Technology - Layer Class

Layer Classes define what type of Layers you can have in your design and what they can be used for.

Shortcuts

Menu: Setup

Default Keys: T

Command: Technology

Locating this option

Available from: Setup menu > Technology option > Layer Class tab

Using the Layer Class dialog

On selection, the Technology dialog opens, select Layer Class. The existing Layer Class for the Technology being used will be presented.

Navigation

The buttons to the right side of the dialog are used to navigate the grid, the general common buttons are detailed on the Technology Navigation page.

Using the editing pane

This dialog gives a list of the defined Layer Classes in the design. A Layer Class will normally have a descriptive name, such as Silk Screen which will give you an idea of what it would be used for.

Layer Class Name

A Layer Class must have a unique Name, this is used to reference the Layer Class. You should choose a descriptive name.

Reset To Default

The Reset to Default button will reset all the settings on this dialog back to their ‘factory’ settings. Pulsonix has a set of factory defaults that have been pre-programmed to match an expected ’ normal’ set of conditions for each particular layer class type. This option is described in more detail on the Reset To Default help page.

Layer Type

The Layer Type is one of the following list. You cannot change the Layer Type, once the Layer Class has been used, as this would affect the integrity of the design.

• Construction

  Construction layers are Non-Electrical physical layers, you cannot put anything on these layers. These would be used if you wished to fully document the layer stack and would be positioned between the Electrical layers. Examples would be laminates and epoxy resin.

• Documentation

  Documentation layers can contain text and figures which are not directly related to the position of any physical design items. Examples would be drill tables and design notes.

• Drill Drawing

  Drill Drawing layers are for displaying drill letters and symbols and other drill information. When you create a Drill Drawing layer, you will need to associate a Layer Span, and specify what types of Drill Holes should be displayed (Plated / Non Plated, Round / Non Round).

• Electrical

  A layer of type Electrical would normally be a conductive layer and would contain tracks, copper areas, lands, etc. Power Planes are also of type Electrical. You would typically have a Top, Bottom and an even number of Inner Electrical layers. You can create more than one Electrical Layer Class if you wish.

  You can also use electrical layers to represent other layers that will not form part of the physical layer stack, see Physical Copper Layer below for details.

• Non-Electrical

  A Non-Electrical layer would normally have documentation text and figures which correspond with physical items such as Components. Examples would be Silk Screen and Assembly layers. You would typically have a Top and a Bottom layer for each one of these classes.

• Wire

  Wire layers would normally be used for layers that are used for jumper wires or bond wires. These are very limited and used for special ‘wire’ items.

Essential For Manufacture

If a Footprint contains items on an Essential layer, it cannot be added to a design which does not contain a matching layer. Similarly, items on non-essential layers will not be added to a design without a matching layer, but the Footprint itself can still be added. This can be useful for construction lines, dimensions or alternative outlines.

Physical Copper Layer

This check box is only shown if the type is Electrical. Most electrical layers must have this box checked as they represent a physical copper layer in the construction of the final board.

Uncheck it if you need an electrical layer that represents something else, for example an inner layer to display embedded component die pads on. These layers need to be electrical so that a layer span can be created to take micro vias down to the die pads.

Pad Oversize

You can provide an oversize for the given layer, the oversize can be negative, giving an undersize. The oversize is in the current design units (Absolute Size), or as a percentage of the width of the pad (Percent of Pad Size). This would normally be used for Non-Electrical layers such as, Paste Mask or Solder Resist layers where the size of the pads must be adjusted for the manufacturing process.

Note that the oversizing is applied all around the pad, so an oversize of 5 thou would make the pad 10 thou wider and longer. Similarly a 5% oversize would make a pad 10% wider and add the same amount to the length.

Min Undersized Pad

When pads are undersized, you can specify a minimum size. The Pad Undersize can be checked using the Design Rule Checker. The size is in the current design units. This is only relevant when you provide a negative Oversize.

Board Visible

You can decide if the Board Outline will be plotted on this layer. This is relevant for Electrical and Non-Electrical layers.

Merge Cutouts, during post processing, will cause the Board Outline to be merged with any Area Board Cutouts (Plated or Unplated) which would be visible on this layer. This is important if any of these areas overlap the board edge.

Pad Types

On Non-Electrical layers, you can control what types of Pads will be plotted. This is used in combination with the Pad Condition and Pad Appearancesections to customise which Pads are plotted and how they are plotted. It is also used to select which pads are used in the Break Shapes option.

Pad Condition

For Non-Electrical layers, you can control which Pads are plotted according to the type of pad. So you can choose not to plot Surface Mount pads by unchecking the Surface Mount check box. Or you can ONLY plot pads which are TestPoints by checking the Only If Testpoint check box.

The Exception Only check box will cause only pads which have an explicit pad shape assigned to that layer to be drawn. This is useful if you only want pads with specific pad styles to appear on a layer.

Draw/Plot Appearance

For Non-Electrical layers, you can choose to plot the Pad Land, its Drill Hole, or both, subject to the conditions specified. If you uncheck both these, the pad does not appear, but it is still selected for the Break Around Pad option.

Areas Visible

You can decide if the Areas will be displayed on this layer. This is relevant for Electrical and Non-Electrical layers. For components, you can decide which types of areas are shown on this layer. You can also decide if Plated or Unplated Board Cutout areas are displayed.

Note that if an area is on a specific electrical layer, rather than on a set of layers, it will always be displayed even if areas are disabled in the layer class.

Design

Use the Design check box to display areas that have been added at the design level. This would all areas not defined within a component.

Board Cutouts

Use the Unplated or Plated check boxes to display Board Cutouts Areas that have a plated status defined as plated or unplated on this layer.

Break Shapes

For Non-Electrical layers, you can choose to break documentation shapes around, pads or text. The pads are selected using the Pad Types and Pad Condition described above.

For example, you may want to break silkscreen shapes around drilled component pads. You should therefore enable Component Pads in the Pad Types section and the Plated Through Hole in the Pad Conditions (because these are the shapes you wish to avoid), but disable Pad Land and Drill Hole (because you do not want these pads to actually appear on the silkscreen layer). Finally enable Break Around Pad and specify the Gap.

If you want the silkscreen outlines to break around text items (such as the component names), you should enable the Break Around Text option.

Use Break Comp Shapes At Board to specify that documentation shapes are truncated to the board outline. For example, use this to stop silkscreen shapes from being plotted outside of the board.

Shapes are only broken for post processing, they appear unbroken when displayed on screen.

The Gap defines how far from the pad or text the shape is broken off.

Variant Components

Items Visible In All Variants - Determines whether items of this layer class are visible for not fitted components when using variants. For Electrical layers this will always be true, but for Non-Electrical layers it will default to unchecked, but may be changed if you wish to make items of a given layer class visible for not fitted components.

If a shape is visible when not fitted, it can be drawn with the special Variant line style defined on the Variant Defaults Page by checking the Use Variant Style option.

Layer Mask

Min Mask Width - Thin sections of solder mask can cause problems in the manufacturing process. Use this option to set a minimum distance between openings in the layer mask required across the entire board. This value is used in the Solder Mask Width DRC check.

Min Mask To Track - Misalignment of the solder mask can cause a short circuit by exposing a track. Use this option to set a minimum distance between openings in the layer mask and tracks that could be exposed. This value is used in the Solder Mask To Track DRC check.

Panel

Use these check boxes to include items that appear on layers that use this Layer Class in DRC checks performed using the Panel Items In Design check.

The two Panels check boxes allow Check Items Outside Board to be flagged during checking and the ability to Draw Shapes in Panel Designs when they appear on a Layer that uses this Layer Class. It means shapes can appear in the design but will not be used if the design is used within a Panel.

Protecting Vias

Tented Vias (Type I Via)

Vias can be protected where required and according to the IPC-4761 standards.

There are two approaches to defining vias within a design if they require ‘tenting’, where the dry film resist totally covers the via and its hole, thus sealing it (Note; The result can be dependent on the hole size, so it is advisable to consult the board manufacturer before design). The mask can be applied to one side (Type I-A) or both sides (Type I-b).

One method is where this is required for EVERY via in the design, the other is where it is only applied to individual vias:

Every Via on every Mask Layer:

• The method is to remove Vias from the Pad Type by deselecting them from the Solder Resist Layer Class, (or from a new specific Layer Class). This will mean that the system will NOT process resist in the output for any vias for every resist layer output.
• Using the above method, you can also have a different Layer Class for the Top and Bottom electrical layers so that Via output can be restricted.

Individual Vias or every Via, but Mask Layer controllable:

• The method is to add a By Layer to every Pad Style (Via Style) being used for vias for each solder resist layer, and making the size of the pad zero width. With this approach, you could have ‘tented’ on one solder resist layer only. The Plot Drilled Out Pad Holesoption would need to be deselected on the Output tab in the CAM Plot Wizard for the Resist layer.

Plugged Vias (Type III Via)

The via is partially filled with a conductive (solder) or non-conductive (epoxy) media. This can be applied to one side (Type III-A) or both sides (Type III-b).

The method used for defining plugged vias will be the same as for Tented vias above.

Layer Stiffeners

When creating flexi-boards, you may require a Stiffener to be added along with Stiffener glue. To do this, create two new layer classes; one for the actual Stiffener, and one for the ‘glue’ layer. The layer stack created in the Layersdialog would then use these special non-electrical layer classes.

The actual Stiffener layer would have a shape added to it to indicate the Stiffener material. The glue layer may have a shape or may be a whole layer, that depends on your manufacturing.

Units

The Units button allows you to locally switch between Metric and Imperial units whilst in this dialog. Once the dialog is closed, the units revert back to the original design units. If switching to different units to the design units, the value typed will be converted when you next enter this page.

Related Topics

Technology Overview | Using Dialog Grids | Technology - Layers | Technology - Materials | Suppress Lands Rule