Backup Project :
Use Project > Project Packager to Create a Backup First !
Or Commit the if you are using Version Control.
Schematic:
Run a Tools > Update From Libraries (for the whole design)
Project > Validate > Update PCB
Project > Validate > Update PCB
Review the ECO list, it will list all changes
Review BOM for Fitted / Not Fitted Parts and Variant Part Numbers.
Review the ECO list, it will list all changes
Review BOM for Fitted / Not Fitted Parts and Variant Part Numbers.
PCB:
Review all required electrical and mechanical design constraints.
Review return paths, look for signal traces crossing moats in GND pours.
Review all project outputs for Fabrication and Assembly.
Review Solder mask, Solder Paste and Silkscreen. Fix as needed.
Check Board Stackup for Proper Internal Layer Naming.
Check Board Fiducials, Markings PCB and PCA numbers.
Check Position of the Database Origin.
Check Fab Dwg - Notes, Dimensions, Drill Table, Stackup and Impedance Table.
Check Assembly Dwg - Notes and Dimensions.
Check for Antennae Nets (Vias and Tracks).
Check for Via Stubs if Applicable
Check for Return Path Vias (use DRC Checks)
Check for Components and Pads on Mechanical Layers.
Check for No-Net Copper (Vias, Track, Arc, Fills, Regions, etc. . .
Execute Selection Filters and Check the Properties Panel for Selected Objects.
Note: All Fixes Should be Pushed to the Footprint Library.
Select Pads with No Paste Enabled
Pads - Select Pads with NO Solder Paste
(ObjectKind = 'Pad') And (PasteMaskEnabled <> 'True') And IsSMTPinThe selected PADs may Include Thermal Paddles with Windowed Paste.
The selected PADs may Include Fiducials, Fiducials should not have Paste.
Suggested solution for Windowed Paste and Fiducials is Paste Enabled with -100% Expansion.
Nothing should be selected after executing the PCB Filters shown below !
Tip: Zoom Out (Short Cut Keys VF) before executing each Filter.
Components - Select Components that are Not on Top and Bottom Layers
(ObjectKind = 'Component') and not OnOutside
Polarity Text Dots - Select Text Strings with Zero Height
(ObjectKind = 'Text') And (AsMM(TextHeight) < 0.01)
NPTH - Select NPTH Pads with Plated Enabled to Find Mistakes
((HoleDiameter >= PadXSize_AllLayers ) OR (HoleDiameter >= PadYSize_AllLayers)) And (PadIsPlated = 'True')
Pads - Select Thru-Hole Pads that have Paste In Pin for Review
(ObjectKind = 'Pad') and IsThruPin And (PasteMaskEnabled <> 'False') Pads - Select Pads with Excess Solder Paste for Review
IsSMTPin And (PasteMaskExpansionMode = 'Manual') And (AsMM(PasteMaskExpansion) > 0)
Tracks - Select Tracks with Exposed Copper for Review
(ObjectKind = 'Track') And (SolderMaskExpansionMode = 'Manual') And (AsMils(PasteMaskExpansion) = 0) and OnOutside
VIAs - Select Pads that are Not using Rule Based Soldermask Expansion
(ObjectKind = 'Via') And (SolderMaskExpansionMode <> 'From Rule')
(ObjectKind = 'Via') And (IPC4761ViaType <> 'None')
Find Stacked uVias
IsStackedVia
Regions - Select Free Regions with Exposed Copper for Review
(ObjectKind = 'Region') And (SolderMaskExpansionMode <> 'None') and OnOutside and Not InComponent('*') And (IsCutoutRegion = 'False')
Regions - Select Regions with 0 size Area. These should be deleted.
(ObjectKind = 'Region') AND (Area='0 sq.inch')
Review selected Pad after executing the PCB Filters shown below !
Pads - Select Pads that are Not using Rule Based Soldermask Expansion
(ObjectKind = 'Pad') And (SolderMaskExpansionMode <> 'From Rule')
Paste in Pin (PIP) - ThuHole Pads with Solder Paste
IsThruPin And (PasteMaskEnabled = 'True')
Properties Panel > Select Pad Stack > Simple > Solder Paste > Enabled
or
IsThruPin And (PasteMaskEnabled = 'False')
Properties Panel > Select Pad Stack > Simple > Solder Paste > Not Enabled
Note: Thermal Pads and region may need to use Manual Expansion.
To Fix a Pads in a PCBDoc Select Components > Unlock Primitives
After executing a Filter use Find Similar and Properties Panel to make changes.
Solder Paste and Solder Mask - Examples for Pads:
Properties Panel > Select Pad Stack > Simple > Solder Paste > Enabled and Manual
Properties Panel > Select Pad Stack > Simple > Solder Mask> Rule Expansion
Paste Mask and Solder Mask for Free Regions and Fills in PCBDoc:
Properties Panel > Select Pad Stack > Simple > Paste Shape > NOT Enabled
To Find Fills and Regions on Paste Layers (i.e. Thermal Paddles)
((ObjectKind = 'Region') And (Layer = 'TopPaste')) or ((ObjectKind = 'Fill') And (Layer = 'TopPaste')) or ((ObjectKind = 'Region') And (Layer = 'BottomPaste')) or ((ObjectKind = 'Fill') And (Layer = 'BottomPaste'))
Rememeber ! Select Components > Lock Primitives when done.
Useful Components and Designators Filters
Components - Select All Components Except Caps and Resistors
(ObjectKind = 'Component') And (Not(Name Like 'C*')) And (Not(Name Like 'R*'))
Components - Select All Components Except Caps, Resistors and Inductors
(ObjectKind = 'Component') And Not(Name Like 'C*') And Not(Name Like 'R*') And Not(Name Like 'L*')
Components - Select All Except Caps, Inductors, Resistors & Fiducials
(ObjectKind = 'Component') And Not(Name Like 'C*') And Not(Name Like 'R*') And Not(Name Like 'L*') And Not(Name Like 'FD*') And Not(Name Like 'FID*')
Components - Select Parts with Designators Like R* or C*
(ObjectKind = 'Component') And (Not(Name Like 'C*')) And (Not(Name Like 'R*'))
Designators - Select Designators with Silkscreen Violations
(ObjectKind = 'Text') And (StringType = 'Designator') And (Layer = 'TopOverlay') and HasViolations
Stackup Folder - readme.txt file
Do not delete this file.
Refer to the Stackup in the Fab notes
If available a copy of an approved fabricator stackup may be placed in this folder.
That's it !
