Layer Stack Manager

Parent page: PCB Dialogs

The Layer Stack Manager dialog.

Summary

This dialog allows the designer to configure and fully define the Layer Stack for the board design. The layer stack comprises all of the layers that are used in the overall PCB design. A variety of types of layers can be included in the layer stack: including copper, dielectric, surface finish and mask layers. Each layer must be completely specified in terms of its material and mechanical requirements, including: the material used, the thickness, the dielectric constant, and so on. The selection of materials and their properties should always be done in consultation with the board fabricator.

For a new PCB document, the default layer stack comprises: a dielectric core, 2 copper layers, as well as the top and bottom solder/coverlay and overlay layers.

Access

The dialog is accessed from the PCB Editor, by clicking Home | Board | , from the main menus.

Options/Controls

  • Save - click this button to save the current layer stackup definition in a Stack-up file (*.stackup). The Save Stack-up dialog will appear, from where you can determine where, and under what name, the file is to be stored.
  • Load - click this button to load a previously saved layer stack definition. The Load Stack-up dialog will appear, from where you can browse to, and open, the required Stack-up file (*.stackup).
  • Presets - click this button to access a menu offering a number of predefined layer stack definitions. Simply choose an entry from the following available, to have it loaded as the layer stackup for the board:
    • Two Layer
    • Four Layer (2 x Signal, 2 x Plane)
    • Six Layer (4 x Signal, 2 x Plane)
    • Eight Layer (5 x Signal, 3 x Plane)
    • 10 Layer (6 x Signal, 4 x Plane)
    • 12 Layer (8 x Signal, 4 x Plane)
    • 14 Layer (9 x Signal, 5 x Plane)
    • 16 Layer (11 x Signal, 5 x Plane)
Ideally, a preset layer stackup should be chosen, or a saved stackup loaded, when the PCB is first created - before any primitives have been placed, and routed. If you attempt to change the layer stack in this way while existing layers are in use, you will be alerted that primitives on those layers will be removed.
  • 3D - enable this option to present a three-dimensional view of the layer stack in the graphical preview region. When copying the layer stack as a bitmap image to the Windows clipbiard, this option determines whether that image is 2D or 3D.
  •  (Undo) - click this button to undo (roll-back) the last performed action in the main Layers region. Click repeatedly to progressively undo changes made.
  •  (Redo) - click this button to redo (reinstate) the last action in the main Layers region to have been rolled back. Click repeatedly to progressively redo changes that have been undone.
  •  (Copy Image to Clipboard) - click this button to copy a bitmap image of the layer stack to the Windows clipboard. The image of the stack will either be 2D or 3D, depending on the state of the 3D option.
  •  (Copy) - click this button to copy the selected cell content, in the main Layers region, to the clipboard.
  •  (Paste) - click this button to paste the clipboard content into target cells of the main Layers region.
Copy and Paste commands are also available from the region's right-click menu, as well as support for standard Ctrl+C and Ctrl+V keyboard shortcuts. Standard multi-select techniques are also supported (Ctrl+click, Shift+click, and Click&Drag). In addition, cell content may be copied to, and pasted from, an external application, such as Microsoft Excel. To include the header information when copying, use the Copy With Header command from the right-click context menu.
  • Layer Stackup Style - use this field to select the style of layer technology to be used on the board. The available options are: Custom, Layer Pairs, Internal Layer Pairs, and Build-up.
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 setting for the Layer Stackup Style.
  • Graphical Preview - this region of the dialog shows a graphical representation of the current layer stack. The view can be switch from a two-dimensional representation, to a three-dimensional one, by enabling the 3D option. The preview can be copied to the Windows clipboard as a bitmap image, by clicking the  button.
  • Layers - this region of the dialog lists all of the layers currently defined in the layer stack, in tabular format. The properties of each layer are edited directly within this region of the dialog. To edit a cell double-click on it, if that cell supports editing it will become available for editing. The following is a summary of the layer types, and the properties that must be defined:
    • Signal Layer - Layer Name, Thickness.
    • Dielectric Layer - Layer Name, Material (None, Core, Prepreg, or Surface Material), Thickness, Dielectric Material, Dielectric Constant.
    • Internal Plane Layer - Layer Name, Thickness, Pullback.
    • Soldermask Layer - Layer Name, Material (None, Core, Prepreg, or Surface Material), Thickness, Dielectric Material, Dielectric Constant.
    • Overlay - Layer Name.
Thickness is defined in either mils, or mm, in accordance with the measurement unit employed for the board, as determined by the  and  buttons in the Home | Grids and Units area of the main menus.
The selection of materials and their properties should always be done in consultation with the board fabricator.
  • Total Thickness - this field reflects the total thickness of the board, which is simply the sum of the thicknesses of the individual layers in the stack (signal, internal plane, dielectric, and soldermask layers).
  • Add Layer - click this button to access a menu of layer types that can be added to the layer stack. Choose the layer you wish to add from the following options:
    • Add Layer - adds an internal signal layer to the stack. For all Layer Stackup Styles other than Custom, an associated Dielectric layer will also be added.
    • Add Internal Plane - adds an internal plane layer to the stack. For all Layer Stackup Styles other than Custom, an associated Dielectric layer will also be added.
    • Add Overlays - adds Top/Bottom Overlay layers, and Top/Bottom Solder Mask layers (or remaining layers that are missing if not present in the stack already).
    • Add Dielectric - this command is only available when the Layer Stackup Style is set to Custom. use it to add a Dielectric layer to the stack.
Commands for adding the different layer types to the stack are also available from the region's right-click menu.
  • Delete Layer - click this button to remove the currently selected layer(s) from the layer stack.
The Top and Bottom signal layers cannot be deleted. Their associated core Dielectric layer (by default, named Dielectric 1) can also not be deleted, unless the Layer Stackup Style is set to Custom.
Layer removal can also be performed from the right-click menu, using the Delete Layer command.
  • Move Up - click this button to move the selected layer upward in the stack.
  • Move Down - click this button to move the selected layer downward in the stack.
Commands for moving the selected layer up or down in the layer stack are also available from the region's right-click menu - Move Layer Up and Move Layer Down, respectively.
  • Drill Pairs - click this button to access the Drill-Pair Manager dialog, from where to configure the required drill pairs for the board. Drill pairs must be configured when blind, buried, or build-up type vias are to be used, with a drill pair for each layer-pair that a via spans. It is the presence of drill pairs that lets the system know that blind and/or buried vias are in use. This ensures that when the fabrication output files are generated from the completed board, there are suitable drill files for the various drill jobs that must be performed to create the blind and/or buried vias.
Once the drill pairs have been defined, suitable blind, buried or thru-hole vias are automatically placed during routing, in accordance with the drill pair settings, and the applicable Routing Via Style design rule.
  • Impedance Calculation - click this button to access the Impedance Formula Editor dialog, from where you can view and modify, if required, the formulae used to calculate Impedance and Trace Width, when using impedance-controlled routing. Calculations are made for both Microstrip (a route has a plane layer present on only one side of it) and Stripline (a route has planes present on both sides of it) type traces.

 

You are reporting an issue with the following selected text and/or image within the active document: