The Batch DRC function from the Layout Editor Utilities menu is used to run a complete design rule check on the currently loaded layout. It is strongly recommended to use Batch DRC before generating CAM data and/or passing CAM data to the PCB manufacturer to avoid design rule violations such as short-circuits, unrouted nets or clearance violations. Use the following commands to perform a batch design rule check on the currently loaded layout board of the demo.ddb DDB file:

Utilities

Batch DRC

Please confirm (Y/N) ?

After performing the design rule check, the Batch DRC function implicitly activates the Report function from the Utilities menu to display the checking results and the design state. The Report function can also be called explicitly using the following commands:

Utilities

Report

The following listing is displayed by the Report function or after Batch DRC (zero error lines might be omitted):

File : demo.ddb
Type : Layout / Element : board


Number of Nets .................: 22
Number of Open Connections .....: 0
Number of Short Circuits .......: 0
Copper Distance Violations .....: 0
Documentary Distance Violations : 0
Number of Power Layer Errors ...: 0
Number of Missing Parts ........: 0
Number of Wrong Type Parts .....: 0
Number of Missing Netlist Pins .: 0
Height Distance Violations .....: 0
Power Layers in Use.............: -
Signal Layers in Use............: 1-2

The Number of Nets report entry displays number of nets defined in the net list of the currently loaded layout. The Number of Open Connections entry denotes the number of not yet routed (two-point) connections on the currently loaded layout. The Number of Short Circuits entry denotes the number of short-circuits encountered by the Design Rule Check. The Copper Distance Violations entry denotes the number of copper layer clearance distance violations online-encountered by the Design Rule Check on the currently loaded element. The Documentary Distance Violations entry denotes the number of clearance distance violations on documentary layers. The Number of Power Layer Errors entry denotes number of copper area cross-intersections on split power planes. The Number of Missing Parts report entry denotes the number of net list parts not yet placed on the currently loaded layout. The Number of Wrong Type Parts report entry denotes the number of net list parts placed with a wrong part package type (macro) on the currently loaded layout. The Number of Missing Netlist Pins entry denotes the number of unplaced and/or missing net list pins. Missing net list pins can cause an erroneous open connections count. An indicator is added to the open connections count if net list pins are missing. The checklnl User Language program can be used to track missing net list pins. The Height Distance Violations entry denotes the number of (part) height design rule violations. The Power Layers in Use and Signal Layers in Use report entries display the used power and signal layers. Signal layer 1 to top layer are always assumed to be in use. These entries help to identify power layers without global net assignment, hence with split power planes to be considered by connectivity.

DRC Error Display

The Settings dialog from the Layout Editor View menu provides the DRC Error Display parameter for selecting DRC distance and height rule violation error display modes and/or colors. The Error Color option displays error boxes using the error color selected with the Change Colors function, the default of which is white. The Highlight Layer setting displays error rectangles using the color selected for the layer on which the erroneous element is placed. Errors on layers which are faded-out through Change Colors are not displayed.

The Layout Editor Utilities menu provides the DRC Error List function for displaying the DRC distance and height rule violation error lists. The DRC errors are listed in a popup menu, indicating error type, error layer and error coordinates for each error. A Zoom Window to the error position ist triggered when selecting an error from the list using the left mouse button. The + and - keys can be used to move the zoom window through the error position list in either direction.

Note that the modified BAE HighEnd data structure for storing the layout connectivity data allows for a selective shortcut display, i.e., shortcuts between two nets are displayed by highlighting only those elements causing the shortcut, whilst BAE Professional highlights the whole connection tree affected by the short-circuit.

Hit the spacebar to return to the Layout Editor menu.

^Contents <>

4.6.2 Color Setup, Color Tables, Pick Preference Layer

The Change Colors function from the View menu activates a popup menu for modifying the current color settings. This color setup menu simultaneously can be utilized for displaying the current color assignments. Changing some item-specific color is accomplished by selecting the desired display item using the left mouse button and then selecting the desired color button from the Change Colors function. In the layout system, Change Colors provides a feature for fast display item fade-out/fade-in. Activating and/or deactivating some item-specific display is accomplished by selecting the desired display item entry with the right mouse button which works as a toggle between fade-out and fade-in. The system won't loose information on currently defined colors of faded-out display items; strike-through color buttons are used for notifying currently faded-out display items.

At overlaps of different elements the resulting mixed color is displayed. The highlight color is also mixed with the color of the element to be marked, thus resulting in a brighter display of that element.

The Save Colors function from the View menu is used to save the current color settings with a user-specified name to the ged.dat system file in the BAE programs directory. When starting the Layout Editor (or any other layout program module), the color table named standard is automatically loaded. Any other color table available in ged.dat can be loaded using the Load Colors function from the View menu.

It is a good idea to define color tables for certain tasks such as stackdef for padstack editing (i.e., with drill holes and drill plan visible) or unroutes for fast open connections recognition (i.e., with airlines visible only). At the definition of color tables it is to be considered that screen redraw functions will take longer if more objects must be displayed. It is recommended to define task-specific color tables to display only those objects which are important for the corresponding task.

The Set Edit Layer function is usually used to allow selection on a specific layer. It also has the useful hidden function of loading a layer-specific color table. These color tables have specific names, and if they don't exist there will be no change in the color display. See table 4-3 for the color table names assigned to the pick preference layers (<n> is the layer number, respectively). Table 4-3 also lists short layer names which can optionally be used in certain layer menus for selecting layers via keyboard input.

Table 4-3: Pick Preference Layer Color Tables and Short Layer Names

Layer	Pick Preference Layer Color Table Name	Short Layer Name
Signal Layer <n>	layer_<n>	<n>
Signal Layer All Layers	layer_all	a
Signal Layer Middle Layers	layer_def	m
Signal Layer Top Layer	layer_def
Power Layer <n>		p<n>
Documentary Layer <n> Side 1	layer_d<n>_1	d<n>s1
Documentary Layer <n> Side 2	layer_d<n>_2	d<n>s2
Documentary Layer <n> Both Sides	layer_d<n>_a	d<n>sa
Board Outline		b
Airlines		u

When selecting a certain pick preference layer (e.g., signal layer 2) using the Set Edit Layer function, the color table with the corresponding name (e.g., layer_s2) is automatically loaded if available in ged.dat. This feature is most useful for e.g., manual routing.

^Contents <>

4.6.3 Layout Net List Changes

The Layout Editor provides functions for performing pin/gate swaps to simplify the routing problem. Alternate package types can be assigned to layout parts, and net list part names can be changed for better legibility of the insertion plan (for manual insertion). These modifications are net list changes which must be backward annotated to the schematics using the Backannotation function from the Schematic Editor (see also chapter 3.3).

In this section we will apply some pin/gate swaps and change a couple of part names. First of all, use the following commands to set the coordinate display mode to inch and apply group functions to delete all traces from the currently loaded layout:

Settings

Coordinate Display

Display Inch

Groups

Group Polygon

Traces

Select

Move to [0.1",0.1"]

Move to [2.8",0.1"]

Move to [2.8",2.7"]

Move to [0.1",2.7"]

Done

Delete Group

The Pin/Gate Swap function from the Parts menu is used to perform manual pin/gate swaps. Use the following commands to swap the pins 1 and 2 of the switches named s1000, s1001, s1002 and s1003, respectively:

Parts

Pin/Gate Swap

Move to "s1000.1",[0.2",2.3"]

Move to "s1000.2",[0.5",2.3"]

Pin/Gate Swap

Move to "s1001.1",[0.2",2.1"]

Move to "s1001.2",[0.5",2.1"]

Pin/Gate Swap

Move to "s1002.1",[0.2",1.9"]

Move to "s1002.2",[0.5",1.9"]

Pin/Gate Swap

Move to "s1003.1",[0.2",1.7"]

Move to "s1003.2",[0.5",1.7"]

Note how the Pin/Gate Swap function provides graphical pin/gate swap indicators. A circle (0.6mm diameter, Workspace color) is displayed for every pin/gate swap enabled pin when the Pin/Gate Swap function is activated. The indicator for the first selected pin turns into a filled square, leaving only swappable pins marked by circles and character codes for the possible swap operations. The character codes are P for pin swap, G for gate swap and A (Array) for gate group swap. Selecting black for the Workspace color deactivates the pin/gate swap indicator display.

Each pin/gate swap is performed using the corresponding pin/gate swap definition from the Logical Library (see also chapter 7.11 for a description of the loglib utility program and chapter 3.2 for a description of the Packager program module). The following error message is issued if no swap is allowed for the selected pins and/or gates:

Not allowed to swap these pins!

Use the following commands to swap the gates (1,2,3) and (5,6,4) as well as the pins 12 and 13 of the part named IC10:

Parts

Pin/Gate Swap

Move to "ic10.(1,2,3)",[1.4",1.8"]

Move to "ic10.(5,6,4)",[1.5",1.8"]

Pin/Gate Swap

Move to "ic10.12",[1.4",2.1"]

Move to "ic10.13",[1.3",2.1"]

Use the following commands to perform a part swap for the resistor parts named R101 and R103 (this is allowed because the same attribute values are assigned to these parts):

Parts

Pin/Gate Swap

Move to "r101",[1.6",2.4"]

Move to "r103",[1.4",1.2"]

The Netlist Part Name function from the Parts menu is used to change part names in the net list. Use the following commands to change the net list part name of connector X1000 to filenameX1, and also change the net list part name of diode V1000 to V2:

Parts

Netlist Part Name

Move to "x1000",[2.4",1.5"]

Part Name (X1000) ?

Netlist Part Name

Move to "v1000",[1.2",1.2"]

Part Name (V1000) ?

The Netlist Part Name function issues the following error message if you try to assign a part name which is already in use for another part:

Part name already in use!

Use the following commands to apply the Change Part Name function to change the name of part IC10 to IC1:

Parts

Change Part Name

Move to "ic10",[1.2",1.8"]

Part Name (IC10) ?

IC1

The airlines previously connected to IC10 have been disappeared from IC1. I.e., the Change Part Name function not only performs a part name change, but also replaces the selected part. With the commands above the part named IC10 has been replaced with the part IC1 which is not defined in the net list. Use the following commands to reset this part name change and apply the Netlist Part Name function to change the net list part name to IC1 (note how the airlines connected to IC1 will appear again):

Parts

Change Part Name

Move to "ic1",[1.2",1.8"]

Part Name (IC1) ?

ic10

Netlist Part Name

Move to "ic10",[1.2",1.8"]

Part Name (IC10) ?

ic1

It is recommended to use the Change Part Name function with caution. Multiple misuse of the Change Part Name function can cause short circuits on routed layouts, and it might get very laborious to backtrack part name changes for design corrections.

The layout net list changes accomplished with the previous operations must be backannotated to the schematics and the logical net list. Use the following commands to save the currently loaded layout and return to the BAE main menu:

File

Save Element

File

Main Menu

The BAE main menu is activated. Use the following commands to switch to the Schematic Editor and run Backannotation to transfer the physical net list named board in in demo.ddb back to the schematics:

Schematic

Utilities

Backannotation

Design File Name ?

demo

Layout Element Name ?

board

Backannotation displays the following messages:

==============================
BARTELS BACKANNOTATION UTILITY
==============================


Design File Name ........: 'demo'
Layout Element Name .....: 'board'
No error occurred!

The No error occurred! message means that Backannotation has been successfully completed, and the logical net list in project file demo.ddb has been annotated with the physical net list named board. Hit any key to return to the Schematic Editor main menu and use the following commands to load the SCM sheet sheet1 from DDB file demo.ddb:

File

Load

Sheet

File Name ?

demo

Element Name ?

sheet1

You can now examine the currently loaded SCM sheet for modifications introduced by Backannotation. Particularly note the part name changes (IC1 instead of IC10, V2 instead of V1000, etc.) and the pin assignment changes (e.g., at the gates of IC1 or at the switches S1000 through S1003).

^Contents <>

4.6.4 SCM Changes, Redesign

Bartels AutoEngineer provides features for modifying SCM sheets of an already completed design, without the need to prepare a completely new layout. This section describes how perform a redesign by making changes to the currently loaded SCM sheet.

Use the following commands to change the $plname attribute value of the resistor R104 from minimelf to chip1206:

Symbols

Assign Value

Move to "r104",[210,130]

$plname

Attribute Value ?

chip1206

Return

With the commands above the package type assignment for the resistor part R104 has been changed. Use the following commands to assign value so14 to the $plname attribute of each gate of part IC1, thus defining a non-default package type for IC1 (the default package type was dil14):

Symbols

Assign Value

Move to "ic1.5",[60,110]

$plname

Attribute Value ?

so14

Assign Value

Move to "ic1.1",[100,110]

$plname

Attribute Value ?

so14

Assign Value

Move to "ic1.8",[140,110]

$plname

Attribute Value ?

so14

Assign Value

Move to "ic1.13",[180,110]

$plname

Attribute Value ?

so14

Use the following commands to save the currently loaded SCM sheet and load sheet2:

File

Save

Load

Sheet

File Name ?

Element Name ?

sheet2

The currently loaded SCM sheet contains some Autorouter control parameter settings (net attribute assignments), which should be modified. Use the following commands to change the ROUTWIDTH net attribute of NET from 0.5mm to 0.3mm, change the ROUTWIDTH attribute of net Vss from 0.6mm to 0.45mm and change the MINDIST attribute for net Vdd from 0.4mm to 0.3mm:

Symbols

Assign Value

Move to "NET"/Routwidth Symbol

$val

Attribute Value ?

0.3

Assign Value

Move to "Vss"/Routwidth Symbol

$val

Attribute Value ?

0.45

Assign Value

Move to "Vdd"/Mindist Symbol

$val

Attribute Value ?

0.3

Use the following commands to return to the BAE main menu (the currently loaded SCM element is automatically saved):

File

Main Menu

Now the BAE main menu is activated. Use the following commands to run the Packager to transfer the SCM changes to the layout, i.e., to the physical net list named board (the demo.ddb job file can be used as design library since it contains all of the information required for packaging):

Packager

Design File Name ?

demo

Design Library Name ?

demo

Layout Element Name ?

board

The Packager issues the No error occurred! message after successfully completing the forward annotation to the layout. Hit any key to return to the BAE main menu and use the following command to start the Layout Editor:

Layout

Now the Layout Editor is activated. Use the following commands to load the annotated layout:

File

Load Element

Layout

File Name ?

demo

Element Name ?

board

A connectivity generation is accomplished after loading the layout. Note that there are no airlines connected anymore to the parts IC1 and R104, since the package types have been changed for these parts. Use the following commands to delete all parts with changed package type assignments introduced by net list modifications:

Parts

Delete Update

Please confirm (Y/N) ?

The confirm prompt is only activated if there are parts placed with wrong package types. The Delete Update function can be used for checking the layout for wrong package types (simply type n to the confirm prompt if you want to abort the Delete Update function). The Delete Update call from above deletes the parts R104 and IC1 from the layout and issues the following message:

2 Parts deleted!

Use the following commands to place the previously deleted parts with correct package types:

Parts

Add Part

Part Name ?

ic1

Jump Absolute

Absolute X Coordinate (mm/") ?

1.6"

Absolute X Coordinate (mm/") ?

2.0"

Place Next Part

Mirror On

Rotate Right

Jump Absolute

Absolute X Coordinate (mm/") ?

0.35"

Absolute Y Coordinate (mm/") ?

2.0"

Now all parts are placed again on the layout. You can check this with the Place next Part function which should issue the All parts have been placed already! message.

^Contents <>

4.6.5 Defining and Editing Power Layers

The Bartels AutoEngineer layout system provides features for defining power layers and/or power planes. Use the following commands to define a power layer for signal Vss:

Settings

Set Power Layers

1: ---

Net Name ?

vss

End

Note how the above-mentioned power layer definition removes the airlines connected to the drilled pins of signal Vss. Drilled pins are automatically connected to the corresponding power layer (i.e., the CAM Processor will later generate heat traps at the drillings of power layer pins). The airlines connected to the SMD pins of signal Vss won't be deleted, i.e., the Autorouter will automatically connect these pins to the power layer using vias.

Power layer definitions can be displayed in the BAE layout system. Use the following commands to set the color for power layer 1 to dark blue:

Change Colors

Power 1

Move to Desired Color, dark blue

Exit

On the display of drilled pin definitions there is a distinction whether the pin is connected to a power layer or not. Power layer connections are displayed as circle outlines; isolations, i.e., drills which are not to be connected to any power layer, are displayed as filled circles.

The layer selection menus of the Add Active Copper function from the Areas menu allow for the selection of power layers. Power planes or isolated areas (net name -) can be placed on power layers to perform split power plane editing, i.e., to define more than one signal on a single power layer. Power planes are displayed with their outlines which will later be interpreted as isolation line by the CAM Processor (see also chapter 4.7.6 of this manual). There is a restriction that no power plane can overlap any other power plane partially since this would cause an ambiguity in the power plane tree detection algorithms. Partial power plane overlaps will cause the design rule check to issue power layer errors; the number of power plane errors detected by the DRC is shown with the Power Layer Errors entry of the Report Utilities function. Power planes completely enclosed by other power planes are allowed; the power plane tree detection will always match the "innermost" power plane for connecting.

The layer selection menus of the Add Text function from the Text, Drill menu allow for the selection of power layers. Text can be placed on power layers to add documentary information to the power layers. When placing text on power layers, the design rule check will perform distance checking against the All Layers and Middle Layers signal layers. Power layer text is visible on the PCB only if the corresponding power layer is configured as board outside layer (i.e., as either solder side or component side layer). Usually power layers are defined as board inside layers of a multilayer design. Text placed on power layers can serve as control information (e.g., for the layout designer or as plot or film archive information).

^Contents <>

4.6.6 Autorouter Via Keepout Areas

There is often the need to define areas where the Autorouter is allowed to rout traces but must not place vias (e.g., underneath special parts). Via keepout areas can be defined on a routing layer which is not required for the real layout. This "via keepout layer" should then be prohibited with the Autorouter layer assignment. The Autorouter considers all objects placed on prohibited layers, and vias and/or via drill holes are assumed to be defined on all layers. I.e., the Autorouter refrains from placing vias at positions where via pads would intersect with keepout areas on prohibited routing layers.

Use the following commands to place a keepout area on layer 3 matching the region underneath the switches s1000 through s1009:

Areas

Add Keep Out Area

Layer 3

Move to [0.25",0.4"]

Move to [0.45",0.4"]

Move to [0.45",2.4"]

Move to [0.25",2.4"]

Done

Use the following commands to start the Autorouter (the currently loaded layout will automatically be saved):

File

Autorouter

Use the following commands to define routing layer 3 to be prohibited and start the Full Autorouter (the Autorouter options such as routing grid, trace width, clearance, etc., have already been defined with the previous Autorouter session):

Options

Layer Assignment

Select Layer Number ?

Select Layer Type (P/H/V/A/-) ?

Select Layer Number ?

Autorouter

Full Autorouter

The Full Autorouter will a find 100% routing solution with no vias placed inside the via keepout area. Note also how the SMD pins of the previously defined power layer Vss (see above) are automatically connected using short traces with vias.

Use the following command to return to the Layout Editor after successfully completing the autorouting:

File

Layout Editor

^Contents <>

4.6.7 Area Mirror Mode

The Mirror Display function from the Layout Editor Areas menu is used to set special display attributes for selectable areas. The Visible always option is the default display mode for any area. Visible always defines the selected area to be always visible. The Visible unmirrored option defines the selected area to be visible only when unmirrored (i.e., when placed on the component side). The Visible mirrored option defines the selected area to be visible only when mirrored (i.e., when placed on the solder side). The Mirror Display function can be used on part, padstack and pad level. It is possible to define SMD parts with differently shaped pads or keepout areas depending on which side of the board the part is placed (for supporting different soldering processes on solder and/or component side).

Use the following commands to load the pad symbol p1206 from the demo.ddb DDB file:

File

Load Element

Pad

File Name ?

demo

Element Name ?

p1206

There is finger-shaped contact area defined on the currently loaded p1206 pad. Use the following commands to define this copper area to be visible only when unmirrored (i.e., when placed on the component side):

Areas

Mirror Display

Move to Area Edge

Visible unmirrored

Now the component side pad shape is defined. Use the following commands to define a rectangle-shaped passive copper area to be visible only when mirrored (i.e., when placed on the solder side):

Areas

Add Passive Copper

Jump Absolute

Absolute X Coordinate (mm/") ?

0.6

Absolute Y Coordinate (mm/") ?

0.9

Jump Relative

Relative X Coordinate (mm/") ?

-1.2

Relative Y Coordinate (mm/") ?

Jump Relative

Relative X Coordinate (mm/") ?

Relative Y Coordinate (mm/") ?

-1.8

Jump Relative

Relative X Coordinate (mm/") ?

1.2

Relative Y Coordinate (mm/") ?

Done

Areas

Mirror Display

Move to Area Corner/Edge

Visible mirrored

Use the following commands to save the currently loaded pad symbol and re-load the layout:

File

Save Element

Load Element

Layout

File Name ?

Element Name ?

board

The system accomplishes a connectivity generation to correlate the library modifications with the current net list definition. The p1206 pad is used on the s1206 padstack symbol, which, in turn, is used on the chip1206 part symbol. Note how the layout system uses different pad shapes for the mirrored parts R104 and C101 and for the unmirrored part R105.

The Mirror Display function can be applied on any copper, keepout or documentary polygon defined on a library element which can be mirrored. You can also use this feature to define part keepout areas on documentary layers to perform different part clearance checks depending on which side of the board the parts are placed.

Reflow-Reflow SMT/SMD Soldering Support

A control for setting the Area Mirror Display parameter is provided in the Settings dialog from the Settings menu to support reflow-reflow SMD/SMT soldering techniques. On default, the Mirror Display parameter is activated, and polygons with the Visible unmirrored, attribute are only visible when not mirrored, whilst polygons with the Visible mirrored attribute are only visible when mirrored. However, with the Mirror Display, parameter deactivated, all polygons declared as Visible unmirrored, are always visible, and all polygons declared as Visible mirrored, are never visible, independently of any (part) mirroring. Mirror Display, deactivation allows for SMD libraries designed for conventional SMD soldering to be re-used for reflow-reflow SMD soldering.

^Contents <>

4.6.8 Automatic Copper Fill

The BAE layout system provides powerful automatic copper fill functions with user-definable minimum structure size and isolation distance. The copper fill algorithm support isolated copper area elimination and automatic heat trap generation with adjustable connection widths and heat-trap-specific isolation distances.

The copper fill functions are available through the Copper Fill submenu of the Layout Editor Areas menu.

Copper Fill Parameters

Depending on the current BAE menu setup, copper fill parameters can either be set from the Settings dialog of the Copper Fill submenu or through dedicated menu functions in that same menu.

The Set Fill Clearance function is used to set the copper fill isolation distance parameter for the copper fill algorithm (default 0.3mm). The copper fill clearance distance is applied on default unless some net-specific minimum distance settings are defined through MINDIST net attributes (see chapter 7.11). Net-specific minimum distance attribute settings are considered individually.

The Min. Fill Size function is used to define the minimum structure size for area generation (default 0.1mm). This value should correspond with the smallest Gerber aperture size to ensure valid Gerber photoplot data generation without overdraw errors.

The Round Corners option of the Traces Cut Mode function causes the copper fill algorithm to generate arc-shaped concave area borders during trace segment isolation; on default octagonal circle interpolation is applied (option Octagonal Corners).

The Keep Islands option of the Insol. Area Mode function switches off isolated copper area recognition (i.e., the copper washes over the pad that it is to connect to); on default, isolated copper areas are automatically eliminated during active copper generation (option Delete Islands). The Select Islands option keeps isolated areas and automatically selects them to the current group as they are created.

The Heat Trap Mode options also support for different processing modes for pins and vias. It is possible to decide whether heat-trap connections should be generated for both pins and vias (option Pin & Via Heat Traps), for pins only (option Pin Heat Traps), for vias only (option Via Heat Traps), or if direct connections only should be generated (option Direct Connect).

The Direct Connect option of the Heat Trap Mode function deactivates automatic heat trap generation when filling active copper. The default Heat Trap Mode option Use Heat Traps is used to activate automatic heat trap generation, i.e., to create thermal relieves for copper area connections. With Use Heat Traps selected, the system prompts for the heat-trap junction width and an optional heat-trap-specific clearance distance, where invalid inputs won't change current settings. On default, the heat trap junction width is set to 0.3mm and the heat-trap clearance is set to zero (i.e., heat-traps are isolated using standard minimum clearance settings).

BAE HighEnd provides the HT-Junction option for specifying the maximum heat-trap connections count (1, 2, 3 or 4). The default heat-trap generation sequence is left, right, bottom, top.

Copper Fill Workarea Definition

Copper fill workareas are required for copper fill functions to operate. Use the following Layout Editor commands to define a rectangle-shaped copper fill workarea on layer 1 for the signal named net:

Areas

Copper Fill

Add Cop.-Fill Area

Net Name ?

net

Layer 1

Move to [0.6",0.4"]

Move to [1.7",0.4"]

Move to [1.7",1.7"]

Move to [0.6",1.7"]

Done

A dash string input (-) to the net name prompt of the Add Cop.-Fill Area function creates a copper fill workarea which is not assigned to any net. This feature can be used for generating pure shielding areas.

Passive copper areas with signal net connections (e.g., teardrops created as passive copper) are treated like active copper areas of that net and won't be isolated from copper fill areas of that net.

Automatic Copper Fill

The Fill all areas, Fill single area, Clear all areas and Clear single area functions are used to activate automatic copper fill procedures. Fill all areas performs automatic copper fill on all copper fill workareas. Clear all areas deletes copper areas from all copper fill workareas. With Fill single area and Clear single area, the user is expected to select the desired copper fill workarea.

Use the following commands to set the isolation distance to 0.35mm, specify a minimum structure size of 0.15mm, deactivate the automatic isolated copper area elimination and fill the predefined workarea:

Areas

Copper Fill

Set Fill Clearance

Copper Clearance Distance ( 0.30mm) ?

0.35

Min. Fill Size

Min. Fill Structure Size ( 0.10mm) ?

0.15

Insol. Area Mode

Keep Islands

Fill single area

Move to Copper Fill Workarea

The system fills the selected workarea with active copper assigned to the signal named net and isolated from other signal levels. The copper fill process is very laborious and might last a few moments to complete. You should perform a screen redraw and examine the results after the copper fille procedure is completed. You can reset the copper fill, change the copper fill parameters and re-apply the copper fill function if you are not satisfied with the results (maybe because of either too small or too large structures being generated).

Use the following commands to reset the copper fill from above and re-apply the copper fill with automatic isolated area generation:

Areas

Copper Fill

Clear single area

Insol. Area Mode

Delete Islands

Fill all areas

The minimum structure size (i.e., the smallest area size to be generated with copper fill) has basic meaning for subsequent CAM Processor. The copper fill algorithm uses the minimum structure size for automatically rounding off convex corners to avoid acute-angled areas. You should specify the minimum structure size according to the size of the smallest round aperture defined for Gerber output to ensure that Gerber photoplot data can be generated without overdraw errors (see also chapter 4.7 of this manual).

Copper Fill Complexity

The CPU time and memory requirements of the copper fill algorithm strongly depend on the quantity and complexity of the structures to be isolated and/or generated. Orthogonal structures make the job much easier than e.g., arc-shaped objects since a lot more time consuming geometric distance calculations and complex floating point operations are required for the latter. Figure 4-8 elucidates how the complexity of the objects to be isolated and particularly their mutual positioning strongly affects memory requirements during copper fill. Note, however, that figure 4-8 does not show what large amount of temporary data is required for the area reduction and expansion algorithms used for generating correct copper fill areas. Defining more smaller copper fill workareas instead of a few large ones can often be the workaround when running into memory problems using the copper fill function on main memory limited PC systems.

Figure 4-8: Automatic Copper Fill Complexity

You can use one of the Octagonal Corners, Octagonal Circles and Octagonal Corners+Circles options instead of the Round Corners default option from the Traces Cut Mode function to reduce the complexity and number of fill areas. This allows for trace corners and/or full circles to be isolated like octagons, thus also reducing the amount of Gerber data if no Gerber arc commands can be used.

To avoid long response times after unintentionally activating the copper fill function, automatic copper fill can be canceled by pressing any key and confirming the abort request with a verification menu. Note, however, that canceling is not possible anymore at the final stage of connectivity generation, and that areas generated before the abort request must be explicitly eliminated using the Undo function.

Using the copper fill function considerably increases the number of copper areas and polygon points. This raises the CPU time requirements for the Mincon function if the Mincon function type is set to a corner to corner airline calculation (see chapter 4.3.2 of this manual). In such cases it can be worthwhile to use a pin to pin calculation method to reduce Mincon CPU time requirements. The Mincon Function from the Layout Editor Settings menu is used to set the Mincon function type.

Copper Area Hatching

The Copper Fill submenu provides the Hatch Copper Area function for transforming copper areas into line or cross hatched areas with user-definable hatching width and hatching clearance.

Hatching is accomplished through trace segments generation. The width of the produced trace segments can be set with the Hatching Width function (default 0.3mm) whilst the spacing between produced trace segments can be set with the Hatching Spacing function (default 1/20 inch).

The Hatching Mode function is used to designate the hatching type. The default Line Hatching option generates hatch areas with diagonal trace segments. The Grid Hatching option generates hatch areas with crosswise intersecting diagonal trace segments.

The hatching process is activated by calling the Hatch Copper Area function and selecting the copper area to be hatched.

Use the following commands to set the coordinate display mode to inch, and transform the circle-shaped copper area on signal layer 2 of the layout to a line-hatched area with a hatching distance of 1mm:

Settings

Coordinate Display

Display Inch

Areas

Copper Fill

Hatching Distance

Hatching Line Spacing ( 1.27mm) ?

Hatch Copper Area

Move to Passive Copper Area/Signal Layer 2, [0.8",1.8"]

Use the following commands to set the hatching width to 0.2mm and transform the active copper area (signal vdd) on signal layer 1 of the layout into a cross-hatched area:

Areas

Copper Fill

Hatching Width

Hatching Line Width ( 0.30mm) ?

0.2

Hatching Mode

Grid Hatching

Hatch Copper Area

Move to Active Copper Area "vdd"/Signal Layer 1, [2.5",2.0"]

The Hatch Copper Area function generates a special layout polygon type called hatched copper area. The hatching and the hatching area outline are generated using traces with a trace width according to the hatching width setting. The traces are strongly connected with the hatched copper polygon to support general Layout Editor polygon functions such as Move Area or Delete Area.

The PCB layout example should now look like the one shown in figure 4-9 if you correctly executed all operations.

Figure 4-9: Layout with Filled Copper Areas

This might be a good time to save the layout:

File

Save Element

^Contents <>

4.6.9 Library Update

The Update Library function is one of the most powerful features of the Bartels AutoEngineer. Update Library is usually used to update a job-specific library in order to correlate it with the contents of some master library.

Use the following commands to copy the currently loaded layout to the democopy.ddb DDB file (with default layout element name), and load the copied layout:

File

Save Element As

File Name ?

democopy

Element Name ?

Load Element

Layout

File Name ?

democopy

Element Name ?

Now the copied layout appears on the screen. However, this layout contains only those objects which are directly defined on the layout. The lower level library elements (parts, padstacks, pads) are not displayed since they have not been copied with the Save Element As function to prevent from overwriting existing library elements in the democopy.ddb destination file. The system will issue either the

Connected pins missing!

message or the

Cannot load all elements (display not complete)!

message in the status line. Use the following commands to correlate the job-specific library of DDB file democopy.ddb with the contents of DDB source file demo.ddb:

File

Update Library

Layout

File Name ?

Element Name ?

Source File Name ?

demo

After a few moments the system should issue a Library elements replaced! message which means that all library elements referenced from the currently loaded layout have been copied from the specified library source file. Use the following commands to re-load the layout in order to display the library update (Update Library works on DDB file level, it doesn't affect elements in main memory):

File

Load Element

Layout

File Name ?

Element Name ?

The Update Library function can also be used to correlate the job-specific library with the contents of a different layout library file. Use the following commands to perform a library update for the currently loaded layout using the library source file demolib.ddb, and re-load the layout (note how the r04a25 resistor package type is updated with the definition from demolib.ddb):

File

Update Library

Layout

File Name ?

Element Name ?

Source File Name ?

demolib

Load Element

Layout

File Name ?

Element Name ?

The Replace Element function is used for substituting selectable library elements with definitions from a certain library source file. Use the following commands to replace the r04a25 part symbol and the p1206 pad symbol of the current democopy.ddb DDB file with the corresponding definitions from the demo.ddb DDB file, and re-load the layout (Replace Element works on DDB file level, it doesn't affect elements in main memory):

File

Replace Element

Part

File Name ?

Element Name ?

r04a25

Source File Name ?

demo

Please confirm (Y/N) ?

Replace Element

Pad

File Name ?

Element Name ?

p1206

Source File Name ?

demo

Please confirm (Y/N) ?

Load Element

Layout

File Name ?

Element Name ?

^Contents <>

4.6.10 Back Net List

The Back Netlist function from the Utilities menu is most useful for certain applications such as high frequency design, where net list data is requested to be automatically generated from the copper located on the PCB.

The mode of operation of this function should be demonstrated using the currently loaded layout from DDB file democopy.ddb. Delete the trace which connects the pins NO1 and 4 of the parts named K1 and X1, and reset the definition of power layer vss:

Traces

Delete Trace

Move to Trace,e.g.[2.35",0.9"]

Settings

Set Power Layers

1: vss

Net Name ?

End

Note how the deleted trace and power layer definition are replaced with airlines. Use the following commands to add a trace to connect the pins 2 and 1 of the parts named R100 and R101:

Traces

Add Trace

Move to "R100.2",[1.4",2.4"]

Move to "R101.1",[1.6",2.4"]

Done

The system now indicates a short-circuit error. Use the following commands to save the layout, run Back Netlist to generate a net list with the same file and element name, and immediately re-load the layout again (Back Netlist stores to DDB file without changing the currently loaded net list data):

File

Save Element

Utilities

Back Netlist

File Name ?

Element Name ?

File

Load Element

Layout

File Name ?

Element Name ?

Now the system performs a connectivity generation to correlate the layout with the net list which was previously generated with Back Netlist. Note that there are no airlines displayed anymore after completing the connectivity generation. The layout does not contain any open connections and/or short-circuits anymore (you can check this with Batch DRC and Report from the Utilities menu). Deleting the trace which was previously causing a short-circuit would now result in an airline display.

Another useful application of the Back Netlist function net list generation from Gerber data which was previously loaded with the CAM View module (for more details see chapter 4.8 of this manual).

^Contents <>

4.6.11 Blind and Buried Vias

Blind and buried vias are partial vias which can be used for layer changes when routing multilayer layouts. Routing with blind and buried vias can considerably increase the routability of multilayer layouts with four or more signal layers.

The BAE Layout Editor features arbitrary pad layer assignment (see also chapter 4.2.2 for more details on creating padstacks) and drill classes to support the definition of blind and buried vias. Drill classes should be assigned to certain layer-sets to support CAM drill data output for selectable layer-sets (see also chapter 4.7 for more details on drill data output). There are no system-imposed restrictions on how to define and/or assign drill classes. You can, e.g., use drill class A for layer-set 1-2, drill class B for layer-set 2-3, drill class C for layer-set 3-4, etc. Note, however, that the drill class assignment must be considered for correct drill data output by the CAM Processor, and that the layout top layer setting (see also chapter 4.3.1) gains special meaning when using blind and buried vias.

A typical configuration for 4-layer layouts is the definition of the vias via (for all layers), via_12 (for layer-set 1-2), via_23 (for layer-set 2-3) and via_34 (for layer-set 3-4). All these vias are simultaneously available for routing when selected to the via list (see also chapter 4.3.4 for details on how to select vias)

The Change Layer Layout Editor command used during interactive routing automatically selects the via with the least possible layer occupancy. The same principle is applied by the Autorouter. At least one via for all signal layers required for autorouting. Additionally, the Autorouter can e.g., simultaneously use vias for the layer-sets 1-2-3, 1-2, 2-3, etc. However, to avoid backtracking ambiguities, the Autorouter is restricted in that it can not use vias with multiple mutually intersecting layers. I.e., the Autorouter refuses to use a via for layer-set 1-2-3 and another via for layer-set 2-3-4 at the same time (error message Invalid via padstack (cannot use it)!).

Using the CAM Processor for generating drill data output for the drill holes defined on partial vias requires corresponding drill class(es) to be specified.

The production of PCBs with blind and buried vias is usually more expensive than the production of standard multilayer boards. However, using blind and buried vias increases the routability of multilayer layouts and also supports advanced PCB manufacturing technologies such as plasma-etched via production processes.

^Contents <>

4.6.12 Exiting the Layout System

Don't forget to save the currently edited layout element before exiting the Layout Editor:

File

Save Element

Returning to Main Menu

The following commands can be used from each program module of the BAE layout system (except for the Autorouter) to return to the BAE Main Menu (BAE Shell):

File

Main Menu

The Main Menu function automatically saves the currently loaded layout element. From the BAE Shell, the following command can be used to return to the operating system:

Exit BAE

Exiting BAE

The following commands can be used from each program module of the BAE layout system to return to the operating system, i.e., to exit the Bartels AutoEngineer:

File

Exit BAE

The Exit BAE function activates a confirmation request if the currently loaded element has not yet been saved. In this case you should abort the Exit BAE function, save the current element, and then call Exit BAE again, as in:

File

Exit BAE

Please confirm (Y/N) ?

File

Save Element

File

Exit BAE

Bartels :: Bartels AutoEngineer :: BAE Documentation :: BAE User Manual :: PCB Design :: Special Layout Features

^Contents <>>

	© 1985-2024 Oliver Bartels F+E Bartels Homepage Contact and Corporate Info Web Development by Baumeister Mediasoft Engineering