Search In: Doc:Documentation: Altium Designer
Altium DesignerAltium 365Altium MCAD CoDesignerAltium CircuitMakerCompany DashboardAltium On-Prem Enterprise ServerAltium Infrastructure Server
Ver: Version: 24
2423222120.220.120.019.119.018.118.017.117.016.116.015.1
Close
Suche Search on Documentation

Defining the Layer Stack in Altium Designer

Created: Januar 19, 2024 | Updated: August 21, 2024 | Applies to version: 24

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.

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.

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.

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 do this, the designer must be able to define multiple PCB layer stacks and assign different layer stacks to different zones of the rigid-flex design.

Learn more about Rigid-Flex Design

The Layer Stack Manager

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.

The Layer Stack Manager combines all these layer-specific design requirements into a single editor.

To open the Layer Stack Manager select Design » Layer Stack Manager from the main menus of the PCB editor.

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.

The Layer Stack Manager is used to:

  • Add, remove, and order the signal, plane, and dielectric layers.

  • Select the Material properties from the Materials Library, or configure them manually.

  • Add additional user-defined fields to the Layer Stack.

  • Configure the allowed Via Types, defining which layers each Via Type spans.

  • Configure the Impedance profiles, when controlled impedance routing is being used.

  • Configure advanced features, including rigid-flex design, printed electronics, and back drilling.

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.

Note that a Save action (File » Save to PCB, shortcut: Ctrl+S) must be performed in the Layer Stack Manager before changes are reflected in the PCB.

The functionality is divided over a number of tabs displayed across the bottom of the Layer Stack Manager:

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

Editing the Layer Stack Properties

The Layer Stack Manager presents the layer properties in a spreadsheet-like grid. The properties can be edited directly in the grid or they can be edited in the Properties panel. The panel can be used in each of the Layer Stack Manager tabs, for example, giving access to the impedance profile and transmission line properties in the Impedance tab or the µVia settings in the Via Types tab.

A few of the modes of the Properties panel in the Layer Stack Manager  
A few of the modes of the Properties panel in the Layer Stack Manager

The Properties panel can be enabled/disabled via the button at the bottom-right of the software.

When the Stackup tab of the Layer Stack document is active, the Properties panel allows you to edit the layer properties of the Layer Stack.

  • Name – the name of the layer.
  • Manufacturer – the layer manufacturer.
  • Material – the layer material. This can be pre-defined in the Altium Material Library dialog (Tools » Material Library) in the Constructions field or user-defined in the Layer Stack. Click to open the Select Material dialog to choose the desired material for the currently selected layer in the layer stack.
  • Thickness – the thickness of the signal layer.
  • Dk – this is the Dielectric Constant (also referred to as εr in electromagnetics). This indicates the relative permittivity of an insulator material, which refers to its ability to store electrical energy in an electric field. For insulating purposes, a material with a lower dielectric constant is better, and in RF applications, a higher dielectric constant may be desirable. In addition, the lower the relative dielectric constant, the closer the performance of the material to that of air. This property is critical to matching the impedance requirements of certain transmission lines.
  • Df – this is the Dissipation Factor. This indicates the efficiency of insulating material by showing the rate of energy loss for a certain mode of oscillation, such as mechanical, electrical, or electromechanical oscillation. In other words, this is the property of a material that describes how much of the energy transmitted is absorbed by the material. The greater the loss tangent, the larger the energy absorption into the material. This property directly impacts the signal attenuation at high speeds.
  • Process – displays the copper plating process that is applied to the base copper that makes up the outer signal layers of the PCB (the Top Layer and Bottom Layer).
  • Weight – the weight of the copper per unit area, usually expressed in ounces/square foot (e.g., 0.5 oz/ft2).
  • Orientation – this defines which way the components point (orient) on that layer. For the top and bottom sides, this is set automatically in a new board. For other signal layers, it is used for:
    • Rigid-flex designs, where components mount on an inner signal layer that becomes a surface layer on a flex section, the software needs to know which way those components point. Use the drop-down to select the required orientation. Choices include: Not allowed, Top, and Bottom.
    • For a design that includes embedded components, the software must know which way a component points. Refer to the Designing a PCB with Embedded Components page for information regarding setting the component orientation in the layer stack. Use the drop-down to select the required orientation. Choices include: Not allowed, Top, and Bottom.

  • Copper Orientation – this defines the direction that the copper is laminated onto the core. Use the drop-down to select Above or Below, which determines the direction from which it is etched.

    The Copper Orientation can also be chosen using the drop-down in the Copper Orientation column of the Layer Stack. To enable the column, right-click in the header, choose Select columns then enable the Copper Orientation entry in the Select columns dialog. Also, the Trace Inverted option in the Impedance Profile mode of the panel can be used to configure the copper orientation.

    The orientation can be configured using the Copper Orientation drop-down in the Stackup mode of the Properties panel in the Copper Orientation column (if it is currently displayed) or by the Trace Inverted checkbox in the Impedance Profile mode of the Properties panel.

  • Pullback Distance – the distance from the plane edge to the board edge.
  • Frequency – this is the frequency at which the material is tested and the value that Dk / Df corresponds to a certain frequency. Frequency is also taken from material references.
  • Description – enter a meaningful description.
  • Constructions – for dielectric layers, this displays the constructions of the layer. The numerical reference relates to the structure of the woven glass fabric used in the dielectric layer material; these are standard references used by PCB fabricators.

  • Resin – displays the resin percentage of the layer.

    Notes on Constructions and Resin:
    The choice of laminate construction can significantly impact both cost and performance. As should be expected, a single-ply construction will typically represent a cost savings compared to a multiple-ply construction. The magnitude of these savings will depend on the specific glass styles involved and a host of other parameters. Performance can also be affected and should be considered when specifying the constructions to be used. First, single-ply constructions are often lower in resin content. The other main benefit of single-ply constructions is dielectric thickness control beyond resin content considerations. Tighter thickness tolerances can be achieved using a single-ply construction.
    Constructions with relatively lower resin contents are often preferred since they result in less z-axis expansion and can therefore improve reliability in many applications. In addition, lower resin contents can also improve dimensional stability, resistance to warpage, and dielectric thickness control. On the other hand, constructions with higher resin contents result in lower dielectric constant values, which are sometimes preferred for electrical performance. In addition, a certain minimum resin content is required to ensure adequate resin-to-glass wet-out and to prevent voids from occurring within the laminate. The ability to wet out the glass filaments fully with resin is also important for CAP resistance.
  • Material Frequency – this is the frequency at which the material is tested and the value that Dk / Df corresponds to a certain frequency. Frequency is also taken from material references.
  • GlassTransTemp – this is the Glass Transition Temperature (also known as TG) and is the temperature at which the resin changes from a glass-like state to an amorphous state changing its mechanical behavior, i.e. expansion rate.
  • Note – enter any pertinent notes for the layer.
  • Comment – enter any necessary comments for the layer.
  • Stack Symmetry – enable to maintain layer stack symmetry. Refer to the Layer Stack Symmetry section to learn more.
  • Library Compliance – when enabled, 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.

  • Substack – this information is for the currently selected substack (layers, dielectric, thicknesses, etc.). As you switch from one substack to another, this information will update accordingly (for the currently selected substack).

    The Substack region will only be available if the Rigid/Flex option is enabled in the Features drop-down.
  • Stack Name – enter the substack name. Naming the substack is useful when the X/Y stackup region is being assigned a layer substack.
  • Is Flex – enable if the substack is flex.
  • Layers – the number of conductive layers.
  • Dielectrics – the number of dielectrics.
  • Conductive Thickness – this is the sum of the thicknesses of all signal and plane layers (all copper or conductive layers).
  • Dielectric Thickness – the thickness of dielectric layer(s).
  • Total Thickness – the total thickness of the finished board.
  • Roughness – shows roughness of conductive layers.
  • Model Type – preferred model for calculating the impact of surface roughness (refer to the articles below for more information on the various models). Applies to all copper layers in the stack (should it be the substack?).
  • Surface Roughness – value of the surface roughness (available from your fabricator). Enter a value between 0 to 10µm, default is 0.1µm
  • Roughness Factor – characterizes the expected maximal increase in conductor losses due to the roughness effect. Enter a value between 1 to 100; the default is 2.
  • Copper Resistance - value of the copper resistance in nOhms.
  • Via Plating Thickness - the total thickness of the via plating.

To learn more about the options and controls available for the other Layer Stack tabs, use the links below:

Defining the Layer Stack

The layers you add in the Stackup tab of the Layer Stack Manager are the layers that will be fabricated during the manufacturing process.

Layer properties can be entered directly into the grid, or selected from the Material Library.Layer properties can be entered directly into the grid, or selected from the Material Library.

The properties of a layer can be edited directly in the grid or in the Properties panel.

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

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 in Open Beta and 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

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).

Other Layer-related Design Tasks

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

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

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.
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.

Content