New in Altium Designer

---

Schematic Capture Improvement

Renaming a Reuse Block

You can now rename a Reuse Block for a PCB or schematic by using the Rename command, which can be accessed from the  sub-menu (shown below) and the right-click context menu of the Design Reuse panel. The Rename Reuse Block dialog opens; enter the desired new name of the Reuse Block in the dialog.

PCB Design Improvements

Drill Tools

The ability to generate additional drill tools based on the Drill Symbol groupings defined for your PCB’s Drill Table has been introduced in this release. Enable the Generate Additional Tools by Drill Symbols option in the NC Drill Setup and ODB++ Setup dialogs to access this feature. Previously, drill groupings could only be assigned in a Drill Table object that needed to be manually corrected when necessary. The same drill information is available between the PCB, printouts, and the drill-related fabrication data. This will ultimately decrease fabrication costs and avoid errors arising from manual, error-prone output adjustments.

Columns that are already present in the existing NC Drill files (*.DRR) will not be excluded even if they are not in the drill symbols grouping. Only additional columns used in drill symbols grouping will be added.

Import 3D Models in SOLIDWORKS

Added the ability to import a 3D model that is in SOLIDWORKS Parts File (*.SldPrt) format that is created from versions 2022 or 2023 of SOLIDWORKS. This support has been added when using a generic 3D model with a 3D Body object.

Generate Modified PCB Components as Separate Entries

Previously, when a footprint of a specific component was modified, all footprints with the same name were also changed in outputs. The modification was not being accounted for properly. This release sees enhancements to assist you in generating correct outputs. The affected outputs are the following:

• ODB++ – the Distinguish different footprints with the same name option has been added to the ODB++ Setup dialog. When the option is enabled, the same-named different footprints are distinguished in the generated ODB++ output, so if some of the footprints with the same name have a different structure, the change to one component's footprint will not be propagated to all components having a footprint whose name is the same.

  

• IPC-2581 – the Distinguish different footprints with the same name option has been added to the IPC-2581 Configuration dialog. When the option is enabled, the same-named different footprints are distinguished in the generated IPC-2581 output with a numeric suffix (_n) after their name.

  
  An example of the IPC-2581 output generated with the Distinguish different footprints with the same name option enabled. LED LED9 was modified in the PCB document, and different same-named footprints are distinguished by a unique numerical suffix when the data is generated.

• Pick & Place files – the Distinguish different footprints with the same name option has been added to the Pick and Place Setup dialog. When the option is enabled, the same-named different footprints are distinguished in the generated Pick-and-Place file with a numeric suffix (_n) after their name.

  
  An example of the Pick and Place output being configured with the Distinguish different footprints with the same name option enabled. Capacitors C10 and C11 were modified in the PCB document, and different same-named footprints are distinguished by a unique numerical suffix when the data is generated.

• Draftsman documents – the same-named different footprints are distinguished in the Draftsman documents, so if some of the footprints with the same name have a different structure, the change to one component's footprint will not be propagated to all components having a footprint whose name is the same (e.g., on the Board Assembly View).

Customized Round Rectangles and New Chamfered Rectangle Pad Shape

Pad shapes now include the ability to customize the corners of existing rectangles. You can customize the corners of an existing rounded rectangle pad by toggling the rounded corners on or off using the Properties panel. Choose Rounded Rectangle from the Shape drop-down in the Pad Stack region of the Pad mode of the Properties panel, then enable the Select Corners option. Select the desired corner(s) to round and enter the desired Corner Radius as shown below. Note that if all four corners are enabled (rounded), the pad type will be a normal (not customized) Rounded Rectangle. 

Chamfered Rectangle has been added as a pad type. You can enable/disable the desired corners using controls in the Properties panel to create custom pad shapes. Choose Chamfered Rectangle from the Shape drop-down in the Pad Stack region of the Pad mode of the Properties panel, then enable the Select Corners option. Select the desired corner(s) to chamfer and enter the desired Corner Radius as shown below.

Data Management Improvements

Display VCS Commit ID in Short Hash Format

Special strings with a short hash format (the first eight characters) have been added and can be used to display the VCS (Git-only) commit ID in the schematic, PCB and Draftsman editors. Refer to the following images for access and examples of the full commit ID (highlighted in green) and the new short hash format (highlighted in purple).

• Schematic     

• PCB

• Draftsman

Circuit Simulation Improvements

Schematic Variant Support

Variants are now supported for all mixed-signal simulation modules; simulations will be performed for the active variant.

PSpice Enhancements

• Support has been added for PSpice digital tristate gates (AND3, AND3A, OR3, OR3A, XOR3, XOR3A, BUF3, BUF3A, NAND3, NAND3A, NOR3, NOR3A, NXOR3, NXOR3A, INV3, and INV3A).
• Support for timing models (UTGATE) for PSpice digital gates has been added.
• Support has been added for input/output models (UIO) for PSpice digital gates.
• Simulation options DIGIOLVL, DIGMNTYMX, DIGMNTYSCALE, and DIGTYMXSCALE were added to customize PSpice timing and input/output models. These can be found on the Advanced tab of the Advanced Analysis Settings dialog (click Settings in the Simulation Dashboard panel).

Zero Delay in Timing Models

The ability to use zero time delays in all digital components has been added. When the number of cycles reaches a prescribed limit (limits are set at 50 iterations), an error is reported and the simulation terminates.

Features Made Fully Public in Altium Designer 22.11

The following features have been taken out of Open Beta and have transitioned to Public in this release:

• New Gerber Dialog with Improved Support for PCB Panels - available from 22.4 
• Improved Component Placement Performance - available from 21.6

Schematic Capture Improvements

View Alternative Pin Names

This release introduces the ability to view available alternative pin names. In the Component mode of the Properties panel on the Pins tab, use the Show Full/Show Short links at the top of the grid to show or hide the alternative pin names for all pins listed. When in Show Full mode, all extended names are displayed in the Name column and the search function will search for all extended names. When in Show Short mode, only the current pin name is displayed.

Display the full or short pin name; hover the cursor over the image to see full and short name examples.

PCB Design Improvements

Added Max Current and Resistance Values for Tuning Objects

Calculated Max Current and Resistance values are now available in the Net Information region of the Properties panel for a selected tuning object (i.e. Accordion, Sawtooth, and Trombone).

Max Current is the maximum current that the selected object(s) can carry as determined from the IPC-2221A formula (Section 6.2):  

I = k * ΔT^0.44 * A^0.725

where:

I = current [amps]
A = cross-sectional area [sq mils] (trace width * layer stack copper thickness)
ΔT = allowable temperature rise above ambient [°C]
k = constant, such that:

k = 0.048 for outer layers
k = 0.024 for inner layers

Resistance is the sum of the resistance of the selected object(s) determined from the derived formula:

R = (ρ * L / A) 

where:

R = resistance [Ω]
ρ = resistivity of copper [Ω*mm²/m]
L = trace length [m]
A = cross-sectional area = T * W [mm²]
T = trace thickness (from layerstack) [mm]
W = Trace width [mm]

Assumptions:

• Ambient temperature = 22 °C
• Allowable temperature rise = 20 °C
• Thruhole copper wall thickness = 0.018mm 
• Resistivity of copper = 0.017 Ω*mm²/m

Improved Detection of Minimum Annular Ring Violation

Violations of the Minimum Annular Ring design rule can now be detected for pads and vias with connections on layers on which pad/via shapes are smaller than the pad/via hole (e.g., if pad/via shapes have been configured manually in the Properties panel or removed by using the Remove Unused Pad Shapes tool). An example of the new behavior is shown in the image below.

An example of the improved violation detection for the Minimum Annular Ring design rule.

Data Management Improvements

Commit Tags

This release introduces support for adding a single, custom-named tag to any commit of a design project (and only where that project is stored in a Workspace under its internal Git VCS system). Tags can greatly help you to navigate through the project history quickly by 'tagging' a particular commit to share or help to quickly find the desired stage of the design. You can create a tag only for the commit that is already saved in the Workspace. Tags can be created when viewing the history for the project (right-click on the name of a project or document then choose History & Version Control » Show Project History. Click  to open the menu then choose Create Tag as shown in the image below.

After running the command, the Create Tag dialog opens. Enter the desired tag then click Create. Tags are displayed on the History tab as shown below.

When the project is released using the Project Releaser and its latest commit does not yet have a tag, a tag will be assigned automatically to this latest commit. This tag will be in the form of RELEASE_<RevisionID>, where <RevisionID> is the revision number of released project sources (A.1, A.2, etc.,), for example, RELEASE_A.3.

A tag is created automatically for the latest commit by the Project Releaser.

You can rename or delete tags by clicking  and then hovering over the Tag entry as shown below. A dialog will open in which you can enter the new name of the tag. If Remove is selected, the tag is deleted immediately.

The Create Tag command can also be accessed by right-clicking on the name of a project or document in the Projects panel and then choosing History & Version Control » Create Tag to create a tag for the last/latest commit.

Сustom Part Providers

Added support for Custom Parts Providers when specifying preferred suppliers at the project level to be used by ActiveBOM when processing supply solutions. To access the Project Part Providers Preferences dialog, in the Properties panel of an ActiveBOM document (*.BomDoc), click the Edit button associated with the Favorite Suppliers List in the Supply Chain region. Enable the Custom Parts Provider option to view your custom part sources along with all other providers.

Manufacturer Part Search Panel Improvements

Improvements to the Manufacturer Part Search panel introduced in this release make the panel more intuitive to work with searched components and populate your own Workspace Library.

Controls for Saving a Component

When connected to a Workspace, the panel’s controls will naturally align with component acquisition to that Workspace with the Save button, the Save to My Workspace command in the menu drop-down of this button, or the Save to My Workspace command of the component entry's right-click menu. Use the Save button to save the component to the current Workspace by choosing the component type and then choosing which component data you want to acquire. 

The saving process can also be initiated by hovering over a component’s image in the results and then clicking  to initiate the save process.

Saving a Component without Models

Previously, you could only acquire components that had models. This release allows you to save model-less components to your Workspace Library, obtaining them with their richness of parametric data and leaving you to whip up models at a later date.

Acquire component data even if the component has no models.

Resolving Mismatches between Parameters and Template

Detecting any mismatches between the naming of parameters between the component being acquired and a template in your Workspace, you can now fix such occurrences on the fly during acquisition, and save those changes to your global preferences. In the Use Component Data dialog, disable the Show only matching with template option to show all component parameters. For a parameter with a detected mismatch, use the Fix control to open the Parameter Mapping Configuration dialog and apply the changes as required.

Use the Parameter Mapping Configuration dialog to resolve mismatches between component parameters and the component template.

Part Choice Management Permissions

This release sees an enhanced control for part choice management. The Edit Operation Permissions dialog now includes a new Part Choice Management entry. Using this entry, administrators of the Workspace can manage which users and roles are able to change component part choices.

The Part Choice Management entry in the Edit Operation Permissions dialog

Any user who does not have permission to manage part choices will be prevented from doing so when attempting to add/modify part choices for a component through the Component Editor (in its single and batch component editing modes).

 
A user will be prevented from editing a component's part choices if they do not have permission to do that.

A user without Part Choice Management permission will also be prevented from editing part choices when accessing the Operations » Create/Edit PCL command from the right-click menu of a Workspace component entry in the Components panel, accessing the Edit PCL in Library command from the Add Solution button menu in an ActiveBOM document or clicking the Edit button on the Part Choices aspect view tab of the Explorer panel when browsing a component.

Circuit Simulation Improvements

Default Settings for Digital and Analog Models

Default settings are now provided and used when ADC/DAC components are automatically inserted by the simulation engine to process analog-to-digital and digital-to-analog interconnections. Settings for digital input low and high voltage (DIGIL, DIGIH), digital input rise and fall delay times (DIGIRD, DIGIFD), digital output low and high voltages (DIGOL, DIGOH), digital output undefined voltage (DIGOU), and digital output rise and fall times (DIGOR, DIGOF) can be found on the Advanced tab of the Advanced Analysis Settings dialog (click Settings in the Simulation Dashboard panel).

Added Expressions for Capacitor and Inductor Models

For capacitor and inductor models, output voltage (v[<capacitorname>]), power (p[<capacitorname>]), and current (i[<capacitorname>]) have been added as output variables when running an AC Analysis. These are available when adding output expressions prior to simulation. The variables have been added to the Add Output Expression dialog and can also be added as wave items using the Sim Data panel.

Features Made Fully Public in Altium Designer 22.10

The following features have been taken out of Open Beta and have transitioned to Public in this release:

• Detect Copper Primitives with No Net Assigned - available from 22.5
• Working in the Schematic with the 'Find Text - Jump' Dialog - available from 22.9

Schematic Capture Improvements

Working in the Schematic with the 'Find Text - Jump' Dialog

The Find Text - Jump dialog is now a non-modal dialog, which means you can work with Altium Designer’s interface including objects on the schematic sheet while the dialog is open.

New Variant Manager

The process of managing variants in your design has been greatly enhanced. For creating, editing, and managing design variants, a new document-based Variant Manager is now available.

In addition to traditional variant management for specific components in the design, you now have the ability to create groups of components from a chosen schematic sheet, sheets referenced by a chosen sheet symbol, or a chosen component class with a functional-based view of component variations. For each group, you can define one or more ‘options’, which essentially reflect some variation of one or more components in the group. Variants themselves can then be created based on these defined groups and options, with support for creating a hierarchy of variants.

The new Variant Manager allows creating design variants based on options defined for component groups. Shown here is the Variants tab of the Variant Manager with three variants created and different options applied for a component group. Hover the cursor over the image to see the Groups tab where these options are defined.

When a change is made, editing a value within a group option is instantly reflected in all variants that use that group option rather than having to change each varied component across each defined variant one at a time. The impressive time-saving efficiency gained in variant creation and editing will be appreciated by all users, especially those who deal with a sizable number of design variations. No matter if you are dealing with a handful of variants or hundreds, the new document-based variant management interface presents your variants in a far more readable form.

PCB Design Improvements

Minimum Thermal Relief Conductor Gap for Custom Pad Shapes

This release adds the ability to check the minimum gap between thermal relief conductors of custom pad shapes. The new Min Distance option is accessed by enabling the Thermal Relief option in the Pad Stack region of the Properties panel in Pad mode, then clicking the associated  to the right of the option. The Edit Polygon Connect Style dialog opens. The new Min Distance option appears in the dialog when the Conductors by Pad Edges option is enabled. When Min Distance is enabled, you can enter the desired minimum distance of thermal relief conductors of the custom pad. 

Added Detection of Zero Area Polygons in the Health Check Monitor

The Health Check tab in the Properties panel (accessed in Board mode) now gives you the ability to detect and delete polygons with zero areas. The new Zero Area Polygons field has been added to the Polygons category so now you are able to delete all of these polygons at once using the Fix Issues button in the Issues region. 

Added Command to Place a Text Frame

To support the quick placement of a Text object in String and Frame modes implemented in a previous release, a new Text Frame command has been added to the main Place menu and the Active Bar of the PCB and PCB footprint editors in addition to the existing String command.

Use the new Text Frame command to quickly place a Text object in Frame mode.

When the Text Frame command is selected, Frame mode is active for the Text object being placed.

Data Management Improvements

Alternative PCB Layouts in a Reuse Block

When creating a reuse block, multiple PCB models can now be added to it. To do this, use the Add New to Project » PCB command from the right-click menu of the reuse block's entry in the Projects panel.

Use the Rename command from the right-click menu of the added PCB model's entry in the Projects panel to define a meaningful name for it. Use a Design » Update command from the schematic editor main menu to update the required PCB document.

When the reuse block is saved to the Workspace, its PCB models are listed in the reuse block's PCB section within the Design Reuse panel that can be presented by clicking the Show more control within the reuse block's tile. Select the required PCB model in the list, and the reuse block will be placed with this model. The selected PCB model is shown in the preview area of the reuse block's tile when PCB is selected for preview.

Added 'Permissions' Property to Open Project Dialog

The new Permissions field that has been added to the Open Project dialog on the General tab for projects that are in a Workspace allows you to quickly see your permissions for the selected project: Can Edit or View Only.

Added 'View Only' Indicator in Projects Panel

Projects you have shared with viewing-only capabilities by using the Can View option in the Share dialog now display a new View Only indicator in the Projects panel. This non-clickable indicator is displayed for the user with whom you have shared the project.

Note that a project shared with a viewer should be available for download for them so that they can open it in Altium Designer. Click the Advanced Settings control in the Share dialog to configure appropriate settings.

Improved Filter in the Comments and Tasks Panel

The filter in the Comments and Tasks panel (accessed by clicking the down arrow next to the filter icon) has been streamlined to eliminate any inaccuracies between the panel and the Tasks dashboard.

The filter has been updated to display the following:

• Tasks only - enable this option to show only comments that are assigned to a user.
• ASSIGNED TO - all options are disabled by default. Consequently, all tasks/comments are shown and sorted by name (the first entry in the list is the current user). When checkboxes are enabled, only the entries of those enabled will be displayed.

Note that the functionality for creating and managing tasks is not supported with the Altium Designer Standard Subscription. As such, with this level of access to Altium 365, this enhancement will not be available and the filter options in the Comments panel will be the same as in the previous release.

This enhancement is also not available when connecting to an Enterprise Server Workspace.

Ability to Add and Edit Comments in BOM Documents

This release added the ability to create and edit comments in an ActiveBOM document.

A comment can be added to a BOM item in the document in the following ways:

• Click the  button available in the Comments and Tasks panel.
• Click  near the top right-hand corner of the design space.
• Use the Tools » Comment command from the main menus.

After selecting a command, click on a row in the document to add a comment. Alternatively, right-click on a row then select the Comment command to add a comment to this row.

Enable Actionable VCS Status Icons

The feature that provides improved document VCS status has been enabled by default. To recap, this feature turns the VCS icons for project documents in the Projects panel into active controls that can be clicked to access more specific information, along with commands to perform applicable actions. This feature is accessed by the UI.ActionableDocumentStatuses option in the Advanced Settings dialog.

Circuit Simulation Improvement

Source of a Placed Component

The sourced location of a placed component is now displayed in the Sim Model dialog in the Location field. This allows you to quickly see if the source used is the desired location.

Features Made Fully Public in Altium Designer 22.9

The following features have been taken out of Open Beta and have transitioned to Public in this release:

• Custom Names for Multi-functional Pins - available from 22.6
• Ability to Work with Objects Located Outside the Schematic Sheet - available from 22.6
• Support for Alternate Parts in Multi-channel Projects - available from 22.6
• Availability of Designators and Net Names in Text Frames - available from 22.6
• Alphabetically Sort Documents in a Grouped Tab - available from 22.7

Schematic Capture Improvements

Marking Multiple Components Fitted/Not Fitted

This release adds the ability to select multiple components on a compiled tab of the schematic sheet and toggle their Fitted / Not Fitted variation state using the  icon in the Active Bar or the Part Actions » Toggle Fitted/Not Fitted command from the right-click menu of the selection.

Example of toggling Fitted / Not Fitted state for multiple components. Shown here are multiple selected components (C32 - C35) in their Fitted state. Hover the cursor over the image to see that their variation state changes to Not Fitted after selecting the Toggle Fitted/Not Fitted command.

Placing a Reuse Block or Schematic Snippet as a Sheet Symbol

In this release, a reuse block or schematic snippet can be placed on a schematic sheet as a sheet symbol, with the content of this reuse block or schematic snippet placed on an automatically-created child schematic sheet. To do this, select the Place as Sheet Symbol command from the Place button drop-down menu or the block/snippet tile's right-click menu.

Example of placing a reuse block as a sheet symbol. Shown here is accessing the Place as Sheet Symbol command from the Design Reuse panel. Hover the cursor over the image to see the content of the reuse block placed on the automatically created child schematic sheet.

The Place command places a reuse block or schematic snippet right on the active schematic sheet like it was before.

PCB Design Improvements

Custom Pad Shapes

This new feature allows you to create custom shape pads in PCB designs and PCB footprints.

An example component placed in a PCB design and featuring pads of a custom shape.

• Custom pad shapes can be created by converting placed regions or a closed outline, or directly by selecting the new Custom Shape entry from the Shape drop-down in the Pad mode of the Properties panel.
• A placed custom shape pad can be edited by using the Outline Vertices table in the Properties panel, the Edit Shape button in the Properties panel, or the Pad Actions » Modify Custom Pad shape command from the pad's right-click menu.
• Thermal relief connections are supported for custom shape pads to both solid and hatched polygons. You can choose to use conductors from each side of the pad region or use a selected number of conductors so that they intersect the pad origin at a specified angle.
• The query language IsCustomPadShape and IsCustomPadShapeOnLayer keywords can be used to facilitate custom shape pad selection, scoping design rules, etc. You can also use the PadShape_AllLayers, PadShape_TopLayer, PadShape_BottomLayer, and PadShape_MidLayer<n> keywords with the 'Custom Shape' string to get pads of custom shape on a specific layer.
• Custom pad shape templates are supported by the PCB Pad Via Templates panel. A template name for a custom pad shape begins with 'u'.
• When generating your manufacturing output (Gerber, ODB++), a custom pad shape is now output as a true contour with arcs.
• Custom pad shapes are supported when saving/loading the PCB in ASCII format.
• The Mentor Expedition^® Importer supports custom pad shapes. When such pads are imported in Altium Designer, they are imported as pads of the custom shape type.

Added Max Current and Resistance Values for Tracks, Arcs, and Vias

Calculated Max Current and Resistance values are now provided in the Net Information region of the Properties panel for a selected Track, Arc, or Via object.

The Max Current and Resistance values are now provided in Track, Arc, and Via modes of the Properties panel.

Added Diff Pair and xSignal Information

For copper objects on a PCB, the information on the Differential Pair, Differential Pair Class, xSignal, and xSignal Class is now shown in the Properties panel if the selected object is part of a differential pair or an xSignal.

The Properties panel now shows comprehensive information on the differential pair and xSignal of which the selected object is a constituent part.

Click a link in the Net Information region to open the net/differential pair/xSignal in the PCB panel.

Improved Working with Single-line and Multi-line Text Objects

You can now switch between single- and multi-line editing modes using the String and Frame buttons in the Properties panel for a selected Text object. When using single-line String mode, use the Text field to type in the value or use the drop-down to select a special string. When in multi-line Frame mode, the text object properties operate as before.

 
The String and Frame editing modes are now provided in the Text mode of the Properties panel.

Rendering of Self-intersected Regions

This feature allows rendering of self-intersecting regions in the PCB editor in the same way as they will be exported to fabrication outputs (Gerber/ODB++).

Example of a self-intersecting region selected in the PCB editor design space. Hover the cursor over the image to see this region in the generated Gerber output.

Net Priorities When Pasting Objects

The behavior of net assignment for objects pasted in a PCB design has been improved by introducing the priorities of different object types.

When an object is being pasted on a copper layer, and it overlaps a set of objects of different types when pasted, a net of the highest priority object will be assigned to the pasted object. The priorities are as follows (1 is the highest priority):

1. Pad
2. Fill
3. Region
4. Track
5. Arc
6. Via
7. Polygon Pour

A net of the highest priority object is assigned to a pasted object. Shown here is an object (track) pasted over a set of objects of different types with different nets assigned. Since the pad is the object of highest priority in this set, its net (Pad_Net) will be assigned to the pasted object. Hover the cursor over the image to see the result.

When an object is pasted on a copper layer and it overlaps a set of objects of the same type when pasted, a net of the object that is under the cursor when clicking to paste the object will be assigned.

A net of the object under the cursor is assigned to a pasted object. Shown here is an object (track) pasted over a set of objects of the same type (pads). Since pad 2 is the object that is under the cursor when clicking to paste the object, the net of this pad (Pad2_Net) will be assigned to the pasted object. Hover the cursor over the image to see the result.

When a set of physically connected objects is pasted on a copper layer and objects of different types in this set overlap existing objects with different nets, a net of the highest priority object in this set will be assigned to all pasted objects. The above priorities are applied in this case.

The net assigned to the highest priority object is assigned to the set of the physically connected objects. Shown here is a set of connected objects (from left to right: Fill, Region, Track, Arc, Via, and Polygon Pour) pasted over objects (vias) with different nets assigned. Since the fill is the object of highest priority in this pasted set, the net assigned to it (Via1_Net) will be assigned to each object in this set. Hover the cursor over the image to see the result.

The New Version of Open CASCADE Technology

This release sees the introduction of the new Open CASCADE Technology 7.5 version. Using the updated version allows to increase the performance of load and export the STEP 3D-model files, especially for large files.

Detecting Dead Copper Primitives in Net

Copper layer objects with a net assignment but not connected to any Pad object of the same net and not connected with other objects of the same net with connection lines will be checked. To run the check, click Tools » Design Rule Check. Ensure the Report Dead Copper larger than option is enabled on the Report Options page of the Design Rule Checker dialog. (The value field of this option applies to the plane. All other objects are checked regardless of size.) This option is enabled by default. Errors are flagged as an Unrouted Net Constraint in the Messages panel and the Design Rule Verification Report.

Prevent Self-Intersections

When placing or editing a polygon-shaped object (e.g. Polygon Pour or Regions) and a self-intersection of its contour occurs, a warning opens to alert you to this fact. You can Proceed with the current shape or click Revert in the warning to roll back to the last non-intersecting vertex.

Data Management Improvements

Added BOM Compare Functionality

The features for comparing locally saved documents of an Altium 365 Workspace project with a commit or release of this project have been extended by implementing support for BOM documents. Select a command from the Save to Server dialog, the Projects panel, or the Project History view to select a required data set with which the locally-saved documents should be compared.

The BOM compare commands can be accessed from the Projects panel.

Added Output Job to Default Templates

An Output Job option has been added to the Data Management - Templates page of the Preferences dialog, which allows an output job template to be added to the connected Workspace. The option can be accessed from the Add drop-down as shown below.

Circuit Simulation Improvements

Added Support for Digital Nodes

In this release, support for digital nodes has been implemented. Digital nodes are the nodes of the circuit connected only to pins of components with digital models. A new Digital wave type was added to represent logical levels (0, 1, undefined) of digital output waves.

• The components of the Simulation Generic Components library are now digital. That allows using these components in both analog and digital calculations.

• To add a digital wave to an output plot, select Digital from the Waveforms drop-down in the Add Output Expression dialog. Digital waveforms are prefixed with d.

  

  Note that nodes to which both analog and digital components are connected can be plotted as a digital signal or voltage.

• The undefined state of a digital signal is denoted with a double line on plots and with the X numeric value.

  

• Support for the PSpice digital stimulus generator has also been implemented.

Defining a New Simulation Model Using the Sim Model Dialog

In this release, the Sim Model dialog is now used to define a new or edit a referenced simulation model for a Workspace library component being created or edited in the Component Editor in its Single Component Editing mode. That allows you to quickly define a reference to a simulation model from different sources.

Use the Sim Model dialog to define a new simulation model for a Workspace library component.

Improved UI for Managing Output Expressions

A number of features and controls have been implemented in the Simulation Dashboard panel for better management of output expressions from the panel:

• Added a plot number drop-down and a color icon that allows defining the number of an existing plot (or creating a new one) and the wave color without opening the Add Output Expression dialog.

  
• When an output expression field is currently active in the panel (the text cursor is within the field), clicking the + Add control at the bottom of the Output Expression region will add a new output expression below the active expression. The Plot Number and Axis Number values of the active expression will be inherited by the new expression.

• The order of output expression lines can now be changed using the drag-and-drop technique. Click and hold the left mouse button on the free space of an output expression line to move it up or down in the list.

  

New Global Parameters Settings

The Global Parameters tab of the Advanced Analysis Settings dialog now displays calculated values of global parameters along with their formulas. If a global parameter is defined using a formula, its value will be shown in the Value column, with the formula in parenthesis next to the value.

The Global Parameters tab of the Advanced Analysis Settings dialog now shows both calculated values and the formulas of global parameters.

Auto-Assignment Messages Display in Messages Panel

Messages relating to the auto-assigned simulation models are now presented in the Messages panel. Click the Edit Model control for an auto-assigned model to open the Sim Model dialog and also show messages related to this model.

An example of messages related to an auto-assigned simulation model.

PCB Design Improvements

Support for Variants in the Paste Mask Outputs

If your design includes variants with 'Not Fitted' components, these components will no longer have Paste Mask included on their pads. All Paste Mask output types have been updated to support this feature.

Paste mask (dark grey color) is automatically excluded for Not Fitted components. Hover the cursor over the image to show a different variant of this board.

Use the new Allow variation for paste mask option in the Edit Project Variant dialog to enable/disable output of the Paste Mask for the variant being configured.

Ability to Change Tuning Object Layer Properties

You can now change the layer for a tuning object (Accordion, Trombone and Sawtooth) through the Properties panel using the new Layer drop-down in the Properties region as shown below for an accordion object as an example.

Data Management Improvements

SSH to HTTPS Repository Connection 

When pushing changes to a project that is under an external Git VCS or making such a project available online and the repository in which that design resides uses the SSH protocol for connection (not supported by Altium Designer), you are now offered the choice to try to have that repository updated to use the supported HTTPS connection protocol instead (provided the repository itself supports this protocol). 

Enhancements to the Exported Comments PDF

Several improvements have been made to the exported comments PDF report.

• The orientation of the report has been changed for better readability.
• The project name and ID and newly-added document name are active links, which you can use to open the Altium 365 web browser. 
• New Assignee and Status columns have been added to show more information about the comment. 

Actionable Soft-Lock Statuses

When multiple users are editing the same 'soft-locked' document that is part of a Workspace project, an associated conflict status icon appears in the Projects panel. In this release, the conflict status icons provided by the soft-locking functionality are now actionable. You can click the icon to resolve the conflict by reverting your edits.

Disable Repository Structure Validation

The repository validation functionality has been disabled due to the inability to commit to an SVN repository. The functionality will be improved and restored in a future release.

Disable Actionable VCS Status Icons

The feature that provides improved document VCS status has been disabled (by default) for the time being. To recap, this feature turns the VCS icons for project documents in the Projects panel into active controls that can be clicked to access more specific information, along with commands to perform applicable actions. If you have not experienced an impact on performance, you can simply enable this feature again. This feature is available when the UI.ActionableDocumentStatuses option is enabled in the Advanced Settings dialog.

Platform Improvements

Alphabetically Sort Documents in a Grouped Tab

When there are a large number of documents open, they are grouped by document kind or by project using the Group documents by kind option on the System - View page of the Preferences dialog. With this release, the list of documents is sorted alphabetically. When the option By document kind is enabled on the System - View page, documents are sorted alphabetically. When the By project option is enabled, documents are sorted alphabetically within document type. An alphabetized grouping of schematic documents is shown in the image below as an example.

Draftsman Improvements

Ability to Add and Edit Comments in Draftsman Documents

This release added the ability to create and edit comments in a Draftsman document, similar to the existing ability in schematic and PCB documents.

Comments can be created in the following ways:

• Click the  button available in the Comments and Tasks panel.
• Click  near the top right-hand corner of the design space.
• Use the Place » Comment command from the main menus.

Circuit Simulation Improvements

Auto-assign Simulation Models for Components without Models

This feature gives you the option to automatically assign simulation models to components without models. To use this feature, click Assign Automatically in the Components without Models region under the Verification stage in the Simulation Dashboard panel. The search will be sequentially performed in the following sources:

1. Local – the models stored locally and located in the path defined in the Model Path field on the Simulation – General page of the Preferences dialog.
2. Libraries – the installed libraries that are listed on the Installed tab of the Available File-based Libraries dialog.
3. Server – simulation models from the connected Workspace.
4. Octopart – simulation models available in the cloud library.

The models found will be assigned to the components, with pins automatically mapped between the component and simulation model. The results of the auto-assignment are displayed in the Simulation Dashboard panel.

If the simulation model cannot be correctly mapped to the component, this component will be listed under the Components with Partly Assigned Models entry in the Simulation Dashboard panel. You can click the Edit Model link for the component to open the Sim Model dialog and edit the pin mapping.

Quick Access to Simulation Generic Components

In this release, you can now quickly access the most popular simulation generic components (resistor, capacitor, transistors, etc.,) from the Simulate main menu.

These commands are also available from the Mixed Sim toolbar.

Schematic Capture Improvements

Custom Names for Multi-functional Pins

This feature allows for the custom naming of multi-functional pins. Use the new Functions field of the Pin mode of the Properties panel in a schematic library document to enter the desired custom name. After clicking Enter, the custom (alternate) name will display below the field as shown in the image below. There are no limitations for the field, and numbers and/or special characters (&, *, %, etc.,) can be used. All Font Settings for the custom name are the same as the original pin name.

In the Component mode of the Properties panel in a schematic document, the custom names are displayed on the Pins tab.

Custom pin names can also be defined when creating a schematic symbol using the Symbol Wizard. When pin names entered in the Display Names column of the Symbol Wizard contain slashes ('/'), these names will be added as custom pin names to the pins of the generated symbol.

Example of a pin name with slash characters in the Symbol Wizard. Hover the cursor over the image to see the properties of the generated symbol's pin.

Display of pin names on schematic symbols can be managed by clicking on the name of a pin with custom names defined. In the pop-up window that opens, check the function names you would like to display on the schematic symbol. If no custom pin name is selected in the list, the default name will be shown.

Example of a pop-up menu for a pin with custom pin names. Hover the cursor over the image to see this pin after selecting some custom names.

Support for Alternate Parts in Multi-channel Projects

When defining a variant for a multi-channel design, it is now possible to select specific/different alternate parts across the channels. Therefore, the Unsupported multi-channel alternate item check is removed from the Error Reporting tab of the Project Options dialog.

Availability of Designators and Net Names in Text Frames

Component designators and net names in text frames that are placed on the schematic function as links and provide cross-probing capabilities within the schematic and printed PDFs. Use the Properties region of the Text Frame mode of the Properties panel to define the link by using '@' in the Text field to access a list of possible choices. Select the desired primitive to search for; the text frame now includes a link as shown in the second image below. 

Clicking the link to zoom to and highlight that primitive on the sheet. 

Ability to Work with Objects Located Outside the Schematic Sheet

Any schematic design object that is placed outside of the schematic sheet boundaries can now be selected and moved. When an object is selected, the same set of operations and commands can be performed as for an object within the schematic sheet boundaries.

PCB Design Improvements

New Parameters Tab for Board Properties

To provide you with a quick view of the current PCB design's parameters, a new Parameters tab for the Board mode of the Properties panel has been added. The tab lists both system parameters (e.g., the PCB file name) and the parameters calculated from the PCB (e.g., the number of components on the PCB and the board thickness).

The parameter listing can be narrowed down using the filter buttons at the top of the panel. A parameter can be quickly placed as a special string using the Place button at the bottom of the list when the parameter is selected in the panel.

The Parameters tab for the Board mode of the Properties panel provides you with comprehensive parametric information on your PCB design.

Added Check for Unused xSignals and From-Tos in Health Check Monitor

This release sees new checks implemented as part of the PCB Health Check Monitor functionality: Unused xSignals and Unused From-Tos. If the PCB design contains xSignals or From-Tos that are not used in any design rules, they will trigger issues of the respective PCB health checks. Unused xSignals and From-Tos can be removed from the design using the Fix Issues button provided on the Health Check tab.

 
New Unused xSignals and Unused From-Tos PCB health checks can be used to find xSignals and From-Tos that are not used in the design rules of the PCB design.

Improved DRC Performance

Added the following options to the Advanced Settings dialog that improve DRC performance.

• Enable the PCB.EngineX.RuleSystem option to use the new DRC implementation.
• Enable the PCB.EngineX.ExpressionEngine option to use the new Expression Engine implementation.
• Enable the PCB.EngineX.ClearanceRule option to use the new Clearance Rule implementation.

Data Management Improvements

Added Comparison of Local Files with a Commit or Release

Features for comparing locally saved schematic documents with a commit or release of the Altium 365 Workspace project for which these documents are constituent parts have been implemented. To compare the schematic documents with a required data set, select a command from the Compare button menu in the Save to Server dialog, the History & Version Control » Compare right-click menu of the project or project document in the Projects panel, or the  control menu of the new Local Changes tile of the Project History view.

After selecting a command, the comparison results will be presented in a new tab of your default web browser.

An example of schematic comparison results.

Added Design Reuse Mode to the Properties Panel

In this release, a new Design Reuse mode of the Properties panel has been implemented. When a selected schematic or PCB component is part of a reuse block placed in the design, this mode can be accessed by clicking the Reuse Block link provided in the Component mode of the panel. The properties of the component's parent reuse block will be presented in the panel. To return to the properties of the initially selected component, use the Component link.

Access the reuse block properties from a component that is a part of this reuse block. The images above display accessing the properties from a schematic component. Hover the cursor over the image to see access from a PCB component.

Display of General Tasks in the Comments and Tasks Panel

General tasks (tasks applied to the current project but are not associated with a project comment or document) are now shown in the Comments and Tasks panel. These tasks are listed in the panel in a separate group under the entry of the project. For general tasks, the same content and attributes are shown in the panel as for regular tasks (assignee, priority, etc.).

General tasks are now listed in the Comments and Tasks panel.

Circuit Simulation Improvements

Simulation Examples

A set of quick-start simulation examples has been added to the Shared Documents folder (C:\Users\Public\Documents\Altium\<PlatformAndVersion>\Examples for default installation). Each example demonstrates a real-world use case of simulation, complete with information on setting up the simulator and interpreting the results.

Logarithmic Form for the Y-axis

In the Sim Data Editor, the Y-axis for simulation results can now be presented in logarithmic form in the same way that was previously possible for the X-axis. Use the Y Axis Setting dialog to configure the Y-axis to be presented in logarithmic form.

Schematic Capture Improvements

'Find Text' Enhancement

You can now mask the results when using search (Edit » Find Text, Ctrl+F) in a schematic document by enabling the Mask Matching option in the Find Text dialog. When this and the Jump to Results options are enabled, all found elements will be zoomed while other elements are dimmed according to the settings on the System – Navigation page of the Preferences dialog.

Custom Differential Pair Suffixes

Previously, differential pairs were defined by adding specific suffixes, namely _P (positive) and _N (negative), however, the predefined suffixes were found to be too confining for users. To give you more flexibility, differential pairs can now be defined using custom suffixes in the Diff Pairs region of the Project Options - Options dialog. Custom suffixes cannot be added if only one suffix of the pair is defined or if any of the suffixes are used in another pair of custom suffixes. The suffixes cannot contain spaces or underscores ("_").

PCB Design Improvements

PCB Health Check Monitor

The final goal of each PCB design is to get a correct and reliable set of assembly and fabrication outputs, and one purpose of any design tool is to provide a user with tools to find and resolve the issues that could arise during the design process before the design goes to production. During its constant development, Altium Designer delivers enhancements and bug fixes in each release to provide you with a better design experience and to help you avoid some “unhealthy” layout aspects of your PCBs. In some cases, such areas of a board might be fine from the perspective of Altium Designer’s DRC system, not leading to serious fabrication issues. However, they could result in software performance degradation and issues during MCAD co-design or generation of PCB outputs. For example, PCB components could have 360 degrees rotation value in previous versions of Altium Designer, but this situation is not allowed anymore in the current versions – the software will set such components to 0 degrees.

These “unhealthy” board layout elements may be present in designs created in versions of the software before it was improved and fixed in certain areas. To help you in detecting and resolving such issues, and some other issues that can arise under certain conditions, the concept of PCB Health Checks has been introduced. These checks allow you to discover common issues in the PCB design, fix them, and avoid potential problems during the next stages of the design and manufacturing process. The list of available PCB Health checks will grow up moving forward.

The Board mode of the Properties panel (available when no object is selected in the active PCB document) has the new Health Check tab that enables you to configure, perform, and explore the results of the PCB Health Check. Recommendations for fixing the issues of a specific type can also be found on this tab of the panel.

The new Health Check tab of the Properties panel is in the Board mode.

To learn more about this functionality, see PCB Health Check Monitor.

Set Board Shape Visibility for Board Arrays

A new Board Shape option has been added to the Embedded Board Array mode of the Properties panel. This button allows you to control visibility for the board shapes of the PCBs that are constituents of the selected board array.

Use the Board Shape button to control the visibility of the board shape. Hover the cursor over the image to see the difference between the enabled and disabled states.

Improved Print Dialog for Configuring PCB Printouts

The Print dialog has been enhanced to streamline the configuration of the pages to be printed from a PCB design. Some options have been relocated and updated from bullets to highlighted boxes in order to improve the readability for our users. The Pages tab now includes Printout Properties options for the display of surface mounts, through-holes, and design views, as well as a Displayed Layers region to configure specific layers.

Default Units for Fabrication Outputs

Millimeters are now the default units when configuring Gerber, Gerber X2, ODB++, and NC Drill fabrication outputs (File » Fabrication Outputs) as shown in the Gerber X2 Setup and NC Drill Setup dialogs in the image below.

Detect Copper Primitives with No Net Assigned

All copper layer objects with a net assignment of No Net will be checked. To run the check, click Tools » Design Rule Check. Ensure the Report Dead Copper larger than option is enabled on the DRC Report Options page of the Design Rule Checker dialog. (The value field of this option applies to the plane. All other objects are checked regardless of size.) This option is enabled by default. Errors are flagged as an Unrouted Net Constraint in the Messages panel and the Design Rule Verification Report.

Data Management Improvements (22.5)

Improved Project Version Control Statuses

Version control status icons provided in the Projects panel for documents are now active controls that can be clicked to receive more information on the VCS status of the document and access options to perform the relevant actions. For example, clicking the  icon for a document that has locally-saved changes but that have not yet been sent to the Workspace shows the date and time when local changes have been saved, as well as options to save the project changes to the Workspace or revert local modifications of the document.

Click a VCS status icon in the Projects panel to show more information on the document status and access-related actions.

Added 'New Library' Dialog

The New Library dialog has been introduced to facilitate the creation of a new library. The dialog is accessed by choosing File » New » Library from the main menus. It provides the flow to create a new Workspace library component, component template, footprint, or symbol, or for creating an older generation library (file-based or database type library).

Added Ability to Edit Properties of a Local Snippet

The Name, Description, and Path of a local snippet can now be edited through the Snippet Properties dialog that is accessed from the Design Reuse panel by clicking  within the local snippet's tile (or right-clicking anywhere on the tile) then selecting the Edit Properties command from the menu.

Edit properties of a local snippet using the Snippet Properties dialog accessed from the Design Reuse panel.

Schematic Capture Improvements

Display of Alternate Component Parameters

When viewing variants on a compiled tab of a schematic document, alternate part properties are now displayed in the Properties panel, rather than the original component properties that were displayed in previous versions. The alternate part properties are read-only.

An alternate part is defined for a component on the schematic sheet. When a compiled tab is selected, the Properties panel will show the properties of the component for the current variant.

Data Management Improvements

New Design Reuse Functionality

The ability to reuse design content not only saves time but also means that a set of proven circuitry blocks can be created, which helps reduce component inventory and frees up your design team to focus on the development of new concepts and products. To extend the existing concept of design snippets, new Reuse Blocks have been implemented in this release. When connected to your Altium 365 Workspace, the new content of the Reuse Block type can be created, used, and managed, as well as Workspace-based schematic and PCB snippets. The new Design Reuse panel provides access to reuse blocks and both Workspace-based and local snippets.

The Design Reuse panel

A reuse block can contain both schematic circuitry and its physical representation for the PCB. When such a reuse block is placed on a schematic sheet, its physical representation will be placed automatically during the ECO process.

New Gerber Dialog with Improved Support for PCB Panels

The Gerber Setup and Gerber X2 Setup dialogs have been replaced by the dialogs with specific options to suit each Gerber format. The new dialogs include two output naming options using either the PCB filename with a unique extension or a unique filename with a common extension.

PCB Panel Support

When Gerber or Gerber X2 output is generated for a PCB panel (an embedded board array), the new dialog includes a column for the panel as well as a column of layers for each board included in the panel. Use this new column to quickly verify that the various board layers are mapped to the correct panel layers.

Learn more about Generating Gerber Fabrication Data.

This release includes several enhancements and improvements to the Library Migrator.

• For better reflection of the tool's purpose, its name has been changed to Library Importer.

• Along with the current ways of accessing the Library Importer (e.g., by choosing File » Library Importer from the main menus) and new ways from the Components and Explorer panels (see the section below), the Library Importer can now be launched for an installed library listed on the Installed tab of the Advanced File-based Libraries dialog. When the library to be imported is selected in the dialog, click the Import control in the dialog's grid section.

  

  Also, the Library Importer can be launched for an integrated library when opening it.

  

• You can now easily access the Properties panel from the Library Importer by clicking  near the top and in the SOURCE LIBRARIES region.

  

• New component categories to be created during the import process and the Uncategorized entry are now labeled with  and  icons.

  

• Default values have been added for library splitting.

  

• Validation now checks for empty Workspace folder paths, conflicting system parameters, and duplicate models.

UI Improved for Components in Workspaces  

For a quicker start of work with a Workspace Library, additional controls have been added to the Components and Explorer panels.

At the first launch of the Components panel in the current Altium Designer session, the following controls are available when connected to a Workspace:

• Use Existing Components – click to browse the component type currently selected in the panel's top drop-down.
• Delete Existing Components – click to open the Delete Existing Components dialog followed by the Data Cleanup page of your Workspace's Settings where you can select the content types to be removed.
• Import Library – click to open the standard Windows Open dialog then select a database or file-based library saved on your local or network folder. After opening a library file, the Library Importer in its Simple mode will launch with the selected library loaded.
• Create Component – click to open the Create New Component dialog followed by the Component Editor in Single Component Editing mode ready to define a new component.

When in offline mode, a warning will be shown in the panel along with controls to keep using the cached component data or to clear the cache.

Creating a new component. existing library import, as well as library cleanup, can also be launched now from the Component panel's  menu.

In the Explorer panel, when a folder of the Components type has no components in it yet, a number of controls are now presented to assist you in populating the folder with components. Use these controls to perform an appropriate action:

• Import Library – click to open the standard Windows Open dialog then select a database or file-based library saved on your local or network folder. After opening a library file, the Library Importer in its Simple mode will launch with the selected library loaded.
• Create Component – click to open the Component Editor in Single Component Editing mode ready to define a new component.
• Create Other Item Type – click to open the Create New Item dialog and create a new item of any type.

Regardless of whether or not there are components in the folder, these actions can also be performed using the options of the menu associated with the Add Component drop-down at the top-right of the panel.

Draftsman Improvements

Different Drill Symbol Sizes for Drill Drawing Views and Drill Tables

The drill symbol size was previously linked between the Drill Drawing View and the Drill Table. With this release, you can set the drill symbol with one size on a Drill Drawing View and a different size on the Drill Table. You can set the desired size defaults on the Drill Symbol tab of the Draftsman - Defaults page of the Preferences dialog or for a specific project in the Drill Symbols Configurations dialog as shown in the images below. Use the Symbol Size Table and Symbol Size View fields to set the drill symbol size. To set different sizes for the Drill Drawing View and Drill Table, click  to unlink the two sizes then set the desired sizes independently of each other.

Added Option for IPC-4761 Via Type

An option has been added to the Via Type mode of the Properties panel that allows you to select from what side covering should be applied. The Side option in the Properties region of the panel includes a drop-down so that you can choose the desired side. The options of the drop-down depend on the via type selected in the ViaType option in the same region of the panel.

For via types 1A, 2A, 3A, 4A, and 6A, choose from either Top or Bottom. For via types 1B, 2B, 3B, 4B, 5, 6b, and 7, the option is essentially disabled with Both as the only option and is the default for those via types.

Circuit Simulation Improvements

Added .CSV File-based Stimulus Type

The circuit simulator now supports using a CSV file to specify the Time-Value Pairs for the interpolated VPWL and IPWL voltage and current sources. Set the Source Stimulus Type to File then specify the path+filename in the File parameter (e.g., C:\Designs\Circuit Simulation\Analog Amplifier\PWL_test.csv).

Schematic Capture Improvements

Generic Components

This release introduces the concept of standard Generic Components, which can quickly be placed in a design without the need to find and choose a specific manufactured part.

Generic Components are intended as placeholders that are easily replaced by parameter-matched real-world components later in the design process. They also can be considered as virtual or parametric components.

New SheetSymbolDesignator Special String

A new SheetSymbolDesignator special string has been added as part of this release. This special string can be placed on a child schematic sheet to display the designator of the associated Sheet Symbol object that is placed on the parent schematic sheet. The SheetSymbolDesignator special string can also be used in a multi-channel design. Select a compiled tab of the child schematic sheet to display the converted value of the special string.

Use the SheetSymbolDesignator special string to show the parent sheet symbol's designator. Hover the cursor over the image to see the special string's converted value on the compiled tab of the sheet.

Updating of Alternative Components in Variants

The Tools » Update from Libraries (schematic editor) and Tools » Update Schematics (schematic library editor) commands are now functional for alternative components in variants. Running either of these commands results in updating parameters of alternate components, which are visible in the Variant Management dialog and a compiled tab of the schematic sheet.

Example of an updated alternate component from the Workspace library. Shown here is the alternate component before the update. Hover the cursor over the image to see the component after creating a new revision and updating the component using the Update from Libraries command.

Support for Negation of Power Ports

You can now negate (include a bar over the top of) a Power Port object as can be done for ports, net labels, and sheet entries. Include a backslash character after each character in the Name field in the Power Port mode of the Properties panel (e.g., V\C\C\3\), or include one backslash character at the start of the net name (e.g., \VCC3) if the Single '\' Negation option is enabled on the Schematic – Graphical Editing page of the Preferences dialog to negate a power port.

Special String Identification Labels

To assist in identifying Text String objects that are using special strings, the name of the special string can now be shown on the schematic sheet. When the new Display Name of Special String option is enabled on the Schematic – Graphical Editing page of the Preferences dialog, each special string has its name displayed as a faint superscript.

PCB Design Improvements

Enhanced UI for Via Stack Editing

To improve the usability of the Via mode of the Properties panel when editing a via stack in Top-Middle-Bottom or Full Stack mode, the user interface of the panel's Via Stack section has been changed. Basic information about the via stack on different layers of the PCB design is now available for viewing and editing in tabular form. When you click within a layer name cell, the Thermal Relief option becomes available. A custom thermal relief can be set if the Relief option is enabled.

Length Tuning Relative to a Chosen Target xSignal

Tuning and matching the route lengths within a specific tolerance is an essential ingredient for a high-speed design as it ensures that timing-critical signals arrive at their target pins at the same time. In this release, tools for specifying length matching requirements have been enhanced by implementing a feature for selecting an xSignal as a target for a Matched Lengths design rule when an xSignal class (or all xSignals of the design) is used as the rule scope. The previous behavior used the longest xSignal of the xSignal class as a target for length matching.

When an xSignal class is selected as a Matched Length design rule scope, one of its xSignals can be selected as a source target.

The xSignal selected as a target will be labeled as such in the new Margin column of the xSignals mode of the PCB panel while deviation from this target length is shown in this column for other xSignals of the selected class.

Deviation from the target length is shown in the new Margin column.

During interactive length tuning, the Interactive Length Tuning mode of the Properties panel provides the ability to switch between tuning relative to the selected target xSignal (the new behavior) or the longest net in the xSignal class scoped by the rule (the previous behavior).

Select a desired mode for the tuning target during interactive length tuning.

Preventing Modification of PCB Component Primitives

If a PCB component has its primitives locked (the Primitives option in the Component mode of the Properties panel is in its  state), most properties of these primitives can no longer be modified by graphical (e.g., using drag-and-drop) and non-graphical (e.g., using the Properties or List panel) editing methods. This will help to prevent occasional changes of component primitives that can result in incorrect assembly and fabrication outputs.

By way of an example, the Pad mode of the Properties panel is shown in the image below for a pad that is a constituent part of a PCB component that has its primitives locked. Note that all properties of the pad (except for Net and Testpoint properties) are dimmed and not available for editing. Note also that the  icon is shown at the far right of the pad's Component field, which denotes that the parent component has its primitives locked, and pad properties cannot be modified.

The Pad mode of the Properties panel (on the left) for a pad of a PCB component that has its primitives locked (on the right).

Print Not Fitted Components

When this feature is enabled, copper shapes and solder masks for not fitted components are displayed in PCB printouts even if their variant(s) is/are set as Not Fitted. 

Circuit Simulation Improvements

Improved Performance

The speed of the simulation process has been increased when running analyses. Also, when using the Components panel for browsing large simulation model libraries, the speed to upload the content of such libraries has been improved.

Simulation Model Caching

Simulation models used in a project are cached now in the project, so simulation of such projects can be easily run on different machines.

Schematic Capture Improvements

Sheet Symbol Indexing Enhancement

Any digit or number may be used as the first or last index of a repeated Sheet Symbol, including 0. Negative numbers are not allowed. The last index must always be larger than the first index.

Component Class Enhancement

Use this new feature to add the new class Component Class Name to set parameters for components within a blanket by means of the Parameter Set mode of the Properties panel.

Associating the Component Class Name to a component (or group of components) will result in sending the information about the component class, its name and members to the PCB as is done currently for Net Classes.

Added Graphical Pull Up/Down Resistors Symbol

Added the ability to mark a pin as containing internal pull-up or pull-down resistors. Choose Internal Pull Up/Down from the Inside drop-down in the Symbols region of the Pin mode of the Properties panel.

The new graphical symbol will be displayed next to the pin as sown in the images below. The left image is the new Internal Pull Up graphical symbol; the right image is the new Internal Pull Down  symbol.

Calculate Formulas and Resolve Special Strings in Text Frames and Notes

Many designers use the special string capabilities available in Altium Designer to create complex strings that display important information on the schematic sheets. Special string support has been added to Text Frames and Notes, allowing you to create complex special string definitions as a single, multi-line text object.

Altium Designer supports resolving numerical calculations defined in a Text String, with support for resolving numerical calculations extended to include those defined in schematic Text Frames and Notes.

When this feature originally entered into closed beta (as indicated above), the special string or formula had to be enclosed in curly brackets. With this release, special strings and formulas are now delineated by opening with the "=" character and closing with a space character.

Special strings and formulas can be evaluated inside a Text Frame or a Note by using the "=" character.

Remember the Last Selected Variant for a Project

The last variant that was set prior to closing a project is now remembered and will be the variant presented when the project is reopened. Previously, the base design ([No Variation]) was always presented when the project was reopened.

PCB Design Improvements

CounterHoles Improvements

A number of improvements have been applied to the Counterholes functionality that was implemented in previous releases.

• Counterholes are now grouped in Counterholes Top and Counterholes Bottom layer pairs in the Hole Size Editor mode of the PCB panel and in the Drill Table mode of the Properties panel.

   
  The Counterholes Top and Counterholes Bottom groups in the Hole Size Editor mode of the PCB panel (the first image) and in the Drill Table mode of the Properties panel (the second image).

  Note that counterholes are excluded from other layer pairs of a drill table, including All Layer Pairs (Composite table) and All Layer Pairs (Separate tables).

• New Counterhole Depth and Counterhole Angle columns are added to the Hole Size Editor mode of the PCB panel and the Drill Table.

  
  Enabling the Counterhole Depth and Counterhole Angle columns in the Hole Size Editor mode of the PCB panel.

  
  Enabling the Counterhole Depth and Counterhole Angle columns for a Drill Table from the Columns dialog.

• For NC Drill, Gerber, Gerber X2, and ODB++ outputs, files for all top and all bottom counterholes are now generated instead of separate files for each counterhole type.

  
  Example of Counterholes Top and Counterholes Bottom file options in the Gerber X2 Setup and ODB++ Setup dialogs.

• If the size of the counterhole is larger than or equal to the pad size, the pad shape is removed from the corresponding side of the PCB (since this pad shape will be drilled out when drilling the counterhole).

  
  Example of a removed pad shape from the top layer.

Access to the Advanced Rigid-Flex Mode

Previous releases include significant improvements to the process of working with Rigid-Flex board designs in Altium Designer. These improvements include new Board Region and Bending Line behaviors when working in Board Planning Mode in the PCB editor, and the introduction of the Board mode in the Layer Stack Manager. This new feature set is referred to as Rigid-Flex 2.0.

In this release, to enable the Rigid-Flex 2.0 functionality for the current PCB design, select the Design » Layer Stack Manager command from the main menus to open the Layer Stack Manager then select Rigid/Flex (Advanced) from the Tools » Features sub-menu or the  button menu.

Enable the Advanced Rigid-Flex mode to configure a Rigid-Flex board; either via the Tools menu or by clicking the features button (hover the cursor over the image to show this).

To enable the Rigid-Flex 1.0 mode, select Rigid/Flex from the same menus.

Note that when trying to disable the Rigid-Flex 2.0 mode or switch to the Rigid-Flex 1.0 mode for a PCB that already uses Rigid-Flex 2.0 features, the warning dialog will open for confirmation.

Added 'Apply to Polygon Pour' Option to Creepage Distance Rule

The Apply to Polygon Pour option has been added to the Creepage Distance design rule. When the option is enabled, the rule tests the creepage distance between scoped polygons and other objects.

The new Apply to Polygon Pour option of the Creepage Distance rule.

If a polygon pour and other objects are scoped by a Creepage Distance design rule with the Apply to Polygon Pour option enabled and a Clearance design rule, both rules are considered and the tightest set of constraints is applied when pouring the polygon. For example, if the Creepage Distance rule has a larger constraint value than the Clearance rule, this larger value will be applied.

Data Management Improvements (22.2)

Draftsman Improvements

New Option to Remove Leading Zeros

Dimensioning and Tolerancing, ASME Y14.5, specifies that for values less than 1, leading zeros should be omitted when using inch units (for example, ".5" versus "0.5"). The Remove Leading Zero option has been added to the Document Options mode of the Properties panel that allows you to automatically remove the leading zero for mil and inch values. This option is disabled by default.

The Remove Leading Zero option on the Document Options mode of the Properties panel

Additional Default Values for Drill Table

Default values of some additional properties of the Draftsman's Drill Table object can now be defined on the Draftsman - Defaults page of the Preferences dialog. The new settings, including Symbol Size, Symbol Line Style, and Grouping, can be found on the Drill Symbol tab of the page when Drill Table is selected in the Primitive List.

Default settings for some additional options of Draftsman's Drill Table can now be defined on the Drill Symbols tab of the Preferences Draftsman - Default page.

Importer/Exporter Improvements

Support for Importing Design Variants from xDxDesigner Projects

The xDxDesigner Importer has been enhanced to allow importing an xDxDesigner project to also import defined variants of that project automatically. To import xDxDesigner project variants, the following steps should be performed:

1. Using Variant Manager in xDxDesigner, export variants via Report » Delimited Text Document.
2. Make sure that Unplaced is defined as the Unplaced keyword in the Settings dialog.
3. Save the variant file as ProjectVariants.txt in the same location as the .prj project file to be imported in Altium Designer.
4. Run xDxDesigner import from the Import Wizard (File » Import Wizard) and point the xDxDesigner project file (.prj) – design variants will be imported automatically.

Circuit Simulation Improvements

Sensitivity Analysis Enhancements

This release brings further improvements to the Sensitivity Analysis tool. Group Deviations of Global parameters as a sensitivity parameter are now supported, and Temperature as a sensitivity parameter is also now supported.

The Global Parameter option has been added to the Sensitivity analysis Group Deviations options; hover the cursor over the image to show where the parameters are defined.

Schematic Capture Improvement

Further Enhancements to Sheet Cross-referencing

Adding cross-references to the project allows you to easily follow the connective flow of nets between the schematic sheets in a project. In this release, the support of cross-references has been extended by adding the Jump to commands for Sheet Entry and Off Sheet Connector objects.

When cross-references are enabled for sheet entries on the Options tab of the Project Options dialog, use the Sheet Entry Actions right-click menu of a sheet entry to Jump to the matching port on the child schematic sheet.

Use the Jump to command to jump to the matching port.

For a flat design, when cross-references are enabled for off-sheet connectors in the Project Options dialog, use the Off Sheet Actions right-click menu of an off-sheet connector to Jump to a matching off sheet connector on a related schematic sheet.

Use the Jump to command to jump to a matching off-sheet connector.

PCB Design Improvements

Keepout Visibility in Embedded Board Arrays

Keepout objects placed in a PCB design can now be shown in a panelized embedded board array using the PCB as a source. Enable visibility of the Keepout layer on the Layers tab of the Properties panel when an Embedded Board Array is selected in the design space.

The Keepout layer of the source PCB can now be shown in the Embedded Board Array.

Note that this feature only provides a visual representation of the Keepout layer. Currently, copper objects will not respect keepouts from the source PCB when placed on the Embedded Board Array.

Ability to Change PCB Cursor Color

The Cursor Color option has been added to the PCB Editor - General page of the Preferences dialog that allows you to change the color of the crosshair cursor in the PCB editor. This gives you the freedom to customize the color in order to distinguish the cursor from grids, etc. Click the color box associated with the new option to open the Choose Color dialog, then select the desired new color for the cursor.

Enhanced UI for Pad Stack Editing

To improve the usability of the Pad mode of the Properties panel when editing a pad stack in Top-Middle-Bottom or Full Stack mode, the user interface of the panel's Pad Stack section has been changed. Basic information about the pad stack on different layers of the PCB design is now available for viewing and editing in tabular form. When clicking within a layer name cell, additional options become available for this layer: Corner Radius (for Rectangular shape) and Thermal Relief (shows the current parameters of the pad's thermal relief; custom thermal relief can be set if the Relief option is enabled).

 
The updated Pad Stack section of Pad properties when editing a pad stack in Top-Middle-Bottom (the first image) or Full Stack (the second image) mode with the Top layer options expanded.

Data Management Improvements

Ability to Control Visibility of Components and Nets Folders in the Projects Panel

Upon validation of a PCB design project, the Components and Nets folders that list the project's components and nets are displayed in the Projects panel. To manage the visibility of these folders, the Show Components and Nets folders option has been added to the Settings pop-up of the Projects panel (appears when the  icon is clicked at the top of the panel) and the General region of the System – Projects Panel page of the Preferences dialog. This option is enabled by default.

The Show Components and Nets folders option in the Projects panel setting pop-up.

The Show Components and Nets folders option on the System – Projects Panel page of the Preferences dialog.

Circuit Simulation Improvement (22.1)

Sensitivity Analysis

Sensitivity Analysis provides a way of determining which circuit components or factors have the most influence on the output characteristics of a circuit. With this information, you can reduce the influence of negative characteristics, or alternatively, enhance the circuit performance based on positive characteristics. Sensitivity Analysis calculates sensitivities as numeric values of given measurements related to components/model parameters of circuit components, as well as sensitivity to temperature/global parameters. The result of the analysis is a table of the ranged values of sensitivities for each measurement type.

In this release, a new Sensitivity option has been added to the Analysis Setup & Run region of the Simulation Dashboard. Once it has been enabled, the Sensitivity properties can be configured in the Advanced Analysis Settings dialog, as shown below.

Draftsman Improvement

New Via Type View

The Via Type View object has been added to Draftsman documents. The object allows the illustration of a via type according to the IPC-4761 standard, Design Guide for Protection of Printed Board Via Structures. A Via Type View can be placed by choosing Place » Additional Views » Via Type View from the main menus. The view will display in the document. Select the view to access its properties.

Schematic Capture Improvements

Cross-Selection for Sheet Entries and PDF Outputs

Adding cross-references to the project allows you to easily follow the connective flow of nets between the schematic sheets in a project. In this release, the support for automatically creating and updating cross-references has been extended for the Sheet Entry objects.

Enable the Automatic Cross References and Sheet Entries options on the Options tab of the Project Options dialog. Sheet Entries will be tagged with sheet and location coordinates of the corresponding port object on the child schematic sheet.

Enable the Automatic Cross References and Sheet Entries options in project options for tagging sheet entries with cross reference values.

Cross references are enabled for sheet entries.

Cross Reference values are also displayed in the Sheet Entry mode of the Properties panel, which simplifies the task of identifying the Cross Reference that is being applied to the selected Sheet Entry.

Cross References can be explored in the Properties panel of the selected sheet entry.

Support of cross references has also been extended in schematic PDF outputs. If an object is related to more than one connected object (e.g., a port is connected to a sheet entry on the parent schematic sheets and ports on other sheets), clicking the object in the PDF output will show the list of sheets where the connected objects reside. Select a list item to open the corresponding page.

In the schematic PDF output, multiple connected objects can be easily navigated using the pop-up menu.

PCB Design Improvements

New 'Gloss And Retrace' Panel and Preferences Page

To give you greater control over the glossing process, a new Gloss And Retrace panel has been introduced for configuring options for the Route » Gloss Selected and Route » Retrace Selected commands. This new panel can be used to set the gloss and retrace parameters that work best for the selected routing that you are currently glossing or retracing in your design.

The panel can be used to control the following Gloss and Retrace Parameters:

• Avoid polygons – when this option is enabled, existing polygons will be respected when the Gloss Selected or Retrace Selected command is run. If the option is disabled (as it was in previous versions), existing polygons will be ignored, affected polygons can then be repoured.
• Avoid rooms – when this option is enabled (as it was in previous versions), existing rooms will be respected when the Gloss Selected or Retrace Selected command is run. If a room scoped by specific routing width requirements is defined in the design and the routing to be glossed/retraced does not cross the room, the resulting routing will not cross this room either when the option is enabled. If the option is disabled, existing rooms will be routed across, and the width to be used within such rooms will be that as defined in the constraints of the room-based rule.

For the following two options, you can choose between the Min, Max, or Preferred value of the corresponding rule. Choose Current to leave the existing width or gap unchanged, or type in a new value.

• Set Width - previously, this was always configured as preferred. You can now use the drop-down to select the width to be applied when the Retrace Selected command is run.
• Set Diff Pair Gap - previously, this was always configured as preferred. You can use the drop-down to select the differential pair gap setting to be applied when the Retrace Selected command is run.

The Gloss and Retrace settings also can be configured in the new PCB Editor - Gloss And Retrace page of the Preferences dialog. Whenever a change is made in the panel or Preferences dialog, it is reflected in the other. The installation defaults are preset to match earlier versions.

IPC-4761 Support 

The IPC-4761 standard, Design Guide for Protection of Printed Board Via Structures, provides information regarding methods for protecting vias on PCBs. You can now select the via type to ensure it is protected according to the IPC standard. Use the new IPC 4761 Via Type drop-down in the Via Types & Features region of the Via mode of the Properties panel or the Via Template Editor to select.

Additionally, when a via that has the via type set to IPC-4761 in its properties is placed in a PCB design, new types of mechanical layers and component layer pairs are automatically added to the design, with corresponding shapes on these layers.

The IPC-4761 via type mechanical layers are automatically added to the design. The Top Tenting layer is shown on the design space by way of example.

New layers are available for the following outputs:

• PCB printouts
• Gerber and Gerber X2
• ODB++
• IPC-2581

The PCB/PCBLIB List panels also now include a column titled IPC 4761 Via Type and you can add columns to a Drill Table object (titled Via Feature and Via Type) that display the IPC 4761 supported via type.

Automatic Update of Designators in Design Rules

Changes made to PCB component designators did not previously update custom, designator-specific design rules. They had to be updated manually. Enabling this new feature changes references in design rules when PCB component designators are: reannotated; updated by an ECO; or manually edited on the board.

Pad Entry and Exit Enhancements

Because of their small physical dimensions, routing in and out of surface mount devices is often dense and complex. In previous versions of the software, if the SMD rules could not be observed, for example, the required 'distance to corner' was not available; the router would fail to place any track segments (as shown in the video below). To improve the pad entry and exit behavior, the following improvements are available:

• Once the pad has been exited, the route is kept away from the pad. The software no longer allows the route to re-enter the pad and then re-exit without regard to the SMD rules.
• SMD rules are ignored if the pad exit is blocked (they are already ignored during pad entry in this situation). Note that if there is a pad exit available that does not violate the SMD to corner rule, that exit will be used.
• Miters are no longer created in violation of SMD rules. The software favors the SMD to corner rule over the miter, allowing the miter to collapse to zero if required.
• Stubs that follow the SMD rules are now created in Any Angle routing mode. In this mode, once the first track segment has been placed arcs will be included in the corners. If you need an arc in the first corner, place the exit stub before attempting to create a corner.

Support for Counterholes

Counterholes in the laminate allow room for screw heads. Countersink and counterbore holes are two types of counterholes that allow for different types of screws. This release introduces the ability to choose counterbore or countersink holes. The key difference between countersink and counterbore screws is the size and shape of the holes; counterbore holes are wider and more square to allow for the addition of washers. Countersink holes create a conical hole matching the angled shape on the underside of a flat-head screw. A countersink is a cone-shaped hole cut into the laminate. It is typically used to allow the tapered head of a screw to sit flush with the top of the laminate. By comparison, a counterbore makes a flat-bottomed hole and its sides are drilled straight down. This is usually used to fit a hex-headed cap or screw. Only one countersink or counterbore hole per pad is allowed.

Use the new options in the Pad mode of the Properties panel to choose the type of counterhole desired. A dashed line appears around the pad in 2D to define the counter hole contour on the active layer as shown in the images below. The positioning of the dashed lines is different for Top Side and Bottom Side as seen in the images. Counterholes are supported in 2D, 3D, and in Draftsman.

The counterholes display as Layers Pairs in the Properties panel modes of the Drill Table mode of the Properties panel and the Hole Size Editor mode of the PCB panel as shown below.

Data Management Improvements

Added Virtual BOM Item to the Project

A 'virtual' BOM item is added to the project in the Projects panel if there is at least one component in the project. You can open, save or remove the BOM item. The basic flow of BOM generation will not be impacted by the virtual BOM item. Click +Add ActiveBOM in the panel to open the virtual BOM in preview mode. Once the new *.BomDoc has been saved it will become a standard project document. If the virtual BOM is not required, right-click in the Projects panel then select Remove from Project. 

Show 'Detached' Comments

When a project document is removed or its UniqueID has changed, the comments for the document can become "detached". Those comments can still be accessed from the Comments panel's Detached Comments collapsible region. Click on a detached comment's tile in the panel to show the comment in the design space of the currently opened document. You can restore a comment by selecting it then clicking the mouse.

Added Ability to Override Part Numbers for Ansys EDB Exports

An 'Override Part Number With' option was added to the Ansys EDB Export Options dialog. This new option allows you to specify which parameter should be used as a Local Part Name rather than using 'Comment' by default. Enable the option then use the associated drop-down to select the desired parameter.

Circuit Simulation Improvements

Calculate and Review Simulation Measurement Results

A focus for this release is a number of improvements in the ability to analyze simulation measurement results. Along with additional measurement types, a number of new measurement-based features have been added. These include:

• Additional measurement types - new measurement Types have been added to the list of available measurements.
• Measurement Statistics - measurement statistics are calculated automatically and displayed in the lower region of the Sim Data panel.
• Display measurement results in a table - a full table of the measurement results can be displayed in the main SDF window by clicking the Expand the table link. Data in the table can be selected and copied to a spreadsheet.
• Display Histogram - visualize the distribution of data by generating a histogram directly from the measurement results. Hover the cursor over the image below to display a histogram of the Monte Carlo analysis results.
• Derive plot from measurements - generate a plot of one variable against another. For example, if a parametric sweep has been performed where two component values have been swept, these can be plotted against each other.
• Show on Chart - click the button in the Measurements tab of the Sim Data panel. The measurement cursors will display on the chart, highlighting the region of the chart that the measurement has been calculated over.
• Add new measurement - click the Add button in the Sim Data panel to open the Add Waves to Plot dialog where a new measurement can be defined.
• Edit existing measurement - click the Edit button to edit the currently selected measurement; no need to return to the Simulation Dashboard panel.

The Show on chart feature displays the measurement cursors where that measurement was calculated. Hover the cursor over the image to show a Histogram of the measurement results.

Draftsman Improvements

Added Counter Hole Support

The Counter Hole View object has been added to Draftsman documents. A Counter Hole View can be placed by choosing Place » Additional Views » Counter Hole View from the main menus. The view will display in the document. Select the view to access and view and edit the properties.