OrCAD / Allegro PCB Editor Design Guide

Nordcad Systems A/S
support@nordcad.dk
VI HAR RESSOURCERNE …

Agenda
– Purpose
– Shortcuts
– Design topics
– Schematic preparation
– Netlisting
– Board outline
– Constraints
– Placement
– Routing
– Autorouting
– Shapes (copper pours/areas)
– Design Rule Check and design status
– Post Processing
– Data for manufacturing
• Requirements
– Installed company setup for paths,
shortcuts, templates etc.
– Libraries correct and configured

Purpose
• To aid the occasional user of PCB Editor in the most common and daily tasks
• To get more knowledge
– Attend training
– Try doing experiments
– It comes with experience
– Use online documentation
– Use http://sourcelink.cadence.com
– Signup at http://www.nordcad.dk/dk/teknik__service/e-service/
sourcelink_videndatabase_tilmelding.htm
– Receive technical tips and tricks from e-SERVICE newsletter
– Signup at http://www.nordcad.dk/dk/teknik__service/e-service/e-service_tilmelding.htm
• Comments and suggestions to this guide are welcome
– support@nordcad.dk

Important Shortcuts
• Standard windows shortcuts
– Save (Ctrl+s)
– File, Open (Ctrl+o)
– Undo/Redo (Ctrl+z/ctrl+y)
– Refresh screen (F5)
• See much more shortcuts much later in
this presentation
• More capabilities
– Slide (s + l)
– Pan (Middle mouse and hold)
– DRC Check (.)
– Measure (M)
– Change between widths (W ~ shift+w)
– Change to another width (lx)
– Change application mode (ctrl+a)
– Layer setup (l)
– Constraint Manager (c)
– Display Status (comma)
Legend: S=Shift, C=Ctrl, SC=Shift and Ctrl

OrCAD Capture and Layout like Shortcuts
– Zoom area (z)
– Zoom fit (Shift+Home)
– Add via at cursor location(V)
– Add via at last mouse click position (v)
– Place (p)
– Route (w)
– Zoom in (i or Ctrl + mouse wheel)
– Zoom out (o or Ctrl + mouse wheel)
– Horizontal scroll (Shift + mouse wheel)
– Vertical scroll (mouse wheel)
– Use arrow keys to scroll
up/down/left/right
– 1 turn top layer on/off
– 2 turn bottom layer on/off
– 3 turn layer3 on/off
– 4 turn layer4 on/off
– …
– Ctrl+7 turn solder mask top on/off
– Ctrl+8 turn solder mask bottom on/off
– Ctrl+9 turn solder paste top on/off
– Ctrl+Alt+0 turn solder paste bottomo
on/off
– Ctrl+Alt+1 turn silkscreen top on/off
– Ctrl+Alt+2 turn silkscreen bottom on/off
– Ctrl+Alt+3 turn assembly top on/off
– Ctrl+Alt+4 turn assembly bottom on/off
– Ctrl+Alt+5 turn drill on/off

Application modes
General Edit Application Mode
Objekt Type Drag Shift Drag Ctrl Drag
Group Move Move Copy
Symbol Move Spin Copy
Via Slide Move Copy
Cline Slide Move Copy
Line Move Move Copy
Shape Move Move Copy
Cline
Slide
Segment
Figure Move Move Copy
Text Move Move Copy
Rat Tee Slide Move
Etch Edit Application Mode
Objekt Type Drag Shift Drag Ctrl Drag Single klik
Group Move Move copy
Symbol Move Spin copy Move
Pin Move Add connect
Via Slide Move Copy Add connect
Cline
Shape Move Move copy
Cline Seg Slide Delay tune Slide
Rat Add connect
Rat Tee Slide Move
• Use ’ctrl+a’ to shift between
the 2 application modes
– Observe status bar (’EE’ or
’GEN’) to see current
application mode
• Mouse over object and use
action or right click to get
options
– Mouse over and pressing
’TAB’ shifts between object
types

Schematic preparation
– Edit properties on Nets and Comps
– How
– Select one or more nets/components
– Ctrl+E to edit properties
– Select Filter By to ’Cadence-Allegro’
– Net Properties – use Flat Nets
– ’Min_line_width’ is the default width used
during routing
– ’Net_physical_type’ puts net into netclass
for easier handling of width and via
assignments
– ’Net_spacing_type’ puts net into netclass
for defining advanced spacing constraints
– Netclass (spacing and physical type)
definitions are needed for auto matchup
towards board template
– Component properties
– ’Room’ used to group components for
easier placement
Constraints = Design Rules

Spacing and physical rule matchup
• Use the following Net_Physical_type
names to get constraints as shown
• Use the following Net_spacing_type
names to get constraints as shown
Net_Physical_Type Width Via type
<None> 0.2mm via26
Power 0.5mm via40
AD 0.1mm via26
Constraint Sets in PCB Editor
01mm 0.1mm via26
02mm 0.2mm via26
05mm 0.5mm via40
Via names Size Hole
Via40 1mm 0.6mm
Via26 0.7mm 0.3mm
via75 2mm 1mm
Net_Spacing_Type <None> Power AD
<None> 0.2mm 0.5mm 0.2mm
Power 0.5mm 0.5mm
AD 0.1mm
Constraint Sets in PCB Editor L-L L-S V-S V-V V-P
01mm 0.1mm 0.1mm 0.1mm 0.1mm 0.1mm
02mm 0.2mm 0.2mm 0.2mm 0.2mm 0.2mm
05mm 0.5mm 0.5mm 0.5mm 0.5mm 0.5mm
Legend Type Description
L Line Track/cline
P Pin Component pin
S Shape Copper pour/area
V Via
• Individual Constraints (properties like Min_line_width) overrule above table per default
• See animation slide for creating constraint sets and matchup as shown above

Netlisting
– Tools, Create Netlist
– Choose PCB Editor tab
– Select
– Create PCB Editor Netlist
– Leave ’Nelist Files Directory’ as is
– First time netlisting on job
– Select ’Create or Update ..’
– Specify ’Input Board File’ to template
– Leave ’Output Board File’ as is
– Already started on PCB job
– Select ’Create or Update ..’
– Specify ’Input Board File’ to existing job
– Add number to ’Output Board File’
– Choose ”Board Launching Option” to
– ”Allegro” for installation from Allegro CD’s
– ”OrCAD” for installation from OrCAD CD’s

Board Outline
– Setup, Outlines, Board Outline
– Select Create
– Specify the ’Board Edge
Clearance’
– Creates route and place keepin
at a distance inside outline
– Takes care of spacing to the
edge of the PCB
– Select ’Create Option’
– ’Draw Rectangle’ to draw a
rectangle
– ’Place Rectangle’ to specify
size in design units
– ’Draw Polygon’ to make any
kind of outline
– To edit, move or delete the
outline select the command
Setup, Outline, Board Outline
again

Board Outline – the DXF way
• File, Import, DXF
– See movie for
guidelines
• Use Edit, Z-copy to
create
– route keepin
– Package keepin

Constraints
• How
– ’c’ for Constraint Manager
– Excel like spreadsheet with constraint
values
– Preferred method
– Create Constraint Sets (Csets)
– In ”Physical/Spacing Constraint Set” section of
constraint manager
– Let Net and NetClasses reference these
Csets
– Use ”Referenced Physical/Spoacing CSet”
column
– Individual constraints can be set
– Blue values denotes overrides
– On net
– Mouse over net, Right click, Property Edit

Placement
• Press ”p” for placement dialog
– Filter components by room, net, refdes etc.
– To place using coordinates click p-icon at
the bottom
• Most used Place Shortcuts
– Rotate 90 degree (r)
– Rotate 45 degree (R)
– Rotate other angles
– Set angle in options panel
– Mirror (m)
– Place by coordinate (x or y)
– ’P’ for hidden placement dialog
– Use to move placed components

Routing
• Shift to ’EE’ application mode
– Use ’ctrl+a’ until status bar shows ’EE’
– Click rat, pin or via to add connect
– Click cline to slide
– Change settings during route using Right click
options or Options panel
– Layer and net informtion can be seen in status bar
• Most used Route shortcuts
– Route (w)
– Change between widths (W)
– Change corner type (A)
– Finish route (f)
– Slide (s)
– Add via at mouse cursor (V)
– Add via (v or double click)
– Toggle corner (ctrl + t)
– Change routing layer (+/-)

Shapes (copper pours/areas)
• Add shape using icons
– Adjust settings in Options panel
– Draw using mouse
– Change existing shape
– Shape Select
• Change global parameters for shapes
– Shape, Dynamic Params
• Change object parameters
– Mouse-Over, right click, property Edit
– Use Dyn_xxx properties
• Delete islands
– Use Options panel to control delete
operation

Design Rule Check and Design Status
• Run Design Rule Check
– Press . (point sign) or icon
• In case of DRC errors
– Get information using Mouse over DRC
marker, right click, show element
– Waive any DRC errors that are
acceptable.
– Mouse over, Right click, Waive DRC
• Footprint library path check
– Tools, Quick Reports, Symbol Library
Path Report
– Will show if all footprints are taken from
company footprint library
• Display Status
– Press , (comma)

Post processing
– Double check Display, Status menu
– Create drill legend (drawing)
– Manufacture, NC, Drill customization
– Click ’Autogenerate symbols’ for unique drill
symbols to each drill type/size
– Manufacture, NC, Drill Legend
– Adjust settings to your need and press OK
– Now place the legend on the PCB
– Create drill files
– Manufacture, NC, NC Drill
– Check settings and press ’Drill’
– Create Route files (if slots are present)
– Manufacture, NC, NC Route
– Check settings and press ’Route’
– Ipc out
– File, Export, IPC 356 and click export

Post processing
– Create Pick and place data
– File, Export, Placement
– Select the correct option and press Export
– Create Gerber films
– Custom, Create Gerber Settings to create the
gerber films necessary
– Create Gerber data
– Select Manufacture, Artwork
– Check that all settings are as expected

Data for manufacturing
• Gerber RS274X (Extended Gerber) or ODB++
use is recommended
– All gerber files get the filmname specified in the Artwork
dialog and file extension ’.art’
– Navnene tager udgangspunkt i vores setup
– 1_TOP.art (copper layer)
– 2_GND.art (copper layer)
– 3_VCC.art (copper layer)
– 4_BOTTOM.art (copper layer)
– Soldermask_top.art (solder mask top)
– Soldermask_bot.art (solder mask bottom)
– Solderpaste_top.art (solder paste top)
– Solderpaste_bot.art (solder paste bottom)
– Silkscreen_top.art (silkscreen top)
– Silkscreen_bot.art (silkscreen bottom)
– Assembly_top.art (assembly top)
– Assembly_bot.art (assembly bottom)
– Board_outline.art (Board outline)
– NCLEGEND-x-y.art (drill drawing)
– Where ’x’ is the start layer and ’y’ the end layer for drill
– Use of blind/buried vias will create more ’.art’ files
• Drillfiles
– Designname-x-y.drl (plated holes)
– Where ’x’ is the start layer and ’y’ the end layer for drill
– Designnavn-x-y-np.drl (non-plated holes)
– nc_tools_auto.txt (drill sizes)
– Also embedded into ’.drl’ files if ’Enhanced Excellon’ is used
• Pick’n’place data
– Place_txt.tx (x,y coordinates)
• IPC-356 netlist
– Designname.ipc
• Remember to create a text file that describes
all file types. E.g., use data shown on this
page.
• Zip all this up and send to PCB manufacturer
• Add text description separately
• Ask manufacturer to check gerber and
compare against IPC netlist file.

Appendix – Create design template
• 2 Slides
– First describes constraints to be
implemented
– Second shows how this setup can be
accomplished

Nordcad Systems A/S

Agenda
• Agenda
– Purpose
– Configuration
– Shortcuts
– Add-on programs in NsWare, Nordcad and
PCB Flow menu
• Preparation
– Decide a directory for company setup and
configuration
– E.g., C:CadenceCompany
– Change this to network drive. Above is used
during this setup guide for explanation

Purpose
• To customize and setup the PCB Editor for
– most efficient use
– standardizing on a common company setup for library and setup management
– Can be used as a single user setup also – see next page
• To get more knowledge
– Attend training
– Try doing experiments
– It comes with experience
– Use online documentation
– Use http://support.cadence.com
– Signup at http://www.nordcad.dk/dk/teknik__service/e-service/sourcelink_videndatabase_tilmelding.htm
– Receive technical tips and tricks from e-SERVICE newsletter
– Signup at http://www.nordcad.dk/dk/teknik__service/e-service/e-service_tilmelding.htm
• Comments and suggestions to this guide are welcome
– support@nordcad.dk

Get configuration files
• Notice: If you downloaded and installed SmartStart all the configuration is
done during installation
• Download from
– http://www.nordcad.dk/dk/teknik__service/downloads/setupguide.htm
• Unzip to directory of your choice
– Will create the directory structure shown
• Single user setup
– Run ’PCBEditor_Setup.bat’ to use as is
– Will not establish company setup!
– Will establish setup files on individual PC
• Company configuration
– Installation guide on next page

Install setup
• Do the following
– Copy the complete pcb folder to a directory of your choice
– In the example C:CadenceCompany is used
– Change ’C:CadenceCompany’ directory path to your own directory
choice inside ’setup_regdata.reg’ (use text editor)
– Install client data by running PCBEditor_user.bat
– Go to Control Panel → System → Advanced → Environment
Variables
– Click OK
• Now you can start PCB Editor and it will contain the new settings

• Place your own files in the correct directories
• Padstack files
– .pad
• Symbols
– Package (.psm) ~ footprint
– Shape (.ssm) for use in padstack
– Flash (.fsm) for use in padstack
– Format (.osm) is logos and titleblocks
– Mechanical (.bsm) is outlines, mounting holes etc.
• More directories are described on the next page
27
Directory structure at
C:CadenceCompany
Padstack files (.pad)
Contain pad definitions
All types of symbols including footprints
(.psm, .bsm, .fsm, .osm, .ssm)

28
Directory structure at
C:CadenceCompany
Device files for 3rd party netlist
import (.txt)
DFx check setup(.arl & rle)
(Performance Option)
DFA setup (.dfa)
(XL & GXL)
Extracta command files (.txt)
Used for custom reports
Tools → Reports
Dialog windows (.form) for skill
programs
Bitmap pictures (.bmp) for skill
dialog windows
Drill legend templates (.txt)
Scripts (.scr)
File → Script
Technology files (.tech)
Menu files (.men)
Parameter files (.prm)
File → Import → Parameters
Signoise models & IBIS models
(.dat, .wave, .ibs, .mod, .ctl)
Read readme.txt in directory
Visibility setup (.color)
Found in the Visibility panel
Crosstalk tabels (.xtb)
For autorouting with PCB Router
PS: Use Topology directory for
topology templates

Shortcut and setup
• All company configurations are stored in
– ’site.env’
– This includes shortcuts
• All user setup is stored in
– ’C:Cadenceuser_setupenv’
– Changes made using the Environment editor will be
saved inside this file.

Shortcuts
Keyboard combination Functionality
spacebar Minimizes connections during ’place, manually’
comma (,) Status manager
point (.) DRC update
”a” Toggle rats on/off
”A” Toggle between corner types (45, 90 and off) during ’route’ and ’slide’
”Ctrl+a” Toggle between application modes (General, Etch Edit and Placement)
”b” Design Parameter dialog
”c” Constraint Manager
”C” Show constraints
”d” Done (right mouse click → Done)
”f” Finished current route (single net autoroute)
”g” Toggle grid display on/off
”ly” Opens Cross-Section (layer stackup)
”lx” Change width during add connect (illegal or no value return to constraint val)
”L” Fix
”h” Toggle ’bubble’ during ’route’ and ’slide’
”H” hilight
”i” Zoom in
”J” Dehighlight
Notice many changes compared to earlier setup guides

”m” Mirror component to other side of PCB during placement
”M” Measure
”n” Next
”o” Zoom out
”p” Place manually
”P” Place manually with hidden dialog, very good for moving components
”q” Show element (query items)
”r” Rotate with 90 degree increments
”R” Rotate with 45 degree increments
”s+c” Snap to arc or circle center
”s+f” Snap to figure
”s+i” Snap to intersection
”s+l” Activates slide command
”s+f” Snap to figure
”s+p” Snap to pin
”s+v” Snap to via
Shortcuts
”s+s+m” Snap to Segment Midpoint
”s+s+o” Snap to Symbol Origin
”s+s+v” Snap to Segment Vertex

”S” Toggle shadow mode on/off (very good function for review)
”t” Delay tune
”ctrl+t” Toggle cline segments between horizontal and diagonal during route
”V” Add via at cursor location
”v” Add via at latest mouse click location
”w” Activate ’add connect’ command (interactive routing)
”W” Toggle cline (track) width during routing between 0.1, 0.3, 0.5, 1, 1.5 and 2
”X” Route from the other end of connection (exchange ends)
”alt+F1” List of available commands and help on commands
Shortcuts
”ctrl+s” Save
”x” or ”y” Specify coordinate.
”ctrl+y” Redo
”z” Zoom area
”ctrl+z” Undo
”shift + home” Zoom fit
”Del” Activates Delete command
F12 Show scroll button and shortcut definitions
”Home” Zoom fit

”ctrl+0” → ”ctrl+6” Toggle inner layer 9 → 15 on/off
”ctrl+7” and ”ctrl+8” Toggle soldermask top (7) or bottom (8) information on/off
”alt+ctrl+1” and ”alt+ctrl+2” Toggle silkscreen top (1) or bottom (2) information on/off
”alt+ctrl+3” and ”alt+ctrl+4” Toggle assembly top (3) or bottom (4) information on/off
Shortcuts
Hold Middle mouse button (scroll wheel) Pan
Mouse scroll wheel Scroll vertically
Ctrl+mouse scrooll wheel Zoom in/out
Shift+mouse scroll wheel Scroll horizontally
Shift+ctrl+mouse scroll wheel Change active subclass
Arrow keys Pan up/down/left/right
”0” Toggle all layer information on/off
”1” Toggle top layer information on/off
”2” Toggle bottom layer information on/off
”3” → ”9” Toggle inner layer 3 → 8 information on/off
”ctrl+9” Toggle pastemask top information on/off
”alt+ctrl+0” Toggle pastemask bottom information on/off
”alt+ctrl+5” Toggle drill layer information on/off
”alt+ctrl+8” Toggle dimensioning information on/off

• Use the file 'user.men'
– Placed in C:Cadenceuser_setupmenu
• Add MENUITEMS and specify command to be used for
this
34
Change Example menu

OrCAD / Allegro PCB Editor Design Guide

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Similar to OrCAD / Allegro PCB Editor Design Guide

Similar to OrCAD / Allegro PCB Editor Design Guide (20)

Recently uploaded

Recently uploaded (20)

OrCAD / Allegro PCB Editor Design Guide