Defining the Layer Stack

Note

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

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

The PCB is designed and formed as a stack of layers. In the early days of printed circuit board (PCB) manufacturing, the board was simply an insulating core layer clad with a thin layer of copper on one or both sides. Connections are formed in the copper layer(s) as conductive traces by etching away (removing) unwanted copper.

Fast forward to today, where almost all PCB designs have multiple copper layers. Technological innovation and refinements in processing technology have led to a number of revolutionary concepts in PCB fabrication, including the ability to design and manufacture flexible PCBs. By joining rigid sections of PCB together via flexible sections, complex, hybrid PCBs can be designed that can be folded to fit into unusually shaped enclosures.

A single-sided PCB is shown on the left, typical of early PCB design. On the right is a rigid-flex PCB, where rigid sections are connected via flexible sections of PCB.        
A single-sided PCB is shown on the left, typical of early PCB design. On the right is a rigid-flex PCB, where rigid sections are connected via flexible sections of PCB.

In printed circuit board design, the layer stack defines how the layers are arranged in the vertical direction or Z plane. Since it is fabricated as a single entity, any type of board, including a rigid-flex board, must be designed as a single entity. To achieve this, the designer must be able to define multiple PCB layer stacks, and assign different layer stacks to different regions of the rigid-flex design.

The Layer Stack Manager Copy Link Copied

The definition of the PCB layer stack is a critical element of successful printed circuit board design. No longer just a series of simple copper connections that transfer electrical energy, the routing of many modern PCBs is designed as a series of circuit elements, or transmission lines.

Achieving a successful, high-speed PCB design is a process of balancing the material selection and layer stackup and assignment against the routing dimensions and clearances required to achieve suitable single-sided and differential routing impedances. There are also numerous other design considerations that come into play when designing a modern, high-speed PCB, including layer-pairing, careful via design, possible back drilling requirements, rigid/flex requirements, copper balancing, layer stack symmetry, and material compliance.

These layer-specific design requirements are combined into a single editor – the Layer Stack Manager

To open the Layer Stack Manager, select Design » Layer Stack Manager from the main menus of the PCB editor. The Layer Stack Manager opens in a document view, in the same way as a schematic sheet, the PCB, and other document types. It can be left open while the board is being worked on, allowing you to switch back and forth between the board and the LSM. All of the standard view behaviors, such as splitting the screen or opening on a separate monitor are supported. Changes made in the Layer Stack Manager become available in the PCB editor after a Save is performed.

All aspects of layer stack management are performed in the Layer Stack Manager.
All aspects of layer stack management are performed in the Layer Stack Manager.

Depending on the board structure, the layer Stack Manager will include the following tabs:

Stackup Add, remove, and order the signal, plane, and dielectric layers; and assign/configure the Material properties assigned to each layer.
Impedance Configure the Impedance profiles, when controlled impedance routing is being used.
Via Types Configure the allowed Via Types, defining which layers each Via Type spans.
Back Drills Configure the layer spans to be back-drilled when there is a pad or via stub present.
Printed Electronics Configure the layer arrangement in a printed electronics design.
Board Configure how the different substacks are arranged in an advanced rigid-flex design.

Editing the Layer Stack Properties

The Layer Stack Manager presents the layer stack properties in a spreadsheet-like editing grid. The properties can be edited directly in the grid, or in the Properties panel. Depending on the board structure, the Layer Stack Manager will include the following tabs, each presenting its own set of attributes in the editing grid and the Properties paneli.

To change the measurement units used in the active layer stack, choose Tools » Measurement Units then select the desired unit of measure (milinµ, or mm). Alternatively, use the Ctrl+Q keyboard shortcut to cycle through the measurement units.

Stackup Tab

The Stackup tab details the fabrication layers. In this tab, layers can be added, removed, and configured. For a standard rigid-flex design, the layer set used in each stack can also be enabled and disabled in this tab. An advanced rigid-flex design is configured in the Board tab.

Right-click to add, remove and reorder the layers. Values can be edited in the Properties panel, or directly in the cell of the grid.Right-click to add, remove and reorder the layers. Values can be edited in the Properties panel, or directly in the cell of the grid.

Editing the Layerstack

Add a layer

To add a layer Right-click in the layer grid, click the button or use the Edit » Add Layer commands to add a layer. The new layer will be added next to the layer currently selected in the grid. Adding a Signal or Plane (copper) layer will also add a dielectric layer when an existing adjacent layer is also a copper layer. A maximum of 32 signal layers and 16 plane layers can be added. If required, plane layers can be split any number of times, and split-within-split areas defined – learn more.

Move a layer Right-click in the layer grid then choose Move layer up / Move layer down or use the Edit » Layer Up / Edit » Layer Down command from the main menus to move the selected layer up or down in the Layer Stack within the layers of the same type.
Delete a layer Right-click in the layer grid or use Edit » Delete Layer from the main menus to delete the selected layer in the Layer Stacki. If the layer to be deleted contains primitives, a dialog asking for confirmation will open before deletion occurs. Click Yes to proceed with the deletion.
Define the Layer Material

The layer Material can either be typed into the selected Material cell or selected in the Select Material dialog, which is accessed by clicking the  button.

Stack symmetry If the Stack Symmetry option is enabled in the Board section of the Properties panel, layers are added in matching pairs centered around the mid-dielectric layer.
Additional properties

Right-click a column header, then choose Select columns to access the Select Columns dialog (), where you can enable/disable and order the columns displayed in the layer grid. Note that only the commonly used properties are displayed in the Properties panel.

Apply Surface Finish Surface Finish can be added to an outer copper layer by using the appropriate right-click sub-menu and adding a Surface Finish layer.

Impedance Tab

The Impedance tab is used to configure the Impedance profiles, when controlled impedance routing is being used. Click on the Impedance Tab at the bottom of the Layer Stack Manager to configure the Impedance Profile requirements. Once the impedance profiles have been configured, the required profile can then be selected in the Routing Width or Differential Pairs Routing design rules.

Add a new Profile, enable the layers that it applies on, configure the reference layers, and define the properties of the Profile in the Properties panel.Add a new Profile, enable the layers that it applies on, configure the reference layers, and define the properties of the Profile in the Properties panel.

Editing an Impedance Profile

Adding a Profile

Click (or the Add Impedance Profile button if no profiles have been added yet) to add a new Impedance Profile, then define the required Type, Target Impedance and Target Tolerance in the Properties panel. The Description is optional.

Choosing the layer

The next step is to define which layers the currently selected profile will be available on. The grid is divided into two zones: the layers in the stackup are displayed on the left, and on the right are the layers that the currently selected impedance profile will be available on. Use the layer checkbox in the Impedance Profile region to make that layer available for the selected impedance profile.

 

When you select an enabled layer in the Impedance Profile region, all layers in the layer stack are faded, except those being used to calculate the impedance for that selected signal layer ().

Assign the reference layers Once the layer has an Impedance Profile assigned, edit that layer's reference layer(s) in the Top Ref and Bottom Ref columns. Note that reference layer(s) can be of Type Plane or Signal.
Configure the impedance properties The impedance calculators support forward and reverse impedance calculations. If you enter the Target Impedance, the Width will change automatically (forward calculation), or enter the Width and the Target Impedance will change automatically (reverse calculation).
Define the etch The Etch = 0.5[(W1-W2)/Thickness] , calculated from the (hover the cursor over the ? in the panel to display the formula)
Configure the differential impedance calculation

For a differential impedance calculation, lock either the Width or Trace Gap by clicking the appropriate button. The unlocked variable will then be calculated as the Target Impedance value changes. Alternatively, edit the unlocked variable to change the Target Impedance.

  • Impedance calculation support is delivered by the Simbeor® software. The calculator supports single and differential coplanar structures, and the differential impedance calculator supports an asymmetric stripline structure. All calculations use a frequency of 1 GHz. To improve calculation speeds, impedance profiles are calculated in separate threads (when available).

  • For a stripline structure, the dielectric height is calculated as the distance between copper layers (see H2 on the image).

  • The impedance calculator supports multiple adjacent dielectric layers. These layers can have different dielectric properties.

Learn more about setting up the Properties for Controlled Impedance Routing.

Via Types Tab

The Via Types tab is used to define the allowed Z-plane layer-spanning requirements of the vias used in the design. The X-Y properties of the vias, including the diameter and hole size are controlled by the the applicable Routing Style design rule.

Define each of the required Via Types.Define each of the required Via Types.

Editing the Via Types

The default via The Layer Stack for a new board includes a single, thruhole via span definition in the Via Types tab of the Layer Stack Manager.  For a two-layer board, the default via is named Thru 1:2, the naming reflecting the via type and the First and Last layers that the via spans. The default thruhole span cannot be deleted.
Add a new Via Type

Click the button to add an additional Via Type, then select the layers that this Via Type spans in the Properties panel. The new definition will have a name of <Type> <FirstLayer>:<LastLayer> (e.g., Thru 1:2). The software will automatically detect the type (e.g., Thru, Blind, Buried) based on the layers chosen and name the Via Type accordingly.

Adding a µVia If a µVia is required, enable the µVia checkbox. This option will be only available when the via spans adjacent layers or adjacent +1 (referred to as a Skip via).
Mirroring a via If the Layer Stack has the Stack Symmetry option enabled, the Mirror option will become available. When Mirror is enabled a mirror of the current via, spanning the symmetrical layers in the layer stack, is automatically created. 
Selecting a Via Type during routing

When you change layers during interactive routing:

  • The Properties panel will display the applicable Via Type ( ).

  • If multiple Via Types are available to suit the layers being spanned, press the 6 shortcut to cycle through the available Via Types.

  • The proposed Via Type is detailed on the Status bar ().

Vias placed in the workspace include a Name property dropdown, which lists all of the Via Types defined in the Layer Stack Manager. All vias used in the board must be one of the Via Types defined in the Layer Stack Manager.

Learn more about setting up the Properties for Via Types on the Blind, Buried & Micro Via Definition page.

Back Drills Tab

In a high-speed design, signal reflections can occur when the barrel of a via extends beyond the signal layers that the signal is routed on. This can lead to signal degradation and signal integrity issues. One approach used to resolve this is to drill out the unused via barrels using controlled depth drilling, a technique also referred to as back drilling.

Back drill properties are configured in the Back Drills tab. This tab appears when Back Drills are enabled in the Tools » Features sub-menu or by clicking the  button then choosing Back Drills.

Editing the Back Drills

How Back Drills work The Back Drills tab is used to define the layer spans that are required to be back-drilled when there is a pad or via stub present. These settings are used in conjunction with the Max Via Stub Length design rule, where the maximum stub length and the drill oversize amount are specified. The Where the Object Matches setting in the rule can be used to restrict stub-removal to specific nets.
Add a new Back Drill

Click the  button to add a new back drill definition. The definition will be named according to the First layer and Last layer selected in the Back Drill section of the Properties panel, for example, BD 1:3. First layer defines the first layer to be drilled, Last layer defines the layer that drilling stops before (Last layer is the first layer in the layer stack that will not be back drilled).

Mirroring a Back Drill If the Substack Properties has the Stack Symmetry option enabled in the Properties panel, the Mirror option will become available in the Back Drill section of the panel. When this is enabled, a mirror of the current Back Drill is created, for example, BD 1:3 | 6:4.

Learn more about setting up the properties for Back Drills on the Controlled Depth Drilling (Back Drilling) page.

Printed Electronics Tab

Using modern printing technology, it is possible to print conductive and non-conductive layers directly onto a substrate material, building up an electronic circuit. This is referred to as printed electronics. The layer stack is configured for printed electronics by selecting the Tools » Features » Printed Electronics option. In this mode, all tabs are replaced by the single Printed Electronics Stackup tab.

Printed electronics use a different approach to defining the layerstack.Printed electronics use a different approach to defining the layerstack.

Configuring the Layerstack for Printed Electronics

Defining the layers Traditional dielectric layers are not used in printed electronics. Instead, local dielectric patches are printed where routing must cross over. When the Printed Electronics option is enabled in the Features drop-down, all dielectric layers are removed from the layer stack and instead, the dielectric patches are defined by placing suitably shaped region objects on non-conductive layers.
How Layers are named In printed electronics, copper signal layers are referred to as conductive layers, and insulating layers are referred to as non-conductive layers.

Learn more about setting up the Properties for Printed Electronic layer on the Designing for Printed Electronics page.

Board Tab

The Board tab is used to configure the different substacks required in a rigid-flex design. The tab is automatically displayed when the Rigid-Flex (Advanced) mode is enabled. Note that the Board tab is not used/available when the standard Rigid-Flex mode is chosen.

The Board tab being used to configure a bookbinder style rigid-flex PCB, note that the center section has two flexible Substacks.The Board tab being used to configure a bookbinder style rigid-flex PCB, note that the center section has two flexible Substacks.

Working in the Board View Tab

Add a new Substack Additional substacks can be quickly created from an existing substack using the Shift+Click shortcut to select the required layers, and then dragging the selection horizontally to position it in the set of substacks.
Configure layer intrusion Use the Intrusion Left / Right fields to configure if adjacent layers intrude into the neighboring Substack.
Configure layer adjacency Configure the relationships between layers in adjacent Substacks, e.g., Do they share layers (Common), or are the layers unique in that Substack (Individual)
Editing a substack Double-click on a specific substack in the Board tab to open its Layer tab, where it can be edited.
Adding a Branch Add additional Branches. Branches are used when the design has multiple flex sections radiating from a single rigid section. Learn more about Branches.

Configuring the Layer Properties and Materials

The properties of each layer can be edited directly in the LSM grid, or a pre-defined material can be selected from the Material Library by clicking the ellipsis button () in the Material cell for the selected layer. The Stackup Tab collapsible section earlier on this page summarizes the various techniques available for adding, removing, editing, and ordering the layers.

User-defined property columns can be added and the visibility of all columns can be configured in the Select columns dialog. To open the dialog, right-click on any column heading in the grid region then choose Select columns from the context menu.

The Select columns dialog
The Select columns dialog

Layer Types and their Properties

There is a large variety of materials used in the fabrication of a printed circuit board. The table in the collapsible section below gives a brief summary of the common materials used.

Materials Library and Library Compliance

The properties of each layer can be edited directly in the LSM grid, or a pre-defined material can be selected from the Material Library by clicking the ellipsis button () in the Material cell for the selected layer. The Stackup Tab collapsible section earlier on this page summarizes the various techniques available for adding, removing, editing, and ordering the layers.

The Select columns dialog allows for the addition of user-defined property columns and the configuration of the visibility of all columns. To open the dialog, right-click on any column heading in the grid region and choose Select columns from the context menu.

The Select columns dialog
The Select columns dialog

Layer Types and their Properties

There is a large variety of materials used in the fabrication of a printed circuit board. The table in the collapsible section below gives a brief summary of the common materials used.

Materials Library and Library Compliance

Preferred layer stack materials can be pre-defined in the Material Library. In the Layer Stack Manager, select Tools » Material Library to open the Altium Material Library dialog, where existing materials can be reviewed and new material definitions added.

The Altium Material Library dialog
The Altium Material Library dialog

The material for a specific layer is not selected in the Altium Material Library dialog. To use a specific material for a layer, click the ellipsis () for that layer in the Materials cell of the layer stack grid or click  in the Material field in the Properties panel when the layer is selected in the layer stack grid. This will open the Select Material dialog, which restricts the library to only show materials suitable for the layer that the ellipsis control was clicked.

The Select Material dialog
The Select Material dialog

To select the columns displayed in the Altium Material Library dialog or the Select Material dialog, click the  button to open the Material Library Settings dialog.

The Material Library Settings dialog
The Material Library Settings dialog

If the Library Compliance checkbox is enabled in the Layer Stack Manager, then for each layer that has been selected from the Material Library, the current layer properties are checked against the values of that material definition in the library. Any property that is not compliant is marked with an error flag. Re-select the material () to update the values to the Material Library settings.

Layer Stack Symmetry

If you require the board layer stack to be symmetrical, enable the Stack Symmetry checkbox in the Board region of the Properties panel. When this is done, the layer stack is immediately checked for symmetry around the central dielectric layer. If any pair of layers that are equidistant from the central dielectric reference layer are not identical, the Stack is not symmetric dialog opens.

The Layer stack symmetry mismatches grid at the top of the dialog details all detected conflicts in layer stack symmetry.

The lower region of the dialog provides the following options available to achieve layer stack symmetry:

  • Mirror top half down - the settings of each of the layers above the central dielectric layer are copied down to the symmetrical partner layer.
  • Mirror bottom half up - the settings of each of the layers below the central dielectric layer are copied up to the symmetrical partner layer.
  • Mirror whole stack down - an additional dielectric layer is inserted after the last copper (Surface Finish) layer, and then all of the signal and dielectric layers are replicated and mirrored below this new dielectric layer.
  • Mirror whole stack up - an additional dielectric layer is inserted before the first copper (Surface Finish) layer, and then all of the signal and dielectric layers are replicated and mirrored above this new dielectric layer.

When Stack Symmetry is enabled:

  • An edit action applied to a layer property is automatically applied to the symmetrical partner layer.
  • Adding layers will automatically add matching symmetrical partner layers.
Use the Stack Symmetry option as a quick way of defining a symmetric board - define half of the layer stack, enable the Stack Symmetry option, then use one of the mirror whole stack options to replicate that set of layers.

Layer Stack Visualization

An excellent way to verify the layer stack is to visualize it in 3D. The Layerstack Visualizer dialog lets you see the layer stack in either 2D or 3D.

  • Select Tools » Layerstack Visualizer in the Layer Stack Manager to open the Layerstack Visualizer.
  • Use the controls to configure the presentation of the layer stack.
  • Right-click and drag to reorient the board in the visualizer.
  • Left-click on the image, then Ctrl+C to copy the image to the Windows clipboard.

Defining and Configuring the Rigid-Flex Substacks

Main page: Rigid-Flex Design

Rigid-Flex is under active development and now supports two modes of Rigid-Flex design. The original, or standard mode, referred to as Rigid-Flex, supports simple rigid-flex designs. If your design has more complex rigid-flex requirements, such as overlapping flex regions, then you need the Advanced Rigid-Flex mode (also known as Rigid-Flex 2.0). As well as overlapping flex regions, the Advanced mode also brings: a visual definition of the substacks, easier definition of the rigid and flexible board regions, bends on nested cutouts, custom-shaped splits, and support for bookbinder-type structures. The required mode is selected in the Layer Stack Manager, as shown below.

The interface changes as you select either the standard or Advanced Rigid-Flex mode (hover the cursor over the image to show the difference).The interface changes as you select either the standard or Advanced Rigid-Flex mode (hover the cursor over the image to show the difference).

Learn more about Designing a Rigid-Flex PCB.

 

Each separate zone or region of a rigid-flex design can be made up of a different number of layers. To achieve that you need to be able to define multiple stacks, referred to as substacks.

Learn more about Designing a Rigid-Flex PCB

Single Layer PCB Support

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

A single-layer PCB stack can be created by deleting either the top or bottom layer from a 2-layer PCB stack.

In a 2-layer PCB, you can now delete either the Top or Bottom Layer from its layer stack.
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.
  • For a single-layer PCB, you can only create impedance profiles of Single-Coplanar and Differential-Coplanar types on the Impedance tab of the Layer Stack Manager.
  • 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.
  • 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.

Saving and Loading a Layer Stack Copy Link Copied

Saving and Loading a Layer Stack using a Stackup Document File

To save the current stackup to a stackup document file (*.stackup or *.stackupx), use the File » Save As command from the main menus. A dialog will open in which you can select the location, name and type of the file.

To load a stackup from an existing stackup document file, use the File » Load Stackup from File command from the main menus. The Open Stackup Document dialog will appear from where you can browse and open the desired file.

Saving and Loading a Layer Stack using a Connected Workspace

To save the current stackup to your connected Workspace, choose the File » Save to Server command from the main menus. The Choose Planned Item Revision dialog will appear – use this to choose an existing Workspace Layerstack to save the stackup to its next revision.

  • If the target Workspace Layerstack doesn't exist, you can create it through the Choose Planned Item Revision dialog on the fly in the chosen Workspace folder by right-clicking in the revision list region of the dialog and selecting the Create Item » Layerstack command. In the Create New Item dialog that opens, disable the Open for editing after creation option; otherwise, you will enter direct editing mode.
  • A number of Workspace Layerstacks are provided by default within the Managed Content\Templates\Layer Stacks Workspace folder (if you opted to include Sample Data upon the activation/installation of your Workspace).

  • A new layerstack can also be created using the Layerstack command from the menu of the Add button or the context menu of the template grid on the Templates tab of the Data Management – Templates page of the Preferences dialog. After selecting the command, click OK in the Close Preferences dialog that opens to close the Preferences dialog and open the temporary Stackup Editor. A planned revision of the new Workspace Layerstack will be created automatically in a Workspace folder of the Layerstacks type.
  • A new Workspace Layerstack can also be created by uploading an existing stackup document file (*.stackup). Select the Load from File command from the menu of the Add button or the Add context menu of the template grid on the Templates tab of the Data Management – Templates page of the Preferences dialog. In the Open dialog (a standard Windows open-type dialog) that opens, select the Layer Stack-up File (*.stackup) option in the drop-down at the right of the File name field and use the dialog to browse to and open the required file that will be uploaded into the initial revision of the new Workspace Layerstack created automatically in a Workspace folder of the Layerstacks type.
  • If the required stackup document file resides in the Local Template folder (defined at the bottom of the Data Management – Templates page) and is listed under the Local entry of the template grid, it can be migrated to a new Workspace Layerstack by right-clicking on it and selecting the Migrate to Server command. Click the OK button in the Template migration dialog to proceed with the migration process – as stated in this dialog, the original layerstack file will be added to a Zip archive in the local template folder (therefore, it will not be visible under the Local template list).
  • A Workspace Layerstack can be previewed in the Explorer panel. When the layerstack entry is selected in the revision region of the panel, switch to the Preview aspect view tab to see the layer stackup.

To edit an existing Workspace Stackup, right-click on its entry on the Templates tab of the Data Management – Templates page of the Preferences dialog and choose the Edit command from the context menu. The temporary editor will open, with the template contained in the latest revision of the Workspace Stackup opened for editing. Make changes as required, then save the stackup into the next revision of the Workspace Stackup (right-click the stackup entry in the Projects panel and select Save to Server).

If you need to update a Workspace Stackup and you have an updated stackup document file, you can upload that file to that Workspace Stackup. From the Templates tab of the  Data Management – Templates page of the Preferences dialog, right-click on the template entry and choose the Upload command from the context menu. Use the Open dialog (a standard Windows open-type dialog) that opens to browse and open the required file that will be uploaded into the next revision of the Workspace Stackup.

To load a stackup from your connected Workspace, choose the File » Load Stackup From Server command from the main menus. The Choose Item Revision dialog will appear – use this to load layer stackup data from a Workspace Layerstack.

If you are not connected to your Workspace, you can still work with Altium Designer (under your valid Altium Designer license), but you will not be able to access your organization's Workspace or any other services it provides. You will, therefore, not be able to use any Workspace layerstacks. You can only use stackup document files (File » Load Stackup From File).
A Workspace layer stackup can also be used as a configuration data item in one or more defined Environment Configurations. An environment configuration is used to constrain a designer's working environment to only use company-ratified design elements. Environment configurations are defined and stored within the Team Configuration Center – a service provided through the Workspace. Once you have connected to the Workspace and chosen (if applicable) from the selection of environment configurations available to you, Altium Designer will be configured with respect to the use of Layerstacks. If the chosen environment configuration has one or more defined Layerstack Item revisions, then only those will be available to you for reuse. If the chosen environment configuration applicable to you does not have any layerstack revisions specified/added or is set to Do Not Control, then all available saved item revisions (shared with you) will be available. You are also free to use local stackup files. For more information, see Environment Configuration Management (Altium 365 Workspace, Enterprise Server Workspace).

Loading a Predefined Layer Stack

A number of pre-defined layer stacks are available in the Tools » Presets menu.

Exporting a Layer Stack

The current layer stack can be exported to a spreadsheet (*.csv) file by choosing the File » Export CSV command from the main menus. After launching the command, the Save As dialog opens in which you can select the desired location and name of the *.csv file.

Using the File » Export To Simbeor command, you can also export the layer stack to a Simbeor file (*.esx).

The layers in the layerstack form the space on which you build up the design. There are a number of design tasks that are related to the layers that are not performed in the Layer Stack Manager. These tasks are summarized below, with links to more information.

Defining the Board Shape

Where the layer stack defines the board in the Z-plane, the Board Shape defines the board in the X and Y planes. Also referred to as the board outline, the board shape is a closed polygonal shape that defines the overall extent of the board. The Board Shape can be made up of a single Board Region (for a traditional rigid PCB) or multiple board regions (for a rigid-flex PCB).

The Board Shape can be:

  • Defined manually - by redefining the existing shape or placing one or more new board regions in Board Planning mode.
  • Defined from selected objects - typically done from an outline on a mechanical layer. Use this option if an outline has been imported from another design tool.
  • Defined from a 3D body - use this option if the blank board has been imported as a STEP model from an MCAD tool into a 3D Body Object (Place » 3D Body).
  • Pulled directly from an MCAD package - Altium is developing direct ECAD - MCAD design technology called Altium CoDesigner. Learn more about ECAD-MCAD CoDesign.

Learn more about these approaches to defining the board shape.

Once the shape has been defined, bends in the flexible sections of a rigid-flex design are defined by placing Bending Lines.

Learn more about Rigid-Flex Design.

Assigning a Net to a Plane Layer

Panel page: Split Plane Editor
Related page: Internal Power & Split Planes

Assign a net to a plane layer or a net to a split plane region in the Split Plane Editor mode of the PCB panel.

The panel lists all plane layers. When a layer is selected in the Layers section, the section below will list all of the split plane zones on that layer (there will only be one if the plane is continuous with no splits defined). Double-click on a split plane zone to open the Split Plane dialog to assign a net. You can also double-click on the layer in the workspace (when the plane layer is the active layer) to open the dialog.

Configuring the Layer Stack for Components Mounted on an Internal Signal Layer

Related article: Embedded Components

There are two situations where components can be mounted on an internal signal layer:

  1. when there are embedded components, or
  2. when there are components mounted on a flex region of a rigid-flex board, and that flex layer extends from a mid-layer in the rigid section of the board.

The software needs to know which way components are oriented for each layer they are mounted on to know when the component primitives must be mirrored. This is configured automatically for the Top and Bottom Layers; for other layers, the setting is configured by the designer. 

A component embedded on an internal signal layer (the component has been highlighted with blue outlines, the cavity with orange outlines).A component embedded on an internal signal layer (the component has been highlighted with blue outlines, the cavity with orange outlines).

  • Component orientation is configured for a layer in the Orientation column of the Stackup tab of the Layer Stack Manager.
  • If the Orientation column is not visible, enable it by right-clicking on an existing heading in the layers grid and then selecting Select columns from the context menu.
  • The components on a layer can either point upwards (Top) or downwards (Bottom).

Documenting the Layer Stack

Object page: Layer Stack Table

Documentation is a key part of the design process and is particularly important for designs with a complex layer stack structure, such as a rigid-flex design. To support this, Altium Designer includes a Layer Stack Table, which is placed (Place » Layer Stack Table) and positioned alongside the board design in the workspace. The information in the layer stack table comes from the Layer Stack Manager.

Include a Layer Stack Table to document the design.
Include a Layer Stack Table to document the design.

  • To place a Layer Stack Table, select Place » Layer Stack Table.
  • The Layer Stack Table details the following:
    • Layers used in the design
    • Material used for each layer
    • Thickness of each layer (and optionally the total board thickness).
    • The Dielectric Constant
    • The name of each stack and the layers used in that stack
  • Double-click anywhere on the placed table to open the Properties panel in Layer Stack Table mode.
  • The Layer Stack Table can also include an optional outline of the board showing how the various layer stacks are assigned to regions of the board. Use the Show Board Map option and slider bar to configure the map settings.
  • The Layer Stack Table is an intelligent design object that can be placed and updated as the design progresses. Double-click on the Layer Stack Table to edit it in the Properties panel.
  • An alternative approach to documenting the layer stack is to add a Draftsman document to the project and add a Layer Stack Table to it. Learn more about Draftsman.

Place the .Total_Thickness and the .Total_Thickness(<SubstackName>) special strings on a mechanical layer to include this information in your design documentation.

Including a Drill Table

Object page: Drill Table

Altium Designer includes an intelligent Drill Table that is placed like any other design object. The table can either display the drills required for all layer pairs (composite), or a specific layer pair. Place a drill table for each layer pair used in the design if you prefer separate drill information for each layer pair.

An alternative approach to documenting the layer stack is to add a Draftsman document to the project and add a Layer Stack Table to it. Learn more about Draftsman.

High Quality, Flexible Design Documentation Copy Link Copied

Main article: Draftsman

Altium Designer also provides a dedicated documentation editor - Draftsman. Draftsman has been built from the ground up as an environment for creating high-quality documentation that can include dimensions, notes, layers stack tables, and drill tables. Based on a dedicated file format and set of drawing tools, Draftsman provides an interactive approach to bringing together fabrication and assembly drawings with custom templates, annotations, dimensions, callouts, and notes.

Draftsman also supports more advanced drawing features including a Board Isometric View, a Board Detail View, and a Board Realistic View (3D view).

Place drawing views, objects and automated annotations on single or multi-page Draftsman documents. Place drawing views, objects and automated annotations on single or multi-page Draftsman documents.

Learn more about Draftsman

Layer Stackup Terminology Copy Link Copied

Term Meaning
Blind Via A via that starts on a surface layer but does not continue all the way through the board. Typically a blind via descends 1 layer down to the next copper layer.
Buried Via A via that starts on one internal layer and ends on another internal layer but does not reach a surface copper layer.
Core A rigid laminate (often FR-4) with copper foil on both sides.
Double-Sided Board A board that has 2 copper layers, one on either side of an insulating core. All holes are through holes, i.e., they pass all the way from one side of the board to the other.
Fine Line Features and Clearances Tracks/clearances down to 100µm (0.1mm or 4mil) are considered standard for PCB fabrication today. The current technology limit available in component packaging is around 10µm.
High Density Interconnect (HDI) High Density Interconnect technology, a PCB that has a higher wiring density per unit area than a conventional PCB. This is achieved using fine-line features and clearances, microvias, buried vias, and sequential lamination technologies. This name is also used as an alternative to Sequential layer Build-Up (SBU).
Microvia Defined as a via that has a hole diameter smaller than 6 mils (150µm). Microvias can be photo imaged, mechanically drilled, or laser drilled. Laser-drilled microvias are an essential High Density Interconnect (HDI) technology, as they allow vias to be placed within a component pad and when used as part of a build-up fabrication process, allow signal layer transitions without the need for short tracks (referred to as via stubs), greatly reducing via-induced signal integrity issues.
Multilayer Board

A board with multiple copper layers, ranging from 4 to over 30. A multilayer board can be fabricated in different ways:

  • As a set of thin, double-sided boards that are stacked (separated by prepreg) and laminated into a single structure under heat and pressure. In this type of multilayer board, the holes can be all the way through the board (through-hole), blind, or buried. Note that only specific layers can be mechanically drilled to create the buried vias, as they are simply through holes drilled in the thin double-sided boards before the lamination process.
  • Alternatively, a multilayer board is fabricated as described, and then additional layers are laminated onto either side. This approach is used when the design demands the use of microvias, embedded components, or rigid-flex technology.
Prepreg A glass-fiber cloth impregnated with thermosetting epoxy (resin+hardener) which is only partially cured.
Sequential Lamination The name given to the technique of creating a multilayer PCB which includes mechanically drilled buried vias (drilled in the thin, double-sided boards prior to final lamination).
Sequential layer Build-Up (SBU) Starts as a core (double-sided or an insulator), with conductive and dielectric layers formed one after the other (using multiple pressure passes), on both sides of the board. This technology also allows blind vias to be created during the build-up process and discrete or formed components to be embedded. Also referred to as High Density Interconnect (HDI) technology.
Surface Laminar Circuit (SLC) Starts as a multilayer core, with build-up layers added on either side (typically 1 to 4). The common notation used to describe the finished board is Build-up copper layers + Core copper layers + Build-up copper layers. For example, 2+4+2 describes a board with a 4-layer core, with 2 layers laminated on either side (also written as 2-4-2). This technology allows blind vias to be created during the build-up process and discrete or formed components to be embedded.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.