Tutorial - Creating the PCB Drawing in Altium Designer

Main page: Streamlining Board Design Documentation with Draftsman

Altium Designer's Draftsman editor provides tools for creating multi-sheet fabrication and assembly drawings in an automated manner based on the project's PCB document.

Adding and Configuring a New Draftsman Document

Main page: Setting Up a Draftsman Document

To start creating a new drawing, you need to add a new Draftsman document to the project.

1. Right-click the project entry in the Projects panel and select the Add New to Project » Draftsman Document command from the context menu.

   

2. The New Document dialog will open. Select the [Default] entry in the Templates list and make sure that the correct project and PCB document (Multivibrator.PrjPcb and Multivibrator.PcbDoc) are selected in the Project and Document drop-downs.

   

3. Click OK in the dialog. A new blank Draftsman document will open and an entry for it will appear linked to the project in the Projects panel under the Source Documents entry.

   

4. Right-click on the Draftsman document entry in the Projects panel and select the Save As command. The Save As dialog will open, ready to save the document in the same location as the project file. Type the name Multivibrator in the File name field and click the Save button.

5. Adding the Draftsman document has changed the project, so save the project locally by right-clicking the project entry in the Projects panel and selecting Save.

6. If the Properties panel is not visible, click the  button at the bottom right of the design space and select Properties from the menu that opens. The panel displays the properties of the selected object, or if no object is selected, it displays the properties of the Draftsman document.

7. On the Page Options tab of the panel, select Template in the Formatting and Size region, then use the Template drop-down to select the ANSI B Landscape Draftsman template from those that reside in your Workspace.

   

Adding Drawing Views

Main page: Working with Views

Draftsman allows a range of automated production drawings to be placed directly onto a Draftsman drawing document. The drawing data is extracted directly from the source PCB document.

1. Place a board assembly view. To do this:

   1. Select the Place » Board Assembly View command from the main menus.

   2. A top-side board assembly view will be attached to the cursor. Move the cursor to position the view in the top left part of the drawing. Once you are happy with the view's location, click to place it on the drawing.

      If necessary, the location of a view can be changed after placement by using the Click, Hold&Drag shortcut on the view.

   3. Double-click the placed view outside component projections on the view to open its properties in the Properties panel. On the General tab of the panel:

      • Select the 2:1 value from the Scale drop-down in the Scale region.

      • Select the Silkscreen option from the Designator drop-down in the Component Display Properties region. When this option is selected, the position of component designators on the assembly view is defined by the positions of corresponding designators on the overlay layer in the PCB document.

      

2. Place board fabrication views. To do this:

   1. Select the Place » Board Fabrication View command from the main menus.

   2. A top-layer board fabrication view will be attached to the cursor. Move the cursor to position the view at the right of the placed board assembly view and click to place it.

   3. Double-click the placed view to open its properties in the Properties panel. On the General tab of the panel, select the 2:1 value from the Scale drop-down in the Scale region.

      

   4. Place another board fabrication view to show the bottom layer. Select the Place » Board Fabrication View command from the main menus.

   5. Move the cursor to position the view at the right of the placed board fabrication view and click to place it.

   6. Double-click the placed view to open its properties in the Properties panel. On the General tab of the panel:

      • Select the 2:1 value from the Scale drop-down in the Scale region.

      • Select the Bottom Layer option from the Layer drop-down in the Properties region.

      

3. Place a board isometric view. To do this:

   1. Select the Place » Additional Views » Board Isometric View command from the main menus.

   2. Move the cursor to position the view at the right of the placed board fabrication views and click to place it.

   3. Double-click the placed view to open its properties in the Properties panel. In the panel:

      • Select the 2:1 value from the Scale drop-down in the Scale region.

      • Select the Front option from the Face side drop-down in the Properties region.

      

4. Place a layer stack legend. To do this:

   1. Select the Place » Layer Stack Legend command from the main menus.

   2. Move the cursor to position the layer stack legend below the placed board fabrication and board isometric views and click to place it.

   

Annotating the Drawing

Main pages: Drawing Annotation, Dimensioning & Tolerances, Working with Tables

A number of annotation, dimensioning, and other tools are supported to add important information to a Draftsman drawing document.

• Object dimension graphics can be placed on board views to indicate the lengths, sizes, and angles of the object outlines or the distances between nominated objects.

• Industry-standard geometric dimensioning and geometric tolerances symbolic elements that define the manufacturing properties of objects included in a drawing are supported.

• Tables of different types can be placed to convey crucial information for the PCB fabrication and assembly processes in a simple, visual way.

• A range of graphical element tools for placing basic, free-form drawing elements in a document is also provided.

1. Place linear dimensions for the horizontal and vertical size of the board on the board assembly view. To do this (the process is also shown in the video below):

   1. Select the Place » Linear Dimension command from the main menus.

   2. To place the dimension's first reference point, hover the cursor over the top edge of the PCB on the board assembly view and click when the edge is highlighted orange.

   3. To place the dimension's second reference point, hover the cursor over the bottom edge and click when the edge is highlighted orange.

   4. Move the cursor at the left of the view and click to set the position of the dimension text and its associated extension lines.

   5. You will stay in dimension placement mode. Place another dimension by sequentially clicking the left and right edges of the PCB on the board assembly view and clicking below the view.

   6. Right-click to exit dimension placement.

2. Place callouts displaying the BOM positions of the components on the board assembly view. To do this (the process is also shown in the video below):

   1. Select the Place » Annotations » Callout command from the main menus.

   2. Hover the cursor over the edge of the transistor Q1 projection on the board assembly view so it is highlighted and click to place the callout pointer.

   3. Move the cursor at the right of the view and click to confirm the placement of the callout source text.

   4. Identify one more source for the same callout by hovering the cursor over the edge of the transistor Q2 projection and clicking.

   5. Right-click to complete the placement of this callout. You will remain in callout placement mode.

   6. Place callouts for other components on the view as shown below.

   7. When all required callouts are placed, right-click to exit callout placement.

3. Place a BOM table. To do this:

   1. Select the Place » Bill Of Materials command from the main menus.

   2. Move the cursor to position the table below the placed board assembly view and click to place it.

   

4. Save the Draftsman document locally by right-clicking its entry in the Projects panel and selecting Save from the context menu.

5. Close the Draftsman document by right-clicking its tab at the top of the design space and selecting the Close Multivibrator.PCBDwf command from the context menu. 

6. Save the project to the Workspace. To do this, click the Save to Server control next to the project entry in the Projects panel, enter a meaningful comment into the Comment field of the Save to Server dialog that opens (e.g., Drawing is created), then click the OK button.