harness connector type harness entity have been added to the Violations Associated with Harness Entities section of the Data Management – Component Rule Checks page of the Preferences dialog:
-
Duplicate Cavity by Name – this violation occurs when the harness entity's cavity model has two or more cavities with the same name.
-
Missing Cavity Crimp – this violation occurs when no crimp is associated with a cavity in the harness entity's cavity model.
-
Missing Cavity Name – this violation occurs when no name is specified for a cavity in the harness entity's cavity model.
-
Missing Cavity Seal – this violation occurs when no seal is associated with a cavity in the harness entity's cavity model.
-
Missing Plug for Cavity Seal – this violation occurs when no plug is assigned to a seal associated with a cavity in the harness entity's cavity model.
Component Rule Check Added to Harness Workspace Item Menus
Added the Component Rule Check command to the Projects panel's right-click context menu for both Harness Entity and Harness Entity Template Workspace items.
Restricted Seal Assignment in Cavity Models
When adding an associated seal to a cavity through the Properties panel (with that cavity selected in the Cavity Model editor), you can now only add one type of seal. If an Individual type seal is assigned to a cavity, it is not possible to assign an Interface type seal, and vice-versa.
Added Place Cavity Command to the Main and Right-click Menus
Added the Place Cavity command to the Cavity Model editor's main Place menu, as well as the right-click context menu accessed from within the design space.
Harness Library Components – Enhancements in Altium Designer 26.11
Added Default Physical Views
Default physical views are now presented instead of a graphical view when importing data from a wiring diagram into the layout drawing for a harness design. To define a physical view as default for a harness component, enable the view's Set as default view for layout drawing option on the Views tab when editing a linked harness entity model/template.
Cavity Components Added to BOM
Cavity components (crimps/seals) are now presented in the ActiveBOM, as well as the BOM table in a harness manufacturing drawing (*.HarDwf).
Removed Superfluous Crimp and Seal Tabs
When previewing the cavity model for a harness connector type harness entity, on the Cavity Model tab of the Harness Entity editor, the Associated Crimps and Associated Seals tabs will no longer be shown depending on the settings for the Built in Crimp and Sealing Type parameters (on the General tab of the editor):
-
The Associated Crimps tab is not shown when the Built in Crimp option is enabled.
-
The Associated Seals tab is not shown when the Sealing Type option is set to Unsealed.
Added Ability to Update Out-of-Date Crimps and Seals
When defining the cavity model for a harness connector type harness entity, if any crimp or seal components associated with a cavity are not up to date, information is now presented below each applicable section (Associated Crimps and Associated Seals) in the Properties panel when the cavity is selected in the design space. This will let you know if all components are up to date and, if at least one is not, display how many are out of date and provide the ability to update them to their latest revisions (by clicking the
button).
In addition, warnings are now presented in the Properties panel and in a banner at the bottom of the Cavity Model editor design space itself, when settings for the cavity model differ from those of the parent harness entity model. This covers cavity view projection being out of sync with the 3D model for the harness entity, and where crimp or seal configuration is out of sync with the parameters defined in the harness entity.
Interactivity Cross-highlighting for Cavity Model Preview
Cross-highlighting functionality is now available on the Cavity Model tab of the Harness Entity editor, when previewing the cavity model for a harness connector type harness entity. Clicking on a cavity in the preview area will highlight the row for that cavity, on the Cavities tab of the Cavity Details region, and vice versa.
Harness Library Components – Enhancements in Altium Designer 26.12
Visibility of Harness Connector Entity Model Parameters in Layout Drawing
The four parameters defined for a Harness Connector type harness entity model (Connector Gender, Crimp Gender, Sealing Type, and Built in Crimp) are now presented in the Parameters region of the Properties panel when a connector using this entity model is placed and selected in the layout drawing design space.
Grouping of Cavity Names
When browsing Cavity Details on the Cavity Model tab of the Harness Entity editor, Assigned Cavities (on the Associated Crimps and Associated Seals tabs) are now grouped (into a 'range') when at least three sequential cavities are involved. This is supported for the following cavity naming:
-
Numeric, without zero-padding (e.g.,
1,2,3-->1-3). -
Numeric, with zero-padding (e.g.,
01,02,03-->01-03). -
Non-numeric (e.g.,
D,E,F-->D-F).
Note that cavity groups/ranges are listed first, followed by all other cavities, sorted alphabetically.
Related Components
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.
For more information, refer to the Single Component Editing and Batch Component Editing pages.
Design Reviews
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.
Design Reviews – Enhancements in Altium Designer 26.10
Creating a Review for Non-saved and Out-of-date Projects
It is now possible to create a review if you have made local changes to the project, without saving them first.
Also, if a later version of the project exists in the Workspace, you can now create a review without having to update your local version first.
Creating a Review from the Main Menus
The Create Design Review in Web command is now available from Altium Designer's main Project menu.
Selectable Harness Source within Multi-board Design
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.
For more information, refer to the Working with Connections page.
Interactive Dynamic Phase Tuning
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.
For more information, refer to the Length Tuning page.
Improved Return Path Via Detection
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 Constraint Manager
For more information, refer to the High Speed Design page.
Streamlined Approach for Overlapping Polygon Pours
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 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.
For more information about diff pair routing, refer to the Differential Pair Routing page.
Sawtooth Rounding
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
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.
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.
For more information, refer to the 3D-MID Design page.
Automatic Face Filling
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.
For more information, refer to the 3D-MID Design page.
Automatic Face Filling – Enhancement in Version 25.5
Support for Non-flat Surfaces
This release extends the functionality of the automatic face filling feature with the ability to use it on any surface (not just flat). In order to use this feature, the 3DLayout.FaceFilling.AllowAllSurfaces option must be enabled in the Advanced Settings dialog.

An example of using the automatic face filling feature on a cylindrical surface
Automatic Face Filling – Enhancement in Version 25.4
Support for Multiple Output Traces
This release extends the functionality of the automatic face filling feature with support for defining the number of traces to be used in the creation of the geometric pattern, when automatically filling a face of the 3D substrate. In the Face Filling dialog, use the new Output Traces Count option to define the desired number of output traces.
Dynamic Re-route on Component Drag
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
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.
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
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.
For more information, refer to the Internal Power & Split Planes page.
Compact Parameter Auto-Positioning for Discrete Parts
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.
Same-Net Clearance Rule Between Polygon Pours and Pads/Vias
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).
|
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. |
Same-Net Clearance Rule Between Polygon Pours and Pads/Vias – Enhancement in Version 24.5
Pouring Polygons Around Same-Net Pads and Vias
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).
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.
|
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. |
Defining Clearance By Layer
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.
Altium Performance Monitor
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.


















).
).
).















).









































