Adding a via has traditionally been done with a double-click of the LMB. Using the Space Bar can save you several thousand mouse clicks per year. The Space Bar is an easy key to click and hence best for adding vias.

funckey " " "pop bbdrill -cursor" (double quote space double quote)

Adding Vias: Working Layer model

The Working Layer (WL) model is the recommended method to add conventional or HDI vias.

Select your target routing layer from a popup GUI that appears adjacent to the via insertion area.
Go into the Add Connect command, and then select WL in the Options Panel.

A pop-up list appears.
Enable the layers you want to see each time you pop a via.
In Add Connect, choose WL
Select Target Layer during routing

What if you wanted to use HDI vias as the priority vias, and use the through-hole as an exception?

Open Constraint Manager and navigate to the Physical domain.
Click on
Via List cell and note the order of the vias. via019 is first used ahead of the microvias.
Use the down-arrow button to move via019 to the end of the list.
Add the through-hole via (via019) by selecting the (â€¦) button. This is how we access the least preferred vias in the via list.

Deleting a via in a stack

Use Edit - Delete, select the stacked via, and then right-click and choose Split Stack command. From the pop-up list, select the layer pair to delete.

Add Connect: Single-click execution

In the Etch Edit Application mode, make a single pick on a pin, via or rat to begin using Add Connect. Ensure the Enable Single Pick Execution mode is enabled. Access this option by right-clicking and choosing Customize menu.

Add Connect: Add a vertex using a Funckey key

Instead of using the LMB to add a vertex point during Add Connect, consider using a Function Key. You can simply click the X key every time you want to add a vertex during routing.

funckey x "pick_to_grid -cursor"

Add Connect: Prevent null net routing

PCB Designers move the mouse a lot faster. It is easy to make a pick in open space when the intent is to pick on a pin or a dangling end segment.

Set the acon_disable_nullnet_route variable in the User Preference Editor to prevent accidental picks that invoke Add Connect.

Add Connect: Toggle Corner

During the Add Connect command, use the F2 key to toggle the corners between arc and line.
Route one signal and press the F2 key four times to experience dynamic corner behavior.

alias a1 'FORM mini lock_mode Arc;FORM mini lock_direction 45' alias a2 'FORM mini lock_mode Arc;FORM mini lock_direction 90' alias a3 'FORM mini lock_mode Line;FORM mini lock_direction 45' alias a4 'FORM mini lock_mode Line;FORM mini lock_direction 90' alias F2 'settoggle CMD a1 a2 a3 a4;$CMD'

Add Connect: Add a vertex at cursor location

Instead of clicking to add a vertex point during Add Connect, consider using a Function Key. This will save you thousands of mouse picks per year. However, it will take some time to get used to.

You can simply press the X key every time you want to add a vertex during routing. funckey x "pick_to_grid -cursor"

Consider other applications, such as move components and move text, that might also leverage this command.

Changing line width during Add Connect

Not all the line widths are derived from Physical Csets or Regions. Consider creating function keys for the typical line widths you use that are not constraint defined. For example, the GND net may be defined as 10 mils but you might decide to widen at various locations (large pad components). This function key changes the current line width to 25 during the ADD Connect command.

funckey 9 form mini acon_line_width 25

Curving the corners

Use Slide - Vertex Action - Arc Corner or consider the Auto-Interactive Convert Corner command if you wish to convert corners across a larger group of signals.

Disabling shape fill when shapes become disabled

This user preference variable disables the filling of dynamic shapes when these become out of date. This may reduce the need to move shapes off the edge of the board outline when setting the shape fill mode to disabled:

Working in Etch Edit Application Mode

When in Etch Edit Application Mode, you can:

Make a single pick on a pin, via or rat line to begin Add Connect
Even move a component by holding down (drag) the mouse and press ESC key to release drag
Make a pick on a cline segment to invoke the slide command
Easily change the width or fix a cline or segment by hovering over it and then using the pop-up context menu.

Suppress Rats during Add Connect

Want to de-clutter the screen when routing? Consider enabling the "Auto-blank other rats" option. When enabled, all rats other than the primary ones are suppressed during the Add Connect command (Introduced in release 16.6 QIR6).

Expand/Contract a shape or void

Select General Edit Application Mode.
Hover over the boundary of the shape/void or cavity (ensure boundary visibility is enabled in the color dialog under the Stack-Up > Conductor folder).
Use the RMB to access the Expand/Contract command.

Highlight all GND pins on a particular component

Consider using the Find by Query function to locate elements based on qualifiers.
Invoke "Show Element".
Open the Find Filter and select "Find by Query".
Select the Interconnect tab.
Enable PIN and NET.
In the following example screen, enter U7.* in the PIN field and GND in the net field

Candidate objects are listed, and can be highlighted by right-clicking to access the highlight selected objects command.

Slide: Single-click execution

In Etch Edit Application Mode, make a single pick on a cline segment to slide it.

Moving Components: Single-click execution

Select Placement Application Mode.
Click a component to move it.

Moving Component with Slide Etch option

Use the 'Move' command and enable the option "Slide etch". Works best with low pin count components like resistors.

Changing App Modes with Function Key

funckey a "settoggle CMD 'generaledit' 'placementedit' 'etchedit';$CMD"

Changing Active/Alternate Layers using Function Keys in Etch Edit Mode

Increment or decrement the active or alternate layer:

funckey + subclass -+ (use of + character to increment active subclass) funckey - subclass -- ( use of - character to decrement active subclass) funckey a altsubclass -+ (use of a character to increment alternate subclass)

Directly change the active layer:

funckey 1 options subclass TOP funckey 2 options subclass
SIGNAL_2 funckey 3 options subclass SIGNAL_3 funckey 4 options subclass
SIGNAL_4 funckey 5 options subclass SIGNAL_5 funckey 6 options subclass
SIGNAL_6 funckey 7 options subclass SIGNAL_7 funckey 8 options subclass
BOTTOM

Another method to change the active subclass is from right-click: choose ïƒ Quick Utilities ïƒ Change Active Subclass

Note: If you are not in Etch Edit mode, the class must be set to etch for the function key to operate correctly.

Deleting Elements using Function Key

This function key is used more than any other one. Pass your cursor over a cline, segment, via, text or shape and click d to delete it. No click of the mouse. Works on multiple selected elements as well.

funckey d "prepopup; pop dyn_option_select @:@Delete"

Using the Delete by Rectangle command

Use the Delete by Rectangle command to make a window cut in a group of clines. Access the command from Manufacture ïƒ Drafting ïƒ Delete By Rectangle.

Rotating a Component using Function key

Press the function key R to rotate a component during movement: funckey r iangle 90

Mirroring a Component Using Function key

Press the function key M to mirror a component during movement: funckey m "pop mirror"

Snapping Using Funckey key

The snap pick to pop-up menu contains many options. You may want to consider creating function keys for the ones you use frequently. A few examples:

funckey f "prepopup;pop dyn_option_select 'Snap pick to@:@Figure'" funckey i "prepopup;pop dyn_option_select 'Snap pick to@:@Intersection'"
funckey c "prepopup;pop dyn_option_select 'Snap pick to@:@Arc/Circle Center'"
funckey v "prepopup;pop dyn_option_select 'Snap pick to@:@Via'"

Creating a Snap Pick to Shortcut with Scriptmode +e

Type scriptmode +e in the command window.

The e option is used to echo the PCB Editor command language to the command window.

Perform a snap function and note the command is written to the â€˜command windowâ€™.
Select the command then right-click and choose Copy.
Paste the command after a Funckey key and enclose in double quotes. Example:
- o Funckey c pop dyn_option_select 'Snap pick to@:@Arc/Circle Center'

Mirroring a stationary component (do not move it)

While hovering over a symbol, use the RMB and select the Mirror command.

Aligning Components

Window-select a group of components, hover over the anchor component, and then right-click to access the Align components command.
The key point with hovering is you must be hovering over an object. Do not hover in BLACK SPACE!
Consider the options for equal spacing or compress to DFA spacing.

Snapping a rat T to a pin/via

While moving a Rat T, try setting rotation point to Body Center:

Protecting Alias/Function keys

Is there is a way to prevent users from creating aliases that are named the same as Cadence aliases, or the ones originated from site admins?

To protect (for example, read-only) alias/funckey assignments, use the alias_protect command.

Usage:

alias_protect <alias/funckey>

Example:

funckey m move
alias_protect m

Commands assigned the Alias_Protect option will always win out over similar commands sourced from other locations.

Extracting single-footprint from PCB Database

Use the skill command to write out the package symbol data files for a single symbol.

In the following example, SR0201.dra and SR0201.psm are generated along with the respective padstacks.

Enter the following command in the PCb Editor command window:

skill axlWritePackageFile( car(axlSelectByName("SYMTYPE" "SR0201"))->definition)

Refreshing package symbol instance

Select Placement Edit App Mode.
Hover over package symbol, and then right-click to access the Refresh Symbol Instance command.

Using Mouse Wheel to control interface visibility

Net-Groups are part of the Base OrCAD/SIP product line, and provide the user with graphical and CM Objects that are used to map electrical interfaces to physical objects the layout designer can easily understand. This mapping provides convenient grouping of nets that have similar electric, physical, and spacing route path requirements.

The following two button commands let you use the middle mouse wheel while holding the Shift key to ascend or descend the net-group hierarchy:

button Swheel_up interface_vis up button Swheel_down interface_vis down

Top level View Byte Lane Level

Aliasing commands to the Middle Mouse Wheel

The button command can be used to alias the Middle Mouse Wheel to commands. Works with SHIFT, CONTROL and SHIFT + CONTROL combinations.

Examples:

button Swheel_up subclass -+ button Swheel_down
altsubclass -+ button Cwheel_up "roam y -$roamInc" button Cwheel_down
"roam y $roamInc" button SCwheel_up "roam x -$roamInc" button
SCwheel_down "roam x $roamInc"

In Constraint Manager, the experienced designers can use the <Control> Middle Mouse Wheel to increase the font size.

Trimming and Extending Drafting Lines

Access these commands from Manufacturing ïƒ Drafting Menu (This is available from one of the QIRâ€™s for SPB 16.6).

Sliding vias/clines freely into dynamic shape

This variable when set will let you freely slide vias and clines into dynamic shapes. Without the variable, you will experience jumpy behavior at the boundary. Set the Ignore Dynamic Shapes in Etch Edit variable.

This has been made a default behavior in 16.6. The variable is now in the User Preference editor.

Variations of a Route Keepout Area

There are a suite of properties that permit exceptions for route keepout areas

Allow vias - apply the property vias_allowed to KO shape
Allow Shapes apply the property shapes_allowed to KO shape
Allow Routes apply the property routes_allowed to KO shape

Replacing padstacks by window selection

In General Edit Application Mode, window around the set of pins or vias you wish to change, and then use the RMB ïƒ Symbol Pin or Via ïƒ Replace Padstack ïƒ Selected Instances command.

Changing Net Names on vias (skill code)

A skill application named change_net_on_vias.il is located in your install directory share/pcb/examples/skill/cmds.

If not already done, open your allegro.ilinit file (located in your PCBENV dir).
Add this command and then load change_net_on_vias.il.
Enter change_vianet in the command window to launch the application.

Polygon selection window

If a polygon selection window is desired:

Right-click - Selection Set - Select by Polygon

Z-Copy: A powerful utility

Create a Route Keepin area derived from the board outline. Most of you might know how to do this. There is a handy tip following this short step.

Select Edit Z-COPY, and then adjust the options settings as follows:
- Class = ROUTE KEEPIN
- Subclass = ALL.
- Enable â€˜contractâ€™
- Enter value of 25 in the Offset field
Select the Board Outline to create the Keepin shape.

Tip: Z-Copy can be used to target multiple layers in one operation?

If, for example, you wish to create multiple GND planes, the names of the layers may be called GND_1, GND_3, GND_5, GND_8, and so on.
Select Edit -Z-Copy.
Adjust the options form so that Class = Etch.
Select one of the GND layers.
Edit/backspace the numerical part of the layer, and then enter the wildcard â€˜*â€™ character as shown in the following figure.
Set Offset value to 0.
Select the Route Keepin to create the 2 GND planes.

Enabling offset routing (fabric weave)

For routing that requires offset angles (11.3 typical), while in the Add Connect command, click the W key to enable the Route Offset option.

funckey w "pop flip"

Fixing/Unfixing elements in the design

Tips to add and remove the Fixed Property.

The quickest method to remove the fixed property from all the elements in the Design is to:

Click the Unfix Icon.
Right-click and choose Unfix All.

Figure 5
Mouse over the symbol, and then select the Fix command from the context sensitive RMB menu.

Figure 6

Datatip Display of the Fixed Property

By hovering over it, you can know whether an element is fixed.

Figure 7

Configure the datatip setting as shown in the following figure. You might also want to enable other symbol-related properties to display in the datatip window. This is done from the Setup ïƒ Datatip Customization menu. Select Symbol Instance under Object Type, and then enable the value FIXED.

Datatip Options

Figure 8

Controls for delay, location and disablement

The User Preference Editor contains hundreds of variables. The Search box is a very handy mechanism. In this example, when you type in the word datatip and click Search, variables to delay, locate and disable datatips are available to you.

Figure 9

The complete set of variables related to Datatips is located in the Display ïƒ Datatips Category.

Figure 10

Status Form Traffic Lights

You can click on the indicators to obtain a report?

Figure 11

"Go to" X,Y Location

Navigate to an X,Y location in the Design

You wish to quickly go to a specific X, Y location in the Design. For example, you want go to the location x = 5000, y = 7000.

Adjust your zoom level, and then click on the P button located at the base of the canvas display. Enter in your coordinates then click Pick.

Note: Set application mode as none for this behavior.

Figure 12

Disabling Custom Color Assignments

You may inherit a board from another designer or shop and question some of the color assignments. One quick method to disable color overrides that might have been applied to nets, buses, Diff Pairs is to go into the color form. If you select the Nets radio button on top, you will see a new button called Disable Custom Colors. Select this option to revert to layer-based coloring.

Figure 13

Color Dialog: Open the last used folder

Set the color_lastgroup variable located in Setup ïƒ User Preferences ïƒ UI ïƒ

Control_panel.

Displaying a layer

Figure 14

Click the color swatch box to the left of the subclass to quickly turn layers on/off during a command.

Figure 15

Invoking OrCAD PCB Editor in No OpenGL mode

It might be necessary to run PCB Editor in No OpenGL mode. For example, hosting a Net Meeting. Consider creating a Desktop Shortcut for Allegro.exe with the noopengl option.

Figure 16

Displaying properties in the canvas

Any property attached to an element can be displayed in the canvas. From the Display

ïƒ Property menu, select the Graphics tab, and then select properties to display from the left column. Clicking the Create button writes out the property values and/or the respective name to the subclass properties.

Figure 17

Figure 18

Suppressing pin-to-pin violations within the same symbol

PCB Designers often use Constraint Regions to suppress pin-to-pin violations within the same symbol. The nodrc_same_sym_pin property can be applied to the symbol. However, did you know it can also be applied to the drawing? Applying it at the drawing level has a global impact to all symbols.

Go to Edit - Property and then select drawing in the Find by Name field.

Figure 19
Select Drawing Select. I has now moved to the selected objects column.

Figure 20
Click Apply and then pick nodrc_same_sym_pin from the list.

Figure 21

Creating a Command Shortcut with Scriptmode +e

Adding a drawing level property in the previous tip was labor intensive. Now you can create a shortcut.

Enter scriptmode +e in the command window. This echoes the commands you enter.

Figure 22
Copy all the commands above to a single line.
Separate with semicolons.
Map to a function key When using multiple commands in a function key or alias, put these in double quotes.
funckey e "property edit;setwindow form.find;FORM find name_type Drawing;FORM find find_by_name;FORM findname objlist 'Drawing Select';FORM findname done"
Click the e key, and then press ENTER in the command window to launch the property editor dialog.

Figure 23

"scriptmode +i" is a shorthand for "scriptmode +invisible".

Suppose you want to create an alias to toggle end cap display but do not want to see the parameter form appear while executing the script, use:

alias ec "scriptmode +i; prmed; FORM prmedit display_enhance toggle; FORM prmedit done"

DFA Dynamics: Controlling spacing bubble resistance

When placing components to DFA rules, it is difficult to pull back the component when the bubble appears.

The resistance can be controlled by the dfa_pause_level variable located in User Preferences ïƒ DFA_DRC. Set it to 0 for no resistance.

"Locked" Property

The Locked property was designed for Re-Use modules. However,:

The property can be applied to a place replicate circuit to prevent accidental movement of its members.
It can also be applied to a package symbol to prevent editing or deletion of the assembly outline or other data elements.

Suggestion: Consider applying the locked property to the symbol definition (at the library level).

Locating a dynamic shape

A dynamic shape is "out of date" BUT has a "No Etch" status.

You cannot find the shape in question. It says it is at a particular XY location, on a particular layer, but there is nothing there. Turn on the Boundary color item for that layer to locate the shape outline.

Figure 24

Voiding of GND Clines through GND Plane

Here is the method to auto-void GND sense lines being routed through a GND plane. In the following example, a GND net is routed through a GND shape. The 'void_same_net' property was applied to the cline.

Figure 25

How to convert non-Acute angles for shapes to round corners?

This feature is available in 16.3. Go to the dynamic shapes parameter and set the Acute angle control to "Full Round". Static shapes get the same capability in a future ISR with the eap_static_newsmooth env variable.

HTML Reports

Reports and messages can be displayed in HTLM format when the

allegro_htmlvariable is set. One advantage of using HTML is the ability to search through the report.

Figure 26

Figure 27

Printing a form using Control+P keys

Did you know Control+P can be used to print a form?

For example, inside the DFA Symbol classification window, press Cntrl+P to open up the Print form window, and then click the "To File" button to save the information to a text file.

Figure 28 - Control P the click to file

Figure 29 Example of file

Adding Text (from a file)

To add text from a .txt file on disk:

Run the add text command: Add ïƒ Text.
Set the desired text options on the Control Panel Options tab.
Set the Active class to Board Geometry.
Set the Subclass to Dimension (or any other subclass).
Set Marker Size:
Set Rotation:
Set Text Block:
Set Text Justification:
Position the cursor/LMB at the location that you want the first line of text to start.
Right-click and choose: Read from File.

Method to renumber all Ref Des from start

Use the fst_ref_des variable. You must ensure that the refdes digits in the Sequential Renaming section of the UI allow for the number of digits in the fst_ref_des variable. The variable is located in User Preference ïƒ Manufacturing ïƒ Silkscreen.

Why does the system react slowly when moving a comp?

Most likely because your large pin-count nets are scheduled Min Tree. Add a voltage property or RATSNEST_SCHEDULE = POWER_AND_GROUND to large pin-count nets like Vcc and GND.

Why does DRC update take hours to run?

Usually, the slower checking is a result of a large number of constraint areas and/or a large number of overlapping constraint areas. If that is not the case, then it might be the larger spacing values that you have to satisfy you high voltage requirements or simply fudge values entered as no-ops. Large-spacing values result in more neighboring items being examined for each item being checked.

Note: Review your extra-large spacing values. There could be a value of 999 entered. When reduced, DRC update can go down from 1 hour to 3 minutes.

Is my database optimized for performance?

Performance Advisor provides suggestions to increase database performance. The command can be run from Tools ïƒ Database Check ïƒ Performance Advisor.

Figure 30

Read-only variables

A method for a site administrator to make variables read-only.

Add a
readonly entry under the respective variable. In the following example, you wish to prevent the end user from modifying PSMPATH. The readonly psmpath command is added just below the "set psmpath" variable.

Figure 31

To verify in PCB Editor, type readonly at the command line prompt. The window lists variables that are read-only.

Figure 32

When an attempt is made to change psmpath in the User Preferences Editor, the following warning will appear:

Figure 33

BBVIA GAP DRC reporting too many DRCs

Under normal circumstances, the Buried/Blind vias separated by less than the minimum BBVIA gap rule will generate a DRC, no matter how many layers separate them. A drawing level property, BBVIA_SEPARATION, suppresses the DRC if the vias are separated by the specified layer span value or more. In the following example, the property value of 2 suppresses the DRC on the left side.

Figure 34

Same Net DRCs not being generated

It is most likely because your DRC by-layer setting is set to False.

Figure 35

Working with Xnets

Create Xnets Assign Espice models to the discrete devices from the Analyze ïƒ SI/EMI Sim

ïƒ Model Assignment menu.

Prevent Xnets on an Instance basis - Assign the no_xnet_connection property at the component level.

Display Xnets In CM, go to Object ïƒ Filter and enable net to see the nets of the Xnet.

Figure 36

Naming Convention The Xnet name defaults to the net name with the lowest alphanumeric character. In the example, L is before S.

Change the Xnet Name

In CM, select the Xnet, and then right-click and choose ïƒ Rename

Figure 37

Gathering Diff Pair

Looking for tighter coupling at the gathering location?

Decrease the value of the padentry_factor variable located in ETCH category of the User Preferences Editor.

Figure 38

Figure 39 Default

Figure 40 - Padentry set to 10

Routing a Tandem Diff pair

Pre-route each member as shown in the following figure, and then use Add Connect to route as a tandem pair. This assumes a Diff Pair constraint object has been created.

Figure 41

Displaying length meter for non-constrained nets

Set the allegro_etch_length variable located in User Preference ïƒ Route ïƒ Connect category.

Figure 42

Constraint Manager

You wish to display propagation delay analysis for unrouted nets in CM. Enable the unrouted modes in Analyze ïƒ Analysis Modes ïƒ Options tab.

Figure 43

Double-click Margin Column Header, or right-click and choose ïƒ Sort.

Figure 44

Displaying only the failed results

Click Object Header, right-click, choose Filter, and enable failed only, or simply click on the following icon:

Displaying only the nets that have constraints

Click Object Header, right-click, choose Filter, and enable constrained only, or simply click on the following icon:

Segregating sections of CM with divider lines

It, means identifying the transition between buses and matched groups.

In CM, go to View ïƒ Options ïƒ Workbooks ïƒ Enable Object Type Dividers, or simply click on the following icon:

Figure 45

You wish to change a constraint, for example, min line width across a certain layer of all the available PCSets.

Consider working in the By Layer worksheet to change the Top layer constraint across all the available Csets.

Figure 46

TOC

Export to Excel

Constraint Manager can export to a native excel spreadsheet (Windows Only & you must have Excel installed).

In CM, go to Tools ïƒ Excel ïƒ Active Worksheet/Workbook.

TOC

Constraint resolution

You want to see how the constraint resolves between 2 objects?

Use Display ïƒ Constraint, and then window select the 2 elements to obtain spacing resolution. Next, select single element for physical resolution.

In the following example, you window selected the two clines of a Diff Pair to obtain spacing resolution. The actual measured gap is supplied in the middle section of the report.

Figure 47

TOC

Assigning pins of dummy nets to net classes

In 16.3 (June 2010 ISR), enter the cns_dummy_net command or type helpcmd to get the complete PCB Editor command set.

Figure 48

Figure 49

TOC

Preventing Shorts

In PCB Editor, It is possible to override a DRC with properties.
1. Make sure that the nets involved do not have the NO_DRC property on a pin(s).
2. Make sure there are no invalid waived DRCs.
3. Make sure your DRC modes are enabled. Be especially careful with newly-released DRCs (for example, Microvia-based) as those are disabled by default.
4. Run DBDoctor to keep the design in sync and up to date.
5. Make sure the plane layers in the cross section form agree with the artwork control form (negative or positive).
6. Make sure the padstacks are designed properly; both Antipads and thermals.
7. Include the IPC-D-356 netlist in your Fab Package. Ensure that the Fabricator does a netlist to Gerber compare.

Suppressing SIGNOISE warnings and error messages

To suppress Signoise warning and error messages from appearing in the message window, set the â€˜set sigsuppress ERROR WARNINGâ€™ variable.

Write vs. Save

You want to save the current board file you are working on as a new name. However, you want to keep the current file open using its current name. The Save As function will make the saved file the active file.

Enter WRITE in the command window followed by a design name.

Autosave the Database

Key variables to auto save the database.

Figure 51

Reopen command

Most people do not know about this convenient command, which does what is says. It reopens a design file.

Enter reopen in the command window to reopen the same file.

Figure 52

File Management (Artwork, Plots, Log Files, Reports)

Looking to manage your artwork, plots and reports more efficiently? There is a suite of variables beginning with ADS, designed to create subdirectories for the common data files.

Figure 53

What is the earliest version of OrCAD PCB Editor that can open my database?

The command Dbstat will report the PCB Editor database revision and platform type.
Dbstat supports the following file types (extensions):
.brd .mdd .cio .sip .mdd .dpf .scf .pad .dra .mcm .psm .ssm .fsm, .bsm
Type Shell in the PCB Editor command window to bring up a DOS window
Type dbstate <file name> Example:

Open File Manager from PCB Editor

Quick method to explore to your working directory: Tools ïƒ Utilities ïƒ File Manager

Looking for a particular pad stack based on holesize?

There are two methods to obtain a report of library padstacks:

Manufacturing ïƒ NC ïƒ Drill Customization ïƒ Library Drill Report
PadDesigner ïƒ Reports ïƒ Library Drill Report

Sort by column type by placing cursor in one of the cells, and then right-clicking and choosing Sort by.

Figure 54

Testability: Multiple Probe-Type Support

The Testprep parameter form supports entries for multiple probe-types. Typically, the names are 100, 75 and 50 MIL. The names and center-to-center spacing is can be user-defined. To add a row in the form, select a Probe Type cell and RMB ïƒ Add

Figure 55

Drill Legend Support for INCHES and METRIC

Update your default .dlt file as shown here:

?AlternateUnits "millimeters"

?ColumnDefinitions '(

("Figure" "FIGURE" 7)

("Tolerance"	"Tolerance"	15)
("Holesize2"	"SIZE MM"	15)

("Holesize" "SIZE" 15)

("Tolerance2" "TOLERANCE MM" 15)

("PlateStatus" "PLATED" 10)

("NonStandard" "NONSTANDARD" 15)

("Quantity" "QTY" 6)

)

Uprev Symbols

The uprev_overwrite command can be used to uprev library files to the current software revision.

Syntax: uprev_overwrite n where n = *.dra; *.psm; *.ssm Example:

In a command window, enter uprev_overwrite *.dra to update all the .dra files to

the current software level.

For more flexibility in upreving, in a DOS command window, type:

uprev -help

Note: Be sure to make a backup copy of your library before uprev.

Figure 56

Troubleshooting: Running PCB Editor in Safe Mode

Many PCB Editor programs support the -safe command line option. This starts the program without any user customizations or extensions. This can be used as a debug mechanism to eliminate user configurations as the cause of the problem with the product.

It disables loading at startup:

local env file
(<HOME>/pcbenv/env) cds_site configuration data

any user skill code pre-register scripts

ini file which stores window
size/position information most recent used files (MRU)

remembered Windows positions (.geo files)

UNIX: Currently it cannot disable X window resource settings.

In addition, graphic programs support the -noopengl option, which will disable the enhanced Graphics based upon OpenGL.

Example: Run an "out of the box" PCB Editor without opengl: allegro -safe -noopengl

Tips from OrCAD PCB Users

Join the Cadence Community Website and see what other users are saying.

http://www.cadence.com/community/forums/27.aspx?CMP=home

Figure 57

Windows 7: Graphic Issues

Try disabling Aero (desktop composition) for PCB Editor only:

Navigate to the executable or shortcut for the program you wish to disable desktop composition using Explorer.
Right-click on it, and select Properties.
Select the Compatibility tab and check Disable desktop composition, and then click on OK.
As always, ensure your graphic driver is up-to-date.

Search form

You are here

OrCAD PCB Editor – Tips and Tricks

Reducing mouse clicks and travel

Center display at cursor location

Adding Vias: Use of Space Bar