Including Design Details

Now reading version 22. For the latest, read: Including Design Details for version 24
Applies to Altium Designer version: 22
 

Many of the outputs that you generate will require additional details. For example, the manufacturing drawing will need dimensions, the assembly drawing might need an enlarged view of a specific area of the board, and the fabrication drawing will need a Layer Stack Table and a Drill Table. These types of detail can be added in the PCB editor or in the PCBLIB Editor via footprint.

Note that while a PCB design can be documented right in the PCB editor, the software also includes an advanced, yet flexible graphical editing environment for creating board design production documents, called Draftsman. Complete with a dedicated set of drawing tools, the Draftsman drawing system provides an interactive approach to bringing together fabrication and assembly drawings with custom templates, annotations, dimensions, callouts, and notes.

Learn more about Draftsman

General Purpose Drawing Layers

In the PCB editor, detail such as dimensions, and fabrication and assembly instructions are added on mechanical layers. The software supports an unlimited amount of general purpose mechanical layers, which are enabled in the View Configuration panel. These layers can be named as required (right-click on the name then select Edit Layer), and included in printouts and layer-based fabrication outputs.

To learn more about mechanical layers, see Working with Mechanical Layers.

Layer Stack Table

A Layer Stack Table can be placed on a PCB document alongside the design itself. It provides a detailed summary of the board layer stackups and how the layer groups are assigned.
A Layer Stack Table can be placed on a PCB document alongside the design itself. It provides a detailed summary of the board layer stackups and how the layer groups are assigned.

A Layer Stack Table is a tabular graphic object that documents the layers, materials, thicknesses, and dielectric constants implemented in the current PCB design. It is placed and positioned alongside the board design in the design space and also includes a graphical key and option map that shows the layer stack used in each region of the board. A Layer Stack Table is an important documentation asset for designs with a complex layer stack structure, such as a rigid-flex design.

The Layer Stack Table is available in the PCB editor when the design space view is set to normal 2D mode (shortcut 2). After launching the Layer Stack Table placement command, the cursor will change to a cross-hair and you will enter Layer Stack Table placement mode. Placement is made by performing the following sequence of actions:

  1. Click to place the table.
  2. The editor remains in Layer Stack Table placement mode, ready to place another table if required. If not, right-click or press Esc to exit placement mode.
Note the Board Map that appears below the table. This is an outline of the board showing how the various layer stacks are assigned to regions of the board. The Board Map can be disabled or scaled by using the Show Board Map option in the Layer Stack Table mode of the Properties panel.

Additional actions that can be performed during placement while the layer stack table is still floating on the cursor and before the center point of the layer stack table is anchored are:

  • Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement. 
  • Press the Spacebar to rotate the layer stack table counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in increments of 90°.

To move a Layer Stack Table, click, hold and drag the table to the desired location.

Select and drag to reposition a Layer Stack Table.
Select and drag to reposition a Layer Stack Table.

Drill Table

The Drill Table presents a live summary of all drill holes present in the board
The Drill Table presents a live summary of all drill holes present in the board

A drill table is a standard element required for the manufacture of a Printed Circuit Board. The drill table lists the size and number of holes for each drill used on the board. Each drill size can be represented by a symbol, a letter, or the actual hole size. When a drill drawing is generated for the board, each actual drill site is marked by a symbol. The drill table updates in real-time as hole-containing objects, such as pads and vias, are placed or removed from the PCB design.

A Drill Symbol is displayed at each drill site on the Drill Drawing layer when the Show Drill Symbols option is enabled in the Drill Symbols dialog.

A Drill Table can be placed only in the PCB Editor. After launching the command, a drill table will appear attached to the cursor. Position the table in a suitable location outside the board then click or press Enter to place it.

Note that the drill table must be placed on the Drill Drawing layer. It will be automatically placed on the Drill Drawing layer even if this is not the currently active layer.

Additional actions that can be performed during placement while the drill table is still floating on the cursor and before the drill table is anchored are:

  • Press the Tab key to pause the placement and access the Drill Table mode of the Properties panel, from where its properties can be changed on the fly. Click the pause button overlay ( ) to resume placement.
  • Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement. 

Moving a Drill Table

Click and hold anywhere within the drill table then move it to the desired location in the PCB editor design space.

Interactively Resizing a Drill Table

The drill table is automatically sized based on the specified Text Height setting, as well as the number of different hole sizes (rows) and the number of defined columns. To interactively resize the table, click once to select it then click and hold on a corner vertex then move to resize as required. Note that interactively resizing the table will also increase/decrease the font size.

Interactively Switching the Layer Pair to Preview

When the board includes layer-pairs, the displayed layer-pair is controlled by the Layers Pairs option in the Drill Table mode of the Properties panel.

This chosen layer-pair also can be switched using the:

  • PCB Editor right-click menu - right-click on the Drill Table then select the required layer-pair in the Drill Table sub-menu as shown in the image below.

    Right-click on the Drill Table to switch it to display another layer-pair
    Right-click on the Drill Table to switch it to display another layer-pair

  • Layer-pair selection menu accessed via the Layer Tab at the bottom of the design space as shown in the image below.

Drill Table Properties

The Drill Table mode of the Properties panel.
The Drill Table mode of the Properties panel.

Location

The  icon to the right of this region must be displayed as   (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status.
  • (X/Y) – the current X and Y locations of the Drill Table reference point. The reference point is the bottom left corner if Alignment = Bottom, or top left corner if Alignment = Top.
  • Rotation – angle in degrees that the Drill Table is rotated.

Properties

  • Layer Pairs – the drill table supports multi-layer boards that use layer-pair drilling. Use the drop-down to select a layer pair defined on the Via Types tab of the Layer Stack Manager or one of the following options:  
    • All Layer Pairs (Composite table) – displays information for all layer pairs.
    • All Layer Pairs (Separate tables) – displays information for each layer pair in a separate table.

      When this option is selected, the separate tables for different layer pairs are displayed overlapped. When generating the outputs, the drill table for a corresponding layer pair will be produced. For showing the drill table for a specific layer pair in the PCB editor design space, you can select the layer pair from the menu of the icon at the right of the Drill Drawing layer tab at the bottom of the design space.

    • Top - Bottom – only show the thru-holes.
    • Counterhole Bottom – only show the counterholes (counterbores/countersinks) on the bottom side of the PCB.
    • Counterhole Top – only show the counterholes (counterbores/countersinks) on the top side of the PCB.
    The Counterhole Bottom and Counterhole Top options are available only when the design includes Pad objects with Counterhole features enabled on corresponding sides of the PCB.
    Note that counterholes are excluded from layer pairs other than Counterhole Bottom and Counterhole Top, including All Layer Pairs (Composite table) and All Layer Pairs (Separate tables).
  • Text Height – displays the text height.

Font Type

  • TrueType – select to use fonts available on your PC (in the \Windows\Fonts folder). TrueType fonts offer full Unicode support. By default, the software links to a used TrueType font (they are not stored in the PCB file), which means the same font must be present on each PC that the design is moved to. Alternatively, embed used TrueType fonts in the PCB file using the options in the PCB Editor – True Type Fonts page of the Preferences dialog, where you can also select a Substitution Font to be used if a non-embedded Font is not available.
    • Font – use the drop-down to select the desired TrueType font. Use the B to bold or I to italicize text.
  • Stroke
    • Font – use the drop-down to select the desired Stroke font. Choices are:
      • Default – a simple vector font designed for pen plotting and vector photo plotting.
      • Sans Serif
      • Serif
    • Stroke Width – displays the width of the stroke.
  • Show Footer – toggle to enable/disable displaying the footer of the table.
  • Alignment – the table can be built from the bottom-up (Bottom), or from the top-down (Top). Use this setting to allow for table size changes without impacting surrounding objects in the design space.
  • Table Border Width – width of the lines used to create the table border.
  • Drill Symbols – click to open the Drill Symbols dialog in which you can assign symbols/letters to hole sizes.

  • – click to refresh the table whenever there are design changes that affect the drill table. Note that the table is automatically updated during output generation.

Units

  • Primary Units – use the drop-down to set the primary units to either Metric (mm) or Imperial (mil).
  • Dual Units – use the drop-down to set the dual units to either Metric (mm) or Imperial (mil). Use  or  to determine whether these units are displayed or hidden (respectively) in the design space.

Precision

  • Primary Precision – use the drop-down to set the required precision (number of digits after the decimal point).
  • Dual Precision – use the drop-down to set the dual precision (number of digits after the decimal point).

Columns

  • Grid – displays all column headings (Caption) in the drill table, the Align setting, which repositions contents within the grid, the Width, and the Order in which the information in each column is displayed. To change from ascending to descending order and vice versa, click in the Order column to access a drop-down menu then select the desired order: Asc – ascending or Dsc – descending.
  • Edit Columns – click to open the Columns dialog, with which to add new columns to the drill table or edit existing columns.

The dialog presents all existing columns, along with associated (read-only) data. Use the following buttons beneath the grid to curate the data to be presented in the table:

  • Add Column - use to add a new colum to the drill table. Click to open a menu of available columns. Columns that are already used or not available are grayed-out in the menu. This command also is available on the right-click menu.
  • Remove Column - click to remove the selected column(s). Note that there is no confirmation dialog; when the button is clicked, the column is deleted. This command also is available on the right-click menu.
  • Change Header - click to open the Change column header dialog in which you can change the title of the selected column. This command (titled Change column header) also is available on the right-click menu.

The following additional commands are available from the right-click context menu:

  • Text Alignment - use to align the text in the selected column. Choices include: Left, Center, and Right.
  • Set column width - use to set the width of the selected column. Choices include:  Autosize (default), and Manual.  Clicking Manual opens the Set Column Width dialog in which you can enter the desired width.

Design View

Place a Design View to show a specific area of the board. This example has been scaled to 200%.
Place a Design View to show a specific area of the board. This example has been scaled to 200%.

The PCB Design View object is a graphic snapshot of any rectangular-shaped region of the current board or another board. It can be placed anywhere in the design space and scaled to any size.

A Design View can be placed only in the PCB Editor. After launching the Design View placement command, a design view will appear attached to the cursor. Position the design view in a suitable location then click or press Enter to place it.

Additional actions that can be performed during placement while the design view is still floating on the cursor and before the design view is anchored are:

  • Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.

After placement of the design view, you can define the display of desired layers by performing the following steps:

  1. With the Design View selected in the design space, open the Properties panel by double-clicking or right-clicking then choosing Properties from the context menu.
  2. Use the Define button in the Properties panel to interactively define the area of interest.
  3. In the Layers section of the Properties panel, click (toggle) the  icon to enable the display of the desired layers. When enabled in the Properties panel, the desired layer(s) will display the   icon.

Design Views are included in printed and PDF output. The Design View retains its own layer visibility settings in the output allowing it to present as required in the printed/PDF output. Note that the primitives on layers used in the Design View continue to obey the display settings defined for that layer in the Print dialog. For example, if the Top Overlay is displayed in the Design View and the Top Overlay is configured to display tracks in Draft mode for that output in the Output Job, then the Top Overlay tracks in the Design View will also present in Draft mode.

Note that Design Views are not included in Gerber or ODB++ output.

Once a Design View has been placed in the design space, you can interactively adjust the position, scale, size and focus of the View.

  • Change the positionClick+Drag the Design View object to a new location on the PCB design space.
  • Adjusting the Scale – click once to select the Design View then Click+Drag on a corner handle to scale the Design View up (drag out) or down (drag in).
  • Adjusting the View Size – click once to select the Design View then Ctrl+Click+Drag on a corner handle to resize the Design View.
  • Changing the Focus – Ctrl+Click+Drag anywhere within the Design View to slide the currently viewed area around within the Design View window.

Ctrl+Click+Drag to slide and adjust the area currently being viewed in the Design View.
Ctrl+Click+Drag to slide and adjust the area currently being viewed in the Design View.

OLE Object

A placed sequence of OLE objects – an image, spreadsheet cells and word document text (top to bottom)
A placed sequence of OLE objects – an image, spreadsheet cells and word document text (top to bottom)

Object Linking and Embedding (OLE) technology in the PCB editor allows data supplied by Windows OLE applications to be embedded in a PCB design while actively linking back to the source application. In many cases, this allows the embedded PCB data to be edited from within the application that created it.

Typical OLE objects that might be placed in a PCB document include common Excel documents, Word documents, or graphics objects from a suitable OLE image application. The supported file types include universal formats such as CSV and XLS format spreadsheets, DOC and RTF word documents, and BMP image files.

OLE objects are available for placement/embedding in the PCB Editor. After launching the command, choose the desired file from the Choose File dialog then click to place the object in the design space. 

Altium’s Smart Paste capability also allows a selection in an OLE application to be copied and pasted (Edit » Paste) into the PCB document as an OLE object. The text paste option (Edit » Paste Text) can be used to strip the text elements from an OLE object if required. These will be placed as PCB text objects.

Once placed, embedded objects can be proportionally scaled by clicking, holding and dragging their selection handles. With text-based objects such as Word and Excel documents, the embedded text is automatically scaled in size and thickness to suit the new dimensions.

  • An OLE Object also can be converted to a collection of free primitive objects using the Tools » Convert » Explode OLE Object to Free Primitives command. This will break the object into appropriate Regions and/or Text objects.
  • A convert to free primitives option is also offered if the matching OLE application cannot be found when attempting to edit an OLE Object.

Dimensions

The PCB editor includes a range of dimensioning tools, available in the Place » Dimension sub-menu. As you place a dimension, click on an existing object to attach the reference point to that object (press Shift+E to cycle through the object snap-to modes). The dimension will remain attached if that object is moved. Dimensions have a range of configuration options, offering a high-level of customization of the arrows and text.

A dimension's value (where applicable) automatically updates as its start or end points are moved. Likewise, if the position of an object that a reference point of the dimension is anchored to is changed, the dimension will update and expand/contract to reflect this. For a radius/diameter-based dimension, the value automatically updates as the diameter of the reference arc or circle changes.

When the reference or references to which a dimension object is attached are deleted, a dialog will open asking whether the dimension should also be deleted. If the dimension is not deleted, it remains in the design space, but non-referenced.

When dimensioning an object, anchor points become available to you that highlight where the dimension can be attached. The point nearest the cursor will be the one used and where the dimension will attach if you proceed to click or press Enter. The Status bar displays information about the actions needed for each step throughout the process.

A variety of dimension objects are supported to cater for different design requirements. Dimension objects are comprised of one or more string and track segments. A dimension can be converted to its constituent primitive objects using the Tools » Convert » Explode Dimension to Free Primitives command.

Note

The features available depend on your level of Altium Designer Software Subscription.

Content