Welcome to the Bartels Group of Companies
Layouterstellung - Deutsche Version Designing PCB Layouts - English Version
Bartels

Bartels System GmbH
Bartels
Bartels AutoEngineer
BAE Product Info
BAE Price List
BAE Downloads
BAE Documentation
BAE Installation Guide
BAE User Manual
Preface
1 Introduction
2 Circuit Design
3 Packager
4 PCB Design
4.1 General
4.2 Layout Library Symbol Design
4.3 Designing PCB Layouts
4.3.1 Creating and Editing PCB Layouts
4.3.2 Parts, Placement
4.3.3 Text and Graphic
4.3.4 Traces, Routing
4.4 Autoplacement
4.5 Autorouter
4.6 Special Layout Features
4.7 CAM Processor
4.8 CAM View
5 IC/ASIC Design
6 Rule System
7 Utilities
BAE Libraries
User Language Programmer's Guide
BAE Update History
BAE Next Version Release Notes Preliminary
BAE V8.0 Release Notes
BAE V7.8 Release Notes
BAE V7.6 Release Notes
BAE V7.4 Release Notes
BAE V7.2 Release Notes
BAE V7.0 Release Notes
BAE V6.8 Release Notes
BAE V6.6 Release Notes
BAE V6.4 Release Notes
BAE V6.2 Release Notes
BAE V6.0 Release Notes
BAE V5.4 Release Notes
BAE V5.0 Release Notes
BAE V4.6 Release Notes
BAE V4.4 Release Notes
BAE V4.2 Release Notes
BAE V4.0 Release Notes
BAE V3.4 Release Notes
BAE Support
BAE Contributions
BAE Development and Service Companies
Electronics Development
Bartels Sport Service
Company Profile
Corporate Info
Bartels :: Bartels AutoEngineer :: BAE Documentation :: BAE User Manual :: PCB Design :: Designing PCB Layouts
Bartels AutoEngineer® - User Manual

4.3 Designing PCB Layouts

Bartels AutoEngineer® Dokumentation

The layout level is the top hierarchy level of the BAE PCB design system database. On layout level, the PCB contour is defined, the parts (from the subordinate layout part level) are placed, keepout areas, power planes and copper areas are defined, the traces are routed and, finally, the CAM output is generated. Drawing items and text can be created on layout level for such things as plot registration markers, measurement, project identification, etc.

This section explains how to use the basic functions for creating layouts, placing parts, creating text and documentary graphic and performing manual routing. A layout named board will be created in the demo.ddb DDB file, and the layout symbols generated in the preceding chapters will be used on that layout.

Use the following commands to move to the BAE examples directory (i.e. where the example job file demo.ddb resides, e.g., c:\baejobs) and start the Bartels AutoEngineer:

>  C: Return/Enter Key (CR) 
>  cd c:\baejobs Return/Enter Key (CR) 
>  bae Return/Enter Key (CR)

Move the menu cursor to the Layout menu item and confirm this choice by pressing the left mouse button:

LayoutLeft Mouse Button (LMB)

The Layout Editor is activated and you can start to edit PCB layouts.

 

4.3.1 Creating and Editing PCB Layouts

Creating a new Layout

Use the following commands to create a new layout in the demo.ddb DDB file with an element size of 3.2*2.9 inch:

FileLeft Mouse Button (LMB)
NewLeft Mouse Button (LMB)
LayoutLeft Mouse Button (LMB)
File Name ?demo Return/Enter Key (CR)
Element Name ?board Return/Enter Key (CR)
Element Width (mm/") ?3.2" Return/Enter Key (CR)
Element Height (mm/") ?2.9" Return/Enter Key (CR)

A frame designating the element boundaries of the layout appears on the screen. If the system issues an error message such as Element does already exist!, then a layout with the specified element name has already been generated. In this case, the requested element cannot be created, but must be loaded (see below). It is strongly recommended to specify a layout element name identical to the name of the net list for which the layout should be designed, because otherwise the system won't be able to correlate the layout data with the net list definitions.

Use the following commands to store the new layout element and return to the BAE main shell:

FileLeft Mouse Button (LMB)
Save ElementLeft Mouse Button (LMB)
FileLeft Mouse Button (LMB)
Main MenuLeft Mouse Button (LMB)

Editing an existing Layout

Call the Layout Editor again, and use the following commands to reload the previously created layout element (you are now accessing an existing element; thus you can select the file and element name via popup menu and mouse-pick):

FileLeft Mouse Button (LMB)
Load ElementLeft Mouse Button (LMB)
LayoutLeft Mouse Button (LMB)
File Name ?demo Return/Enter Key (CR)
Element Name ?board Return/Enter Key (CR)

The system should load the previously created layout. An error message such as File not found! is issued if the requested DDB file is not available. An error message such as Element not found! is issued if the requested element is not available in the selected DDB file.

When entering the Layout Editor, the system knows the name of the file previously processed in any other BAE module. On subsequent file name queries, this global project name can alternatively be specified by selecting the Project button of the file name popup menu or by entering an empty string (i.e., by pressing the return key Return/Enter Key (CR)) to the file name prompt.

Selecting the Project button of the element name popup menu or entering an empty string (i.e., pressing the return key Return/Enter Key (CR)) to the element name prompt causes the system to use the default layout element name defined with the setup (see also chapter 7.2 for a description of the bsetup utility program and how to use the LAYDEFELEMENT command).

The function for loading a layout does not only load the pertinent data from the lower hierarchy levels (parts, padstacks and pads) but also the corresponding net list. The net list data is correlated with all geometrical data on the layout ("Connectivity Generation"). This indeed presupposes identical names for both the layout and the net list. After successfully generating the connectivity, the system is capable of instantly controlling and/or correlating each layout modification with the net list definitions. This highly sophisticated layout design feature is called "Full Copper Sharing" or "True Connectivity". Full copper sharing enables real-time recognition of missing parts, open connections, short-circuits, etc.

The load layout function issues the

Connected pins missing!

warning message if certain net list parts are not yet placed on the layout.

Use the following commands to set the coordinate display mode to inch (which is preferable for the subsequent operations):

SettingsLeft Mouse Button (LMB)
Coordinate DisplayLeft Mouse Button (LMB)
Display InchLeft Mouse Button (LMB)

From now on, Inch units are used during graphic cursor movement for displaying coordinates in the info field.

Board Outline

The design of a new layout should start with the definition of the board outline. This is a continuous polygon line defining the perimeter of the PCB. Use the following commands to create a board outline as shown in figure 4-2:

AreasLeft Mouse Button (LMB)
Add Board OutlineLeft Mouse Button (LMB)
Move to [0.1",0.3"]Left Mouse Button (LMB)
Move to [0.2",0.3"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
Arc LeftLeft Mouse Button (LMB)
Move to [0.4",0.3"]Left Mouse Button (LMB)
Move to [0.6",0.3"]Left Mouse Button (LMB)
Move to [2.8",0.3"]Left Mouse Button (LMB)
Move to [2.8",2.2"]Left Mouse Button (LMB)
Move to [2.3",2.7"]Left Mouse Button (LMB)
Move to [0.4",2.7"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
Arc LeftLeft Mouse Button (LMB)
Move to [0.4",2.5"]Left Mouse Button (LMB)
Move to [0.2",2.5"]Left Mouse Button (LMB)
Move to [0.1",2.5"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

The board outline must not be confused with the element boundaries. The element boundaries are used to define the size of the layout data element. The board outline is a continuous line defining the perimeter of the PCB thus describing the area where parts and traces can be placed. The board outline is required by the Autorouter, i.e., the Autorouter call will fail if no board outline is defined or if parts and/or pins are placed outside the board outline.

Plot Markers

Use the following commands to define two plot markers as shown in figure 4-2:

AreasLeft Mouse Button (LMB)
Add Document LineLeft Mouse Button (LMB)
Plot MarkersLeft Mouse Button (LMB)
Move to [0.1",0.1"]Left Mouse Button (LMB)
Move to [0.1",0.2"]Left Mouse Button (LMB)
Move to [0.2",0.1"]Left Mouse Button (LMB)
Move to [0.2",0.2"]Left Mouse Button (LMB)
Move to [0.1",0.1"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)
Copy AreaLeft Mouse Button (LMB)
Move to [0.1",0.1"]Left Mouse Button (LMB)
Move to [2.7",2.6"]Left Mouse Button (LMB)

Plot markers (or film registration marks) are plot control symbols which are intended for adjusting the plots and/or films later. The plot markers documentary layer can be defined with the bsetup utility program, thus providing a useful feature of including design information on all plot layers with only one definition (see chapter 7.2 for more details).

Figure 4-2: Layout with Board Outline and Plot Markers

Figure 4-2: Layout with Board Outline and Plot Markers

Top Layer

The Set Top Layer function from the Settings menu is used to set the Top Layer (the component side signal layer) of the layout. This layer assignment is most useful when defining (SMT) library symbols for multilayer layouts where the number of layers is not yet determined. The Set Top Layer function can be used to assign a Top Layer for the currently loaded layout:

SettingsLeft Mouse Button (LMB)
Set Top LayerLeft Mouse Button (LMB)
Layer 1
Layer 2
Layer 3
Layer 4
Select Layer
Abort

The default Top Layer setting for new layouts is signal layer 2. The Top Layer will also be the mirror position for mirroring parts, i.e., objects placed beyond the Top Layer will not be affected by mirror functions. The default routing layer count for the Autorouter is automatically set to the Top Layer (but can afterwards be modified in the Autorouter).

The Bartels AutoEngineer layout system supports two methods for setting the layout Top Layer. The first is to assign the desired Top Layer to each layout. This method requires all Top Layer library elements such as SMD pads to be assigned to the component side layer and all signal inside layer assignments to be correct. The All Layers and Middle Layers signal layers are provided to simplify such library definitions. The second method of defining the Top Layer is to use the default signal layer 2 setting for each layout and to interpret the layers beyond layer 2 as signal inside layers. This might slightly reduce the expense for creating layout elements, but the user must then explicitly set the Autorouter routing layer count when routing layouts with more than two signal layers.

Clearance Check Parameters

The Distance functions from the Settings menu are used to set the clearance check parameters for the currently loaded layout. Different Distance functions can be activated from the Settings menu:

SettingsLeft Mouse Button (LMB)
Distance TR/TR
Distance TR/CO
Distance CO/CO

The Distance TR/TR function is used to set the minimum trace-to-trace distance, Distance TR/CO is used to set the minimum trace-to-copper distance and Distance CO/CO is used to set the minimum copper-to-copper distance checking parameter. When creating new layouts, the default spacing value is set to 0.3mm for each clearance check parameter. The distance check parameters are applied by the Design Rule Check and should be set according to manufacturing requirements before starting with the layout design. Note that too tolerant spacing parameters will produce wasted PCBs, thus involving expensive redesign and re-manufacturing requirements.

Non-default net-specific minimum distance settings introduced with the MINDIST net attribute are also considered by the Design Rule Check when performing clearance checks on traces and/or active copper areas.

 

4.3.2 Parts, Placement

On layout hierarchy level, the Parts menu provides functions for placing, moving and deleting parts, for changing part names and for manually performing pin/gate swaps.

Input Grid

BAE supports arbitrary grids and grid-free input. Nevertheless, it is recommended to use a reasonable grid for part placement, thus avoiding off-grid pin placement and enabling pin channel routing to make the routing job easier and to yield higher routing density. Use the following commands to set a 1/10 inch input grid with grid lock:

ViewLeft Mouse Button (LMB)
Grids/RotationLeft Mouse Button (LMB)
Set Input GridLeft Mouse Button (LMB)
1/10 InchLeft Mouse Button (LMB)
Grid+Rotation OnLeft Mouse Button (LMB)

Library Access

The Select Library function from the Settings menu is used for selecting the layout library from which the part symbols should be loaded. Use the following commands to check the current library path selection:

SettingsLeft Mouse Button (LMB)
Select LibraryLeft Mouse Button (LMB)
Library Name ('c:/baelib/laylib.ddb') ? Return/Enter Key (CR)

The name of the currently selected library is displayed with the library file name prompt. When calling the Layout Editor, a default library path is automatically set according to the system setup (see also chapter 7.2 of this manual for a description of the bsetup utility program).

An empty string input to the library name query does not change the current library path setting. A dash string input (-) resets the library path setting (no library selected). ! and/or . input restores the default library path defined with the setup. Under Windows, the library file name is specified through file dialog box. Use the following commands to check the library path settings:

SettingsLeft Mouse Button (LMB)
Select LibraryLeft Mouse Button (LMB)
Library Name ('c:/baelib/laylib.ddb') ?- Return/Enter Key (CR)
Select LibraryLeft Mouse Button (LMB)
Library Name ('') ?! Return/Enter Key (CR)

The Bartels AutoEngineer supports a highly flexible hierarchical database concept. This allows for any DDB file to be used as symbol library. When loading a part symbol, the system first checks the job-specific library (i.e., the currently edited DDB file) for the requested library element. If the requested element is not available in the the project file, then the search is expanded to the currently selected library. The Layout Editor automatically creates a complete copy of the requested library symbol in the current project file when loading a part symbol from an external library. Subsequent requests for the same symbol will then refer to the job-specific library. Figure 4-3 illustrates the Layout Editor library access concept.

Figure 4-3: Layout Library Access

Figure 4-3: Layout Library Access

Changing the library path setting is meaningful only if a series of different part symbols are to be loaded from a library file which is not accessible through the predefined library path. Use the following commands to set the library path to the demolib.ddb DDB file of the current directory:

SettingsLeft Mouse Button (LMB)
Select LibraryLeft Mouse Button (LMB)
Library Name ('c:/baelib/stdsym.ddb') ?demolib Return/Enter Key (CR)

With the commands above, the library path is set to the demolib.ddb DDB file of the working directory, i.e., requested part symbols on subsequent load operations will be copied from demolib.ddb.

Placing Parts

The Add Part, Place Next Part and Place Parts functions from the Parts menu are used for placing parts. These functions work on the selected part set. Initially after loading a layout, all parts are selected, i.e., the system behaves as usual. The functions from the Part Set submenu can be used to restrict and/or redefine the set of parts selected for placement. The Place Next Part function issues a All parts have been placed already! message if all parts are already placed or a All selected parts have been placed! message if all selected parts are already placed, but there are still unselected parts which have not yet been placed. The part set selection popup window displays placed selected parts as [ name ], placed unselected parts as ( name ), unplaced selected parts as : name and unplaced unselected parts as < name >. See chapter 4.4.1 for more information on part set definitions.

The Add Part function is used to load and place parts on the current layout. On layout hierarchy level, the Add Part function activates a net list part name popup menu with the part name prompt. This popup menu displays placed net list parts in brackets ([, ]). Unplaced net list parts are preceded by a colon (:). When selecting or specifying an unplaced net list part name, this part is loaded for placement. Selecting an already placed net list part prompts for confirmation to replace the placed part. Entering an empty string to the part name prompt or selecting the Unplc. button loads the next unplaced net list part. This feature is also provided with the Place Next Part function and works until all net list parts (from the part set) are placed. The system prompts for the library element name when specifying a part name which is not defined in the net list (e.g., when placing a constructive part). Popup menus are provided with the library element name query for selecting the library file and the library element name. The library file name list is derived from the layout library path defined with the BAE setup, i.e., all DDB files available in the directory of the layout library path are listed. The Lib. button or > input to the library file name prompt selects the standard layout library defined through the Select Library function from the Settings menu. The Project button in the library file name popup selects the current project file. A library element name query is activated after selecting the library file. Library elements can optionally be selected by typing both the library file name (i.e., one of the names displayed with the library file name popup), a slash (/), and the library element name to the library element name prompt (typing ? for the element name activates a popup menu providing the list of library elements from the specified library file). An empty string input to the library element name query causes the system to use the library element previously selected with the Add Part function (if there was already one specified).

The net list part name selection popups are also provided with the Change Part Name and Netlist Part Name functions from the Parts menu. The library element name selection of the Add Part function is also implemented for placing pins (i.e., selecting padstacks) on layout part symbol level and for loading pads onto layout padstack level.

Use the following commands to load the part named IC10 and place it at coordinate [1.2",1.8"]:

PartsLeft Mouse Button (LMB)
Add PartLeft Mouse Button (LMB)
Part Name ?ic10 Return/Enter Key (CR)
Move to [1.2",1.8"]Left Mouse Button (LMB)

The Add Part function checks whether a part with the specified name exists in the net list. If the part is defined in the net list, then the system knows the package to be used for this part and automatically loads the corresponding part symbol (i.e., dil14 in the example above). The system issues an error message such as

Element not found!

if the requested part symbol is not available in the current job file or in the selected library. In this case you should use the Select Library function from the Settings menu in to check whether the correct library is accessed.

Use the following commands to load and place two parts named hole1 and hole2 using the hole3mm package type which was created in chapter 4.2.3 in DDB file demo.ddb:

PartsLeft Mouse Button (LMB)
Add PartLeft Mouse Button (LMB)
Part Name ?hole1 Return/Enter Key (CR)
Library Element Name ?hole3mm Return/Enter Key (CR)
Move to [0.4",0.3"]Left Mouse Button (LMB)
Add PartLeft Mouse Button (LMB)
Part Name ?hole2 Return/Enter Key (CR)
Library Element Name ? Return/Enter Key (CR)
Move to [0.4",2.5"]Left Mouse Button (LMB)

The (constructive) parts hole1 and hole2 are not defined in the net list, i.e., the system does not know the corresponding package types. The Add Part function activates a library element name query with a popup menu providing access to all library files available through the predefined default library path. The Project button of this menu can be used for accessing the job-specific library of the currently processed DDB file. After selecting the library file, another popup menu with a list of all symbols available in the selected library file is activated. An empty string input (i.e., just pressing the return key Return/Enter Key (CR)) to the library element name query causes the system to use the part symbol loaded with the preceding Add Part call.

Use the following commands to load and place the plug named x1000:

PartsLeft Mouse Button (LMB)
Add PartLeft Mouse Button (LMB)
Part Name ?x1000 Return/Enter Key (CR)
Right Mouse Button (RMB)
Rotate LeftLeft Mouse Button (LMB)
Move to [2.4",1.0"]Left Mouse Button (LMB)

Pressing the right mouse button during part placement activates a submenu which provides functions for specifying absolute placement coordinates, part rotation (even at arbitrary rotation angles) and part mirroring (for placing SMDs on solder side).

Use the following commands to place the next part:

PartsLeft Mouse Button (LMB)
Add PartLeft Mouse Button (LMB)
Part Name ? Return/Enter Key (CR)
Right Mouse Button (RMB)
Mirror OnLeft Mouse Button (LMB)
Move to [1.8",1.4"]Left Mouse Button (LMB)

An empty string input (i.e., just pressing the return key Return/Enter Key (CR)) to the part name query causes the Add Part function to load the next unplaced net list part. In the example above, the system automatically loads the SMD capacitor named c100, which then is placed on solder side.

The facility for loading the next net list part (without knowing the corresponding part name) can also be activated with the Place Next Part function. Use this command to place the part named c101 as in

PartsLeft Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Right Mouse Button (RMB)
Mirror OnLeft Mouse Button (LMB)
Move to [1.4",1.4"]Left Mouse Button (LMB)

Use the following commands to place the relay part named k1, the resistor parts named r100, r101, r102, r103, r104, r105 and the switch named s1000:

PartsLeft Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.8",0.8"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [1.0",2.4"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [1.6",2.4"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Right Mouse Button (RMB)
Rotate LeftLeft Mouse Button (LMB)
Move to [1.6",1.2"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Right Mouse Button (RMB)
Rotate LeftLeft Mouse Button (LMB)
Move to [1.4",1.2"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [2.1",2.1"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [2.1",1.8"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Right Mouse Button (RMB)
Rotate RightLeft Mouse Button (LMB)
Move to [0.2",2.3"]Left Mouse Button (LMB)

The Set Default Angle function can be utilized for subsequently placing a series of parts at certain rotation angles and/or mirror modes (e.g., SMD parts). Use the following commands to set the standard placement rotation angle to 270 degrees and place the switches named s1001 through s1009:

PartsLeft Mouse Button (LMB)
Set Default AngleLeft Mouse Button (LMB)
270 Degrees LeftLeft Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",2.1"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",1.9"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",1.7"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",1.5"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",1.3"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",1.1"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",0.9"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",0.7"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Move to [0.2",0.5"]Left Mouse Button (LMB)

Use the following commands to complete the placement, i.e., place part v1 (with absolute placement coordinates and 45 degree rotation angle) and part v1000:

PartsLeft Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)
Right Mouse Button (RMB)
Set AngleLeft Mouse Button (LMB)
Angle (Deg./(R)ad) ?-45 Return/Enter Key (CR)
Right Mouse Button (RMB)
Jump AbsoluteLeft Mouse Button (LMB)
Absolute X Coordinate (mm/") ?0.825" Return/Enter Key (CR)
Absolute Y Coordinate (mm/") ?1.225" Return/Enter Key (CR)
Place Next PartLeft Mouse Button (LMB)
Move to [1.2",1.6"]Left Mouse Button (LMB)
Place Next PartLeft Mouse Button (LMB)

The Place Next Part function issues the

All parts have been placed already!

message once all net list parts are placed. I.e., the Place Next Part function can also be used to check on placement completion.

After correctly executing all work steps of this chapter, the PCB layout example should look like the one shown in figure 4-4.

Figure 4-4: Layout with Part Placement

Figure 4-4: Layout with Part Placement

Moving and Deleting Parts

The Move Part function is used to move parts which are already placed on the layout. Pressing the right mouse button during part movement activates a submenu with special options for rotating and mirroring, absolute or relative placement coordinates input, etc. The Delete Part function is used to delete placed parts from the layout. You should test these functions on the currently loaded layout and use the Undo and Redo functions for estimating design modifications and returning to the original design stage as shown in figure 4-4.

Alternate Part Package Type Assignment

The Alternate Part option is provided with the Layout Editor submenus which can be called by pressing the right mouse button during interactive part placement. This option can be used to change the part package type of the currently placed part. The alternate package type can be selected from a list of layout part macros. The alternate part list is either pre-defined in the logical library using the loglib utility program (see chapter 7.11) or can be defined through an SCM symbol $plname attribute value assignment such as [package1,package2,...]. An error message such as No alternate part macros defined! is issued if no alternate package types are defined for the currently processed part. An error message such as Connected pins missing! is issued if the pin definitions on the selected alternate package type do not match the net list, i.e., if net list pins are missing on the selected macro. Alternate part package type assignments create a backannotation request which triggers automatic Backannotation when loading SCM plans to the Schematic Editor (see chapter 2.7). Backannotation requests also prevent the Packager from forward annotation without confirmation (see chapter 3.2.3).

Mincon Function, Airlines Display

Unrouted net list connections are displayed as airlines. During part placement, the Mincon function performs dynamic (real-time) recalculation of these airlines to display minimum length airline sets. I.e., the Mincon function is a most useful utility for achieving an optimum manual placement. Use the following commands to test different airline calculation methods supported through the Mincon function and note how the Mincon function type affects the way airlines are displayed:

SettingsLeft Mouse Button (LMB)
Mincon FunctionLeft Mouse Button (LMB)
Corners HorizontalLeft Mouse Button (LMB)
Mincon FunctionLeft Mouse Button (LMB)
Pins VerticalLeft Mouse Button (LMB)
Mincon FunctionLeft Mouse Button (LMB)
Mincon OffLeft Mouse Button (LMB)
Mincon FunctionLeft Mouse Button (LMB)
Corners H+V SumLeft Mouse Button (LMB)

The Airlines Display function from the Parts menu is used to set the airline display mode to be applied during part movement. No Airlines switches off the airlines display during part movement. Static Airlines does not recalculate the nearest connection points during part movement. Dynamic Airlines dynamically recalculates the closest connection points (note how the airlines jump to the nearest pins or copper corners during part movement). Dynamic Airlines is the default Airlines Display option.

The Net Visible and Net Invisible Mincon options allow for a net-specific airline display, i.e., it is possible to fade-out (Net Invisible) and/or fade-in (Net Visible) net-specific airlines by selecting the desired net(s) from a net name popup menu which optionally allows for multiple net selections through net name pattern specifications.

The All Nets Visible Mincon option forces the graphical display of all airlines, whilst All Nets Invisible fades out all airlines.

The context menu which is available through the right mouse button during part placement provides the All Nets and Part Nets options for selecting either part-specific or global airline display.

 

4.3.3 Text and Graphic

On layout hierarchy level, text (on documentary layers or on signal layers) and graphic (i.e., polygons such as documentary lines, documentary areas, passive copper areas, active copper areas, keepout areas, copper fill workareas) can be defined. For the following operations it is recommended to set the input grid to 1/20 inch (use the Grids/Rotation and Set Input Grid functions from the View menu) and to set the coordinate display mode to inch (use function Coordinate Display from the Settings menu).

Placing Text

Use the following commands to place the DEMO text string adjacent to the right top of the board outline with a text size of 4mm on the Insertion Plan (Side 2) documentary layer:

Text, DrillLeft Mouse Button (LMB)
Add TextLeft Mouse Button (LMB)
Document LayerLeft Mouse Button (LMB)
Insertion PlanLeft Mouse Button (LMB)
Text ?DEMO Return/Enter Key (CR)
Right Mouse Button (RMB)
Set AngleLeft Mouse Button (LMB)
Angle (Deg./(R)ad.) ?-45 Return/Enter Key (CR)
Right Mouse Button (RMB)
Text SizeLeft Mouse Button (LMB)
Text Size ( 2.54mm) ?4 Return/Enter Key (CR)
Move to [2.4",2.6"]Left Mouse Button (LMB)

Use the following commands to place the Component Side text string with text size 2.54mm on the PCB component side signal layer (Top Layer, Layer n (Parts.)):

Text, DrillLeft Mouse Button (LMB)
Add TextLeft Mouse Button (LMB)
Layer n (Parts.)Left Mouse Button (LMB)
Text ?Component Side Return/Enter Key (CR)
Right Mouse Button (RMB)
Text SizeLeft Mouse Button (LMB)
Text Size ( 4.00mm) ?2.54 Return/Enter Key (CR)
Move to [1.00",2.55"]Left Mouse Button (LMB)

The Text Size function which can be activated whilst placing texts sets the default text size for subsequent calls to the Add Text function. Use the following commands to place a rotated and mirrored text with string Solder Side on the PCB solder side (signal layer 1):

Text, DrillLeft Mouse Button (LMB)
Add TextLeft Mouse Button (LMB)
Layer 1Left Mouse Button (LMB)
Text ?Solder Side Return/Enter Key (CR)
Right Mouse Button (RMB)
Set AngleLeft Mouse Button (LMB)
Angle (Deg./(R)ad.) ?180 Return/Enter Key (CR)
Right Mouse Button (RMB)
Mirror OnLeft Mouse Button (LMB)
Move to [1.80",2.55"]Left Mouse Button (LMB)

Texts placed on signal layers are subject to the design rule check. I.e., the DRC will issue distance errors for intersections between signal layer texts and other objects (pads, traces, copper areas, texts, etc.) placed on the same signal layer.

Moving Part Names and Part Attribute Texts

The Move Name function from the Text and/or Parts menu is used to move part names. Use the following commands to move the names of the SMD resistors named r104 and r105 on top of the parts:

Text, DrillLeft Mouse Button (LMB)
Move NameLeft Mouse Button (LMB)
Move to "r104",[2.1",2.1"]Left Mouse Button (LMB)
Move to [2.1",2.15"]Left Mouse Button (LMB)
Move NameLeft Mouse Button (LMB)
Move to "r105",[2.1",1.8"]Left Mouse Button (LMB)
Move to [2.1",1.85"]Left Mouse Button (LMB)

The Move Attribute function from the Parts and/or Text menu can be used for moving and/or placing selectable part attributes. Attribute text offsets defined through Move Attribute override the global text offset set with Move Name. The attribute to be moved is selected through a mouse-click on the attribute text. Since part names are internally stored as $ attributes, the Move Attribute function can also be used to move part names without changing the placement of other part attributes.

Part names and part attribute texts of group-selected parts can be reset to their library-defined default positions using the Part Texts Reset function implemented with the gedgroup User Language program.

Measuring

The Layout Editor automatically activates a measuring function when placing new text with string #. This function determines the distance between the two input coordinates subsequently to be specified. The resulting text string emerges from the corresponding distance value; the length units (inch or mm) result from the current coordinate display mode selected with the Coordinate Display Settings menu function. Use the following commands to apply measuring on the bottom right board outline edge and place the resulting distance value (2.2") on the Insertion Plan (Side 2) documentary layer:

Text, DrillLeft Mouse Button (LMB)
Add TextLeft Mouse Button (LMB)
Document LayerLeft Mouse Button (LMB)
Insertion PlanLeft Mouse Button (LMB)
Text ?# Return/Enter Key (CR)
Move to Left Coordinate,[0.6",0.3"]Left Mouse Button (LMB)
Move to Right Coordinate,[2.8",0.3"]Left Mouse Button (LMB)
Move to [1.50",0.15"]Left Mouse Button (LMB)

Documentary Lines, Documentary Areas

Use the following commands to create a documentary line and two arrow-shaped documentary areas on the Insertion Plan (Side 2) documentary layer to indicate the previously defined measuring:

AreasLeft Mouse Button (LMB)
Add Document LineLeft Mouse Button (LMB)
Insertion PlanLeft Mouse Button (LMB)
Move to [0.6",0.15"]Left Mouse Button (LMB)
Move to [0.8",0.15"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)
Add Document AreaLeft Mouse Button (LMB)
Insertion PlanLeft Mouse Button (LMB)
Move to [0.6",0.15"]Left Mouse Button (LMB)
Move to [0.65",0.2"]Left Mouse Button (LMB)
Move to [0.65",0.1"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)
Add Document AreaLeft Mouse Button (LMB)
Insertion PlanLeft Mouse Button (LMB)
Move to [2.8",0.15"]Left Mouse Button (LMB)
Move to [2.75",0.2"]Left Mouse Button (LMB)
Move to [2.75",0.1"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

Passive Copper Areas

Use the following commands to create a circle-shaped passive copper area on signal layer 2:

AreasLeft Mouse Button (LMB)
Add Passive CopperLeft Mouse Button (LMB)
Layer 2Left Mouse Button (LMB)
Move to [0.95",1.6"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
Arc LeftLeft Mouse Button (LMB)
Move to [0.8",1.6"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

Active Copper Areas

Use the following commands to create an active copper area on signal layer 1 and assign this copper area to net Vdd:

AreasLeft Mouse Button (LMB)
Add Active CopperLeft Mouse Button (LMB)
Net Name ?vdd Return/Enter Key (CR)
Layer 1Left Mouse Button (LMB)
Move to [2.4",1.7"]Left Mouse Button (LMB)
Move to [2.7",1.7"]Left Mouse Button (LMB)
Move to [2.7",2.2"]Left Mouse Button (LMB)
Move to [2.6",2.3"]Left Mouse Button (LMB)
Move to [2.4",2.3"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

Keepout Areas

Use the following commands to define a keepout area on signal layer 1 and a keepout area on signal layer All Layers (keepout areas define layer-specific regions on the PCB where no traces, no copper areas, no texts, etc. are allowed to be placed):

AreasLeft Mouse Button (LMB)
Add Keep Out AreaLeft Mouse Button (LMB)
Layer 1Left Mouse Button (LMB)
Move to [1.8",1.2"]Left Mouse Button (LMB)
Move to [2.2",1.2"]Left Mouse Button (LMB)
Move to [2.2",0.9"]Left Mouse Button (LMB)
Move to [1.7",0.9"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)
Add Keep Out AreaLeft Mouse Button (LMB)
All LayersLeft Mouse Button (LMB)
Move to [0.6",2.6"]Left Mouse Button (LMB)
Move to [0.6",2.1"]Left Mouse Button (LMB)
Move to [0.9",2.1"]Left Mouse Button (LMB)
Move to [0.9",2.6"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)
 

4.3.4 Traces, Routing

The Traces menu provides functions for interactive routing on layout and/or part hierarchy level, i.e., for manually creating new traces and for modifying or deleting existing traces and/or trace segments. Arbitrary track widths can be defined for individual trace segments or complete routing paths. Special or critical nets such as the power supply can be pre-routed and then fixed to prevent the Autorouter from rerouting such nets.

Graphic Control Functions, Input Grid, Display

During manual routing, the system provides a highlight on all objects of the currently routed signal. After completing the routing of a certain connection, the corresponding airline is removed from the display. Short-circuits and distance violations introduced by manual routing are immediately indicated by the Online DRC using highlight and/or distance error boxes.

If you fail to connect certain (off-grid) pins with the current input grid settings, then you should use the View functions for selecting a smaller input grid (or even release the grid lock).

The middle mouse button can be used to activate the View menu at any time during manual routing. I.e., important display options such as zoom scale, grids, colors, etc. can be changed without cancelling the currently active trace edit function.

The View menu also provides the Set Edit Layer function for selecting the pick preference layer. The pick preference layer is used to resolve ambiguities at the selection of trace elements placed at the same position but on different layers. The pick preference layer is also the default routing layer when starting to route from a drilled ("All Layer") pad or from a copper-free position. On default, the pick preference layer is set to signal layer 1 (solder side).

The algorithm for picking trace corners and trace segments picks the trace element with minimum distance from the pick point if more than one possible pick element is within snapping distance. This allows for reliable selection of trace elements even when working in (small) zoom overview display modes. The trace pick snapping distance is automatically adjusted to the trace width. I.e., trace elements (of wide traces or in high zoom display modes) can easily be picked without having to hit the trace center line.

Highlight Net

The Highlight Net function from the Layout Editor Traces menu is used to mark all connections of the selected net with a special ("Highlight") color. Any power layer heat-trap circles and isolations of the selected net is included with the highlight display, and isolated pins and active copper areas can also be selected for highlight. Starting a new trace on a passive copper area triggers a highlight for the nets connected to that copper area. The Highlight Net function works as a toggle. To reset the highlight of a certain net, pin or active copper area, simply re-select that object with the Highlight Net function. Advanced color support and highlight reset facilities are provided through the Highlight Net (default mode), Color Nets (with highlight color selection) and Reset All (for clearing all nethighlight) options of the Highlight Net function.

In BAE HighEnd, the Highlight Net function causes a highlight and/or de-highlight of the selected nets in all currently loaded plans of the current project file on layout board and schematic sheet level (global net highlight, cross-probing).

Selecting the Via

The Bartels AutoEngineer layout system utilizes special padstack symbols (vias) for connecting different layers of the PCB. At least one via assignment is required before any routing function (i.e. either a trace function or the Autorouter) can be activated. Use the following commands to insert the estk padstack symbol to the currently active via list:

PartsLeft Mouse Button (LMB)
Select ViaLeft Mouse Button (LMB)
New/Delete: Via Name ?estk Return/Enter Key (CR)
New/Delete: Via Name ? Return/Enter Key (CR)

The estk padstack symbol is used as pin symbol on the already placed part v1000 (package type d04a25). I.e., estk is available in the current job file. A series of via padstack definitions are provided with the layout libraries shipped with the BAE software. Usually the padstack symbol named via can be used as standard via. The via assignments introduced with Select Via are stored with the layout element. The Add Trace function issues the following error message if no via is selected:

Default via not defined!

The system is capable of processing several different via definitions at a time in order to support blind and buried vias. The via assignment list can be changed at any time. Previously placed vias will not be affected by via list modifications, i.e., the currently defined via list will apply for the interactive routing of new traces. When changing layers during manual routing the Layout Editor will automatically place vias with the least possible layer usage (if padstacks are defined and selected to the via list accordingly). The current via assignment list will also be used by the Autorouter, and, with the use of blind and buried vias, the Autorouter will minimize layer occupancy as well (this is true for all traces except for fixed traces which will not be processed by the Autorouter).

Standard Trace Widths

The trace function submenus provide options for toggling between thin and wide default track widths during manual routing (necking). The standard values for these default track widths can be changed with the Set Trace Width function from the Settings menu, where the options Set Thin Default (default value 0.3mm) and Set Wide Default (default value 1.0mm) are provided. The routing of a new trace always starts with the thin default track width.

Manual Routing

Use the following commands to route from pin A1 of part K1 to pin C1 of the same part (both pins are connected to net Vdd):

TracesLeft Mouse Button (LMB)
Add TraceLeft Mouse Button (LMB)
Move to "K1.A1",[0.8",0.8"]Left Mouse Button (LMB)
Move to Corner Point,[0.8",0.95"]Left Mouse Button (LMB)
Move to Corner Point,[1.6",0.95"]Left Mouse Button (LMB)
Move to "K1.C1",[1.6",0.8"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

Each trace corner point is set by pressing the left mouse button. The routing of a trace path is completed with the Done option from the submenu available with the right mouse button. This submenu is also available during trace editing with functions such as Insert Corner or Move Segment where the routing layer or the track width can be changed, arc-shaped trace segments can be created, relative and absolute coordinate input can be specified, etc.

Use the following commands to connect the pins C2 and C1 of part K1 with a trace segment on signal layer 2:

TracesLeft Mouse Button (LMB)
Add TraceLeft Mouse Button (LMB)
Move to "K1.C2",[1.6",0.5"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
Layer 2Left Mouse Button (LMB)
Move to "K1.C1",[1.6",0.8"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

Use the following commands to create a trace segment on signal layer 1 starting at pin 9 of the plug named X1000 and ending with a via to connect to the previously generated trace:

TracesLeft Mouse Button (LMB)
Add TraceLeft Mouse Button (LMB)
Move to "X1000.9",[2.45",0.85"]Left Mouse Button (LMB)
Move to Corner Point,[2.45",0.65"]Left Mouse Button (LMB)
Move to Vertical Trace Segment,[1.6",0.65"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
Layer 2Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

Use the following commands to deselect estk from the via list, select the padstack symbol via (which has been created in chapter 4.2.2 in the demo.ddb DDB file) to the via list, and then route a trace on signal layer 2 starting at pin K of the diode named V1000 and ending with a via connecting to the horizontal trace between the pins A1 and C1 of part K1:

PartsLeft Mouse Button (LMB)
Select ViaLeft Mouse Button (LMB)
New/Delete: Via Name ?estk Return/Enter Key (CR)
Please confirm (Y/N) ?y Return/Enter Key (CR)
New/Delete: Via Name ?via Return/Enter Key (CR)
New/Delete: Via Name ? Return/Enter Key (CR)
Middle Mouse Button (MMB)
Set Edit LayerLeft Mouse Button (LMB)
Layer 2Left Mouse Button (LMB)
TracesLeft Mouse Button (LMB)
Add TraceLeft Mouse Button (LMB)
Move to "V1000.K",[1.2",1.6"]Left Mouse Button (LMB)
Move to Corner Point,[1.1",1.6"]Left Mouse Button (LMB)
Move to Horizontal Trace Segment,[1.1",0.95"]Left Mouse Button (LMB)
Right Mouse Button (RMB)
Layer 1Left Mouse Button (LMB)
Right Mouse Button (RMB)
DoneLeft Mouse Button (LMB)

You should now gain more practice by using the trace functions on the currently loaded layout in order to create and/or modify more traces (move, cut and delete trace segments; insert, move and delete trace corner points; change track widths, create arc-shaped traces, etc.). Note the Move without Neighbour, Move with Neighbour and Adjust neighbours options provided with the submenu of the Move Segment function. The Move without Neighbour default mode just moves the corner points of the processed trace segment, whilst the Move with Neighbour mode also rearranges adjacent trace segments in order to keep the angles between the processed trace and the adjacent segments constant. Adjust neighbours considers intersection points between new and neighbouring segments and rearranges neighbouring segments accordingly. This feature is especially useful for moving diagonal segments at trace corners. The Move w.out neighb. option is applied if neighbouring segments cannot be rearranged. Use the Undo and Redo functions to estimate design modifications and return to the original design stage.

Fixing Traces

It is recommended to fix pre-routed traces which must not be modified and/or rerouted by the Autorouter. Use the following commands to fix all prerouted traces of net Vdd:

TracesLeft Mouse Button (LMB)
Fix Trace/NetLeft Mouse Button (LMB)
NetLeft Mouse Button (LMB)
Move to Signal/Net "Vdd",e.g.[2.0",0.65"]Left Mouse Button (LMB)
Right Mouse Button (RMB)

The Unfix Trace/Net function is used to release fixed traces or nets. During fix and release operations the Layout Editor provides a specific highlight for indicating currently fixed elements.

The Layout Editor trace functions for interactive routing keeps traces and vias fixed when processing pre-routed fixed traces. I.e., when manipulating pre-routed fixed traces, there is no need of re-fixing such traces to prevent the Autorouter from re-routing and/or rejecting pre-routed traces.

Bartels :: Bartels AutoEngineer :: BAE Documentation :: BAE User Manual :: PCB Design :: Designing PCB Layouts

Designing PCB Layouts
© 1985-2017 Oliver Bartels F+E • Updated: 11 October 2010, 10:30 [UTC]

© 1985-2017 Oliver Bartels F+E Bartels Homepage Contact and Corporate Info

Web Development by Baumeister Mediasoft Engineering

Layouterstellung - Deutsche Version Designing PCB Layouts - English Version