Layer Stack Manager

Old Content - visit altium.com/documentation

Modified by Annika Krilov on Jul 14, 2015

The Layer Stack Manager(Flex-Rigid) Dialog.

Summary

The Layer Stack Manager dialog allows the designer to configure the layers of the board. It also allows designer to configure drill pairs and impedance formula editor.

Especially, for Flex-Rigid design, the designer can add sub layer stack for different board regions.

The Layer Stack Manager dialog can be edited in two modes: Simple or Advanced. Click the Simple/Advanced button at lower left to toggle between these two modes.

Access

The Layer Stack Manager dialog can be accessed from Design » Layer Stack Manager.

Options/Controls

Simple Mode

In its Simple mode, the dialog provides the features and functionality to manage the layers in the stack for a simple, rigid PCB.

Save - Click this button to save current layer stack settings as .Stackup file. Stackup file can be loaded when you create a new PCB.
Load - Click this button to load .Stackup file and apply it to current PCB layer stack.
Preset - Altium Designer provides some reference layer stack settings from two layers to 16 layers. Use this button to quickly load these preset and apply it to your PCB.

Stackup loading and preset loading is not possible if any of the layers are used on the board.

3D - Check this option to show the Layer Stack in 3D mode.
- Click to roll roll layer stack changes backward.
- Click to roll roll layer stack changes forward.
- Click this icon to copy image to Clipboard.
- Click this icon to copy the selected content to Clipboard. Shortcut key is Ctrl + C
- Click this icon to paste the content in Clipboard to target location. Shortcut key is Ctrl + V

Designers are allowed to paste information to external application such as Microsoft Excel

Layer Stackup Style - Changing the layer stack up style changes the way that the core and pre-preg layers are distributed through the layer stack. Defining the stack up style is only required if you plan to use blind and buried vias and for signal integrity analysis. Select one of the following layer pairs for this layer stack up:
- Custom
- Layer pairs
- Internal Layer pairs
- Build up

Use this option to select the technology that will be used to build the board, the available options include: Layer Pairs, Internal Layer Pairs, Build-up or Custom. Note that this option does not affect the final design of the layer stackup, it is simply used to help select the appropriate type of dielectric layer to add and the location in the stack where it is added, when you run an Add Layer command. In all modes other than Custom, whenever a signal layer is added, a dielectric layer will also be added. The type and location of dielectric added depends on: the current number of layers used, and the current Style setting. Note that once a second layer Stack has been added, the Style is automatically set to Custom. In Custom mode, new layers are added one-by-one.

Add Layer - Click to open a pop-up menu, from which to select and add desired layers, including Signal Layer, Internal Plane, Dielectric Layer, Overlay, Solder Mask. In simple mode, Add Layer is quite straight forward. While in Rigid-Flex, it'll be a little bit complicated. We'll discuss the control in Advanced Mode later.
Delete Layer - Click to open a pop-up menu, from which to delete target layers.
Move Up - Click to move the selected layer upward.
Move Down - Click to move the selected layer downward.
Drill Pairs - Click to create drill pairs for this PCB document. If a PCB design includes blind and buried layers then the drill pairs must be defined to suit the layer stack style. By default a board with no blind and buried vias has only one drill pair comprising the Top and Bottom layers. The drill pair refers to the two layers that a drilling operation starts from and stops at. You can generate drill pairs from the layer stack or from the existing vias of the PCB design.
Impedance Calculation - Click to calculate the impedance and trace width for microstrips and striplines. The calculations rely on the physical order of signal layers and planes and physical height of copper layers and dielectrics. This can be used for accurate impedance controlled routing with the design width constraint rules.
Advanced - Click this button to switch to Advanced Mode.

Layer Properties

Top/Bottom/Signal Layer

Name - Specify a name for the layer.
Copper Thickness - Specify the copper thickness for the selected signal layer.
Orientation - Specify the direction of the embedded components in singal layer, options include: Top, Bottom, None. This can be overridden if needed at the individual component level, by enabling the Flipped on Layer checkbox in the Component properties dialog.

Dielectric Layer

Name - Specify a name for the layer.
Type - Specify the Solder Mask type, options include: Surface Material,Prepreg, Core, None.
Material - Specify the mask layer material.
Thickness - Specify the thickness of the layer.
Dielectric Constant - Specify the dielectric constant of the solder mask material.

Internal Plane Layer

Name - Specify a name for the layer.
Copper Thickness - Specify the thickness of the layer.
Pull Back - Specify the pullback value for internal plane.

Solder Mask Layer

Name - Specify a name for the layer.
Type - Specify the Solder Mask type, options include: Surface Material,Prepreg, Core, None.
Material - Specify the mask layer material.
Thickness - Specify the thickness of solder mask.
Dielectric Constant - Specify the dielectric constant of the solder mask material.

Overlay

Name - Specify a name for the layer.

Layer Stack Preview - Shows the graphical preview of the current layer stack up.

Advanced Mode

For rigid-flex PCBs, you need to get at controls for adding and managing multiple sub-stacks. This is performed by entering the dialog's Advanced mode.

In Layer Stack Manager dialog, below controls are enhanced or added for this purpose.

Stack Layout

Layer Stackup Overview - Shows the graphical preview of multiple sub-stacks in current design.
Add Stack - Click to add a new sub layer stack, which can be assigned to different board regions in Flex-Rigid design.

Select an existing layer and click Add Layer button to add a new layer stack. The properties of the new layer stack will be identical to the source stack

Delete Stack - Click to delete a selected sub layer stack.
Show Stacks Option - Click to select the stacks you want to show
- Show All Stacks
- Show User Stacks
- Show Managed Stacks
Move Left - Click to move the selected sub layer stack to left.
Move Right - Click to move the selected sub layer stack to right.

Stack Properties

Name - Specify the name of the layer stack. Each stack should be named to uniquely identify it, this helps it to be correctly applied to a user-defined board region.
Flex - Enable this option for Rigid-Flex design. Each stack that is flexible needs to have its Flex option enabled, so that required flex bending properties can be applied.
Stack In Use - If the check option is ticked, it indicates selected stack is in use in current design.
Managed - Check this option to set selected stack layers to be managed

Each stack that is flexible needs to have the Flex checkbox enabled, so that required flex bending properties can be applied.
Note that flex bending is defined by placing a Bending Line across the flex region (Press 1 to enter into rigid-flex defining mode and choose Design » Board Shape from menu), and then editing its properties in the PCB panel when the panel is set to Layer Stack Regions mode.

Add Layer - Click to open a pop-up menu, from which to select and add desired layers, including Signal Layer, Internal Plane, Dielectric Layer, Overlay, Solder Mask. New layers are always added to the selected stack.

The currently selected stack has its name highlighted with a blue background, in the stack region of the dialog

Simple - Click Simple button to switch to Simple Mode.