PCB Design Improvements
Single Layer PCB Support (Open Beta)
This release adds the ability to create a single-layer PCB, with corresponding support in the Layer Stack Manager, PCB and Draftsman documents, and generated outputs.
With this support, you can now delete either the top or bottom layer from a 2-layer stack in the Layer Stack Manager.
In a 2-layer PCB, you can now delete either the Top or Bottom Layer from its layer stack.
A single-layer stack can be created for a PCB but not a footprint.
When the layer stack has a single copper layer, the Via Types tab and the Back Drills feature will not be available in the Layer Stack Manager. Also, you can only create impedance profiles of Single-Coplanar and Differential-Coplanar types on the Impedance tab of the Layer Stack Manager for a single-layer PCB.
The Tools » Presets menu now includes a preset for a single-layer stack – show image .
If a PCB has a single signal layer, it will be reflected in the PCB editor user interface (layer tabs, the board's Properties panel, and the View Configuration panel) and in the PCB's layer stack table and drill table.
The removed layer is referenced as a side where applicable. For example, if the bottom layer is removed, it is called Bottom Side
in the Drill Layer Pair column of a drill table, as shown in the image below.
A single-layer PCB is supported in a Draftsman document and in the following outputs: Gerber, Gerber X2, ODB++, IPC-2581, Pick and Place, NC Drill, Layer Stack Report, and PCB prints.
When there are unplated thru-hole pads in a single-layer PCB, they will not be flagged in the Unplated multi-layer pad(s) detected section of the DRC report .
This feature is in Open Beta and available when the PCB.SingleLayerStack.Support
option is enabled in the Advanced Settings dialog .
For more information, refer to the Defining the Layer Stack page.
Predefined Donut Pad Shapes (Open Beta)
A predefined round Donut shape has been added to the listing of pad shapes available when defining the padstack. Use the Shape drop-down in the Properties panel to apply the Donut shape to a pad. The round Donut shape is represented as a full circle arc and is supported in the PCB List panel, Find Similar Objects dialog, and when using expressions. They are also supported on Paste/Solder Mask layers, and also when defining thermal relief connection points to a polygon pour.
The outer diameter of the round Donut pad shape is represented by D and the width is represented by W in the Properties panel, as shown in the above image highlighted in purple. Click in the respective cell to change the values.
Round Donut pad shapes are supported in ODB++, Gerber, Gerber X2, PCB prints, IPC-2581, and DXF/DWG outputs, and in PCB CoDesigner when comparing PCB documents. Also, round Donut pads are supported when importing an Xpedition design/library.
When defining a pad template, automated naming is applied in accordance with the IPC-7351 standard.
When opening a PCB using Donut-shaped pads in a previous version of the software, the information will be lost. In fact, the Donut shape will simply be converted into a series of arcs.
This feature is in Open Beta and available when the PCB.Pad.CustomShape.Donut
option is enabled in the Advanced Settings dialog .
For more information, refer to the Working with Pads & Vias page.
Routing Neck-down Rule (Open Beta)
This release implements a new routing neck-down design rule to assist you with routing in dense areas of a board.
With modern component technology, it is not uncommon for a net to be routed at different widths as the routing travels across the board. For example, routing into or out of a BGA will often require escape routes narrower than the preferred width routes allowed by the applied impedance profile. The new rule lets you define the maximum allowed total length of such narrower traces so that the route still delivers the required impedance.
The Routing Neck-Down rule can be defined in both the Physical view of the Constraint Manager and the PCB Rules and Constraints Editor dialog. Use the Neck-Down Length field to define the maximum allowed length of continuous routes (in each net scoped by the rule) whose width is between the Min Width and Preferred Width defined by the applicable Routing Width rule.
Min Width ≤ Actual Neck-down Width < Preferred Width
Alternatively, use the grid to define the allowed length per layer basis.
Enable the Routing Neck-Down rule type check for online and/or batch checking in the Design Rule Checker dialog to detect violations of the Routing Neck-Down rules in corresponding DRC modes. Detected rule violations will be marked with a hatched pattern on corresponding traces in the design space.
This feature is in Open Beta and available when the PCB.Rules.RoutingNeckdown
option is enabled in the Advanced Settings dialog .
For more information, refer to the Routing Rule Types page.
Routing Auto-shrinking (Open Beta)
In cases when a trace being routed using the interactive router cannot be routed between obstacles with the currently chosen routing width, this new feature allows to automatically shrink the width to a value that would allow routing of the trace in this location (provided that this shrunk trace would not violate the minimum allowed width from the corresponding constraint). Enable the Auto Shrinking option on the PCB Editor – Interactive Routing page of the Preferences dialog and the Properties panel during interactive routing to enable the feature.
This feature is in Open Beta and available when the PCB.Routing.EnableAutoShrinking
option is enabled in the Advanced Settings dialog .
For more information, refer to the Interactive Routing page.
Trace Centering (Open Beta)
A common desire of many designers is to center the routes when they pass between pads or vias whenever possible. The current behavior of the routing engine is to place track segments at the minimum allowed clearance defined in the design rules, leaving the task of spreading or centering the routes between the pads.
The new centering feature helps with the centering process by adding an additional clearance between the net being routed or dragged and existing pads/vias. The routing engine understands that this additional clearance is desired rather than required, so it can take some or all of it back if needed, for example, when pushing a second or third route between the existing pads/vias. If the routing engine is required to take back some of the clearance, it will take it from both sides of the routing so that it remains centered where possible.
The trace centering behavior can be configured using the new options available on the PCB Editor – Interactive Routing page of the Preferences dialog and the Properties panel during interactive routing , interactive differential pair routing or interactive sliding .
Apply Trace Centering – enables the trace centering functionality. When enabled, the following options are available to configure the functionality:
Adjust Vias – when the option is enabled, vias will be pushed to maintain the additional clearance where possible.
To prevent vias from being pushed by trace centering, you can either:
disable the Adjust Vias option. In this case, centering will not be applied between unlocked vias or
disable the Allow Via Pushing option. In this case, vias will not be pushed (even to ensure the minimum clearance from the Clearance constraint).
Added Clearance Ratio – a multiplier of the applicable clearance, which is then added to the clearance. For example, if the applicable clearance is 0.15mm
, setting the option to 2 would instruct the routing engine to clear existing pads and vias by 0.15 + 2*0.15 = 0.45mm
whenever possible. The routing engine can then reduce this clearance down to the specified clearance if required.
Disable Trace Centering When Dragging – when the option is enabled, trace centering is not applied during interactive sliding (even if the Apply Trace Centering option is enabled).
The trace centering options in the Preferences dialog
The trace centering options in the Properties panel
Additional clearance can be added around pads and vias to center the routes.
This feature is available in all routing modes, including Any Angle.
This feature is in Open Beta and available when the PCB.EnableTraceCentering
option is enabled in the Advanced Settings dialog .
For more information, refer to the Interactive Routing page.
True Zero Mitering (Open Beta)
During interactive routing, interactive differential pair routing or interactive sliding, a miter is now not created if the Miter Ratio value is set to 0
(in the corresponding Properties panel or in the PCB Editor – Interactive Routing page of the Preferences dialog), which allows you to create acute corners. In previous versions, a short miter fully covered by adjacent traces was created when Miter Ratio = 0
.
An example of a zero-miter joint between tracks during interactive routing.
This feature is in Open Beta and available when the PCB.ZeroMitersRemoving
option is enabled in the Advanced Settings dialog .
For more information, refer to the Interactive Routing page.
Constraint Manager Improvements
Modifying Directives Imported from Read-only Documents
Directives that have been imported from read-only documents (for example, device sheets and managed sheets) cannot be modified if the Make Device Sheets In Projects Read-Only option is enabled (checked) on the Data Management - Device Sheets page of the Preferences dialog. When the option is disabled (unchecked), the directives can be modified.
After directives have been imported (with the option enabled), the rule is highlighted in blue in the Constraint Manager.
For more information, refer to the Defining Design Requirements Using the Constraint Manager page.
Ability to Enable/Disable Advanced Rules
You can now enable/disable advanced rules that are defined in the All Rules view when the Constraint Manager is accessed from a PCB.
A new Enabled column is now included in the view. The column reflects the state of each advanced rule: True (enabled) or False (disabled). Double-click a cell in the column and toggle the state of a specific advanced rule. Alternatively, toggle the enabled state of advanced rules of a particular type, category, or all advanced rules using commands available from the right-click context menu for the corresponding entry in the Rule Class tree.
❯ ❮
1
Javascript ID: CM_EnableDisableAdvancedRules_AD24_8
The Enabled column reflects the state of each advanced rule.
Double-click a cell in the Enabled column to toggle the state of a specific advanced rule.
Right-click a rule type entry in the Rule Class tree to enable/disable advanced rules of this type.
Right-click a rule category entry in the Rule Class tree to enable/disable advanced rules in this category.
Right-click the Rule Class heading to enable/disable all advanced rules.
For more information, refer to the Defining Design Requirements Using the Constraint Manager page.
When accessing the Constraint Manager from the schematic, it is now possible to configure the Width and Differential Pairs Routing constraints for layers in a chosen layer stack.
Using a new drop-down at the top of the Constraint Manager, select an entry for a specific PCB document of the design project. If the selected PCB contains multiple layer stacks, you can choose the required stack for which constraints need to be configured using tabs in the lower part of the Constraint Manager when the corresponding rule is selected. Also, you can use a chosen Impedance Profile (where defined as part of the selected PCB’s layer stack).
For more information, refer to the Defining Design Requirements Using the Constraint Manager page.
Import/Export Constraints between Designs
Added the ability to export and import constraints between designs. To access this new feature, right-click in the Clearances , Physical , or Electrical view of the Constraint Manager, then select Export » Export Constraints for selected lines or Import » Import Constraints .
Exporting Constraints
After selecting one or more cells in the Clearances view or one or more lines in the Physical or Electrical view and then choosing Export » Export Constraints for selected lines , the Constraints for Export dialog opens with constraints for all objects that have been selected prior to choosing the command listed in the grid. Select the constraints you want to export using checkboxes (constraints related to the current view will be selected in the dialog by default). After clicking OK , the selected constraints will be exported into a file with the extension *.CstrDot
. The file can then be imported into another design.
Importing Constraints
After selecting Import » Import Constraints , the standard File Explorer dialog opens in which you can select a *.CstrDot
file to import. In the Constraints for Import dialog that opens, select the constraints you want to import from the file, then click OK . The selected constraints will be applied to corresponding objects in the target design.
If a net selected for import does not exist in the target design, an entry for it will be added to the Constraint Manager. Since there is no such net in the design, the entry will be marked with the icon. Constraint values can be copied from this entry and pasted into an existing object. The issue can be resolved by adding a net with the same net to the design and then refreshing the data in the Constraint Manager. Alternatively, an unmatched object can be removed from the Constraint Manager by right-clicking its entry and selecting Delete unmatched object – show image .
If a diff pair or xNet selected for import does not exist in the target design, it will not be added to the design.
If a net / diff pair / xNet class selected for import does not exist in the target design, it will be added to the design automatically.
For more information, refer to the Defining Design Requirements Using the Constraint Manager page.
3D-MID Design Improvements
Ability to Drag Multiple Components
In a 3D-MID document, you can now drag more than one component. Select multiple components (using the Shift+Click shortcut or other selection methods), then use Click, Hold&Drag on the selection to move all selected components at once.
For more information, refer to the 3D-MID Design page.
Displaying the 3D Substrate File Name
The name of (and full path to) the 3D substrate file is now presented in the Properties panel. When no object is selected in the 3D-MID document, open the panel's Parameters tab and locate the Pcb 3d Substrate File Name parameter.
The Pcb 3d Substrate File Name parameter value will be updated if you change the 3D substrate using the File » Change Substrate command from the main menus. Note that it will not be updated if the 3D substrate file is renamed (e.g., through the Windows File Explorer ).
For more information, refer to the 3D-MID Design page.
Harness Design Improvements
The ability to add comments to a Draftsman document (*.HarDwf
) has been added. Comments, which are notes a user adds, can be applied to a point, object, or area and can be replied to by other users. Placement can be done using the Place menu, the right-click context menu, the icon at the top right of the design space, or the Ctrl+Alt+C shortcut keys. A comment placed in a Draftsman document is shown in the image below.
For more information, refer to the Document Commenting page.
Layout Label Text Display in BOM
This release adds the ability to display the text value for a layout label in the BOM. Enable the Label Text column in the ActiveBOM document or the BOM table placed in a Draftsman document to display the layout label text. Note that a layout label is shown in the BOM when its Type is set to Standard
.
❯ ❮
1
Javascript ID: HD_LayoutLabelTextBOM_AD24_8
The Type property of layout labels on the Layout Drawing is set to Standard
.
In the ActiveBOM document, use the Properties panel to enable visibility of the Label Text column for the BOM.
In the Draftsman document, use the Properties panel to enable visibility of the Label Text column for the BOM table when it is selected.
For more information, refer to the Creating the Layout Drawing page.
Support for Strip Length and Pull Off Length for Crimp-type Cavities
You can now specify the Strip Length and Pull Off Length when defining a crimp-type cavity in the Wiring Diagram (*.WirDoc
).
Both properties are included in the wiring list and connection table objects in a Draftsman document (*.HarDwf
) with column headings as follows:
For a wiring list:
FromCrimpStripLength
FromCrimpPullOffLength
ToCrimpStripLength
ToCrimpPullOffLength
For a connection table:
CrimpPullOffLength
CrimpStripLength
For more information, refer to the Defining the Wiring Diagram page.
Switching to .NET 6
With this release, Altium Designer switches from using .NET Framework 4.8 to .NET 6. The main reason for the switch is that Microsoft considers the .NET Framework obsolete. Although Microsoft will continue to support it for many years, it will not add any new functionality or features. All new developments and features happen in the .NET Core family that .NET 6 is part of. As a result, the switch is necessary at some point.
Additionally, .NET 6 is much faster than .NET Framework. In our tests, schematic and Draftsman showed great improvements. Many other areas, such as BOM, compilation, and library creation, show smaller improvements.
Lastly, we do not need to install any .NET Framework; we can bundle .NET 6 with Altium Designer. This will remove the issues caused by installing the .NET Framework and when Windows updates interfered.
Any Third Party extensions that were found to be incompatible with .NET 6 have been removed from the software, starting at this release. If later, updated versions of these extensions are made to be compatible with Altium Designer 24.8 (or beyond), contact beta.program@altium.com to get them added back to the installation.
For more information, refer to the System Requirements page.
Data Management Improvements
New 'Number of Pads Exceeds Number of Pins' Check for Components
Added the new Number of Pads exceeds Number of Pins violation type as part of the validation checks that can be configured for a Workspace component. A violation of this type occurs when the number of pads (SMD pads placed on copper layers and plated thru-hole pads) in a footprint model assigned to a component being validated exceeds the number of pins in the component's schematic symbol model.
In this example, two violations appear for a component – one for each footprint where the number of pads exceeds the number of schematic symbol pins.
The default mode of the Number of Pads exceeds Number of Pins violation is Error . If required, it can be configured on the Data Management – Component Rule Checks page of the Preferences dialog.
For more information, refer to the Validating a Component page.
Support for Item ID Matching to an External DB Parameter
A database parameter can now be mapped to a Workspace component's Item ID for a database component synchronization process. Use the Parameter Mapping region of the Properties panel when the required table is selected in the CmpSync document to map the ID parameter to a source database parameter.
For more information, refer to the Component Database to Workspace Data Synchronization page.
Feature Made Fully Public in Altium Designer 24.8
The following feature is now officially Public with this release: