Flex Board Checks

Introduction

The Flex Board Checks Analysis Action is a read-only action indented to find violations of flex design rules, and to locate potential manufacturing defects unique to Flex Boards.

The action contains a set of checks that analyze the interaction of Flex Board layers with specific areas in the flex board such as stiffener locations, air gaps, bend area, and silver shielding (EMI).

The action requires the GenFlex license flexanl .

Definitions

Silver Mask Layer (EMI)

The silver shield or EMI is a conductive coating which is added to the Flex PCB in specified areas as defined by the silver mask layer.

The analysis for Silver mask layer requires that one of the following conditions be met:

  • Areas where the silver mask should be applied are defined by closed outlines. These areas of the silver mask should be defined as layer type conductive_mask and context=board .

An empty layer defined as layer type conductive_mask and context=board , and a punch or rout layer ( context = board ) which has it's span defined on this silver mask layer.

Adhesive Layer

Adhesive is the material that is applied in between signal layers to glue multilayer boards together. Usually the designer will provide an outline where adhesive should be applied and where not. The locations within the board profile where no adhesive is applied are referred to as "air gaps". The main purpose of air gaps is to achieve better bendability of the multilayer flex in specific locations. If multilayers are bonded over the complete surface then the PCB may become too rigid. So, in places where more flexibility is required, there is usually no bonding, and the adhesive material is removed in those locations. The adhesive is usually removed by punching or routing the adhesive material in those places where the air gaps are located.

 

 
Adhesive layer - red areas are locations where adhesive material needs to be applied

 

 
Corresponding adhesive punch: defines the locations that need to be punched out of the adhesive material

The analysis for adhesive/air gaps requires that one of the following conditions be met:

  • Areas where adhesive should be applied are defined by closed outlines. The adhesive layer should be defined as layer type psa and context=board .
  • An empty layer defined as layer type psa and context=board , and a punch or rout layer ( context=board ) which has it's span defined on this adhesive layer.

Bend Area Layer

Bend area defines parts of the board that will be (pre-) bent in order to fit the board in a specific assembly. The bend area should be defined as an outline or surface on a layer with type bend_area and context=board.

 


Stiffener Layer

Stiffener defines an area on the board that should be rigidized, either with FR4 or with adhesive stiffener material (e.g. 3M stiffeners). In the case of FR4, usually a separate stiffener step is created which will be panelized in a different panel. In such cases, the stiffener area will be defined as an area layer.

In other cases, the stiffener might be punched or routed in places where no stiffener is required. In these situations, a "negative" image will be created which defines the locations where no stiffener should be applied.

 

 
Stiffener area defined by 2 area layers (green and blue)

Stiffener analysis requires a layer of type stiffener that defines the boundary of the stiffener by a closed outline or surface.

 

Action Checks

Bend Area

Signal Layer vs. Bend Area Layer

Line width changes in Bend area are not allowed.
Line width change will be reported in the See Changed Width (Bend Area)category.

 

 

Line Changes direction in Bend Area are not allowed.
Line direction change will be reported in See Changed Direction (Bend Area) category.

Lines not perpendicular to bend area are not allowed.
Non-perpendicular line will be reported in See Not Perpendicular (Bend Area) category.

Coverlay Layer vs. Bend Area Layer
  • Coverlay Clearances in or close to Bend Area are not allowed.

Coverlay clearance inside or close to a Bend Area will be reported in the See CVL Clearance in Bend Area (Bend Area) and See CVL Clearance Close Bend Area (Bend Area) categories.

Stiffener Layer vs. Bend Area Layer
  • Stiffener cannot overlap bend area or come too close to it.

Stiffener feature that is inside or close to a Bend Area will be reported in the See Stiffener in Bend Area (Bend Area)or See Stiffener Close Bend Area (Bend Area) categories.

Drill Layer vs. Bend Area Layer
  • Plated/via drills are not allowed in or close to Bend Area.

Plated/via drill that is inside or close to a Bend Area will be reported in the See PTH/Via in Bend Area (Bend Area)or See PTH/Via Close Bend Area (Bend Area)categories.

Air Gap

  • If there is an NC/ROUT/PUNCH layer which pierces only the psa layer, this (accessory) layer will be used for the analysis. Otherwise, the action will use the psa layer for the analysis.
Drill Layer vs. PSA Layer
  • Plated/via holes are not allowed inside or close to air gaps.

Plated/via drill that is inside or close to air gap will be reported in the
See PTH/Via in Air Gap Area (Air Gap)or See PTH/Via Close Air Gap Area (Air Gap) categories.

Coverlay Layer vs. PSA Layer
  • No Coverlay openings are allowed inside or close to air gaps.

Coverlay opening that is inside or close to air gap will be reported in the See CVL Clearance in Air Gap Area (Air Gap) or See CVL Clearance Close Air Gap Area (Air Gap)categories.

Stiffener Layer vs. PSA Layer
  • No stiffener allowed inside or close to air gaps.

Stiffener that is inside or close to an air gap will be reported in the See Stiffener in Air Gap Area (Air Gap)or See Stiffener Close Air Gap Area (Air Gap) categories.

Stiffener

Coverlay Layer vs. Stiffener Layer
  • Coverlay clearances should be either completely inside the stiffener or outside of it.

Coverlay clearance that is too close to edge or overlapping the edge of the stiffener will be reported in the See CVL Clearance Close Stiffener (Stiffener)category.

Drill Layer vs. Stiffener Layer
  • Plated/Via holes should be either completely inside the stiffener or outside of it.

Plated/Via hole close to edge or overlapping the edge of the stiffener will be reported in the See PTH/Via Close to Stiffener (Stiffener)category.

Spatial Overlap

  • Traces on two adjacent layers should not overlap.

Lines that overlap will be reported in the See Line Overlap (Spatial Overlap)category.

  • The Spatial Overlap check will ignore lines with the following attributes: . cross_hatch, .pattern_fill , and .nomenclature .

 

 
Zoom to 200% to see detail

SM/Coverlay

  • Solder mask/Coverlay clearance should keep a minimum distance away from the board edge.

A clearance that is too close to the board edge (profile) will be reported in the See SM/CVL Clearance Close to Profile (Coverlay)category.

Joints

  • Sharp corners between lines provide a potential risk for breaking.

Any connection between lines that is less than a defined angle will be reported in the See Acute Angle (Joints)category.

  • The Joints check only analyzes connection between two line features.

Silver Mask

  • If there is an NC/ROUT/PUNCH layer which pierces only the Silver Mask layer, this (accessory) layer will be used for the analysis. Otherwise, the action will use the Silver Mask layer for the analysis.
  • Silver mask feature should keep a minimum distance from the board edge (profile). In cases where silver mask extends beyond the board edge, the user can specify a negative value.

If the minimum distance is not kept, the distance will be reported in the See Silver Close Profile (Silver Mask)category.

Copper Layer vs. Silver Mask Layer
  • Distance from Silver Mask to exposed copper. Exposed copper is defined as copper that is not covered by either Solder Mask or Coverlay. If both Solder Mask and Coverlay exist in the job for a specific layer, both are taken into account.

In case Silver Mask is too close to exposed copper, the distance will be reported in the See Silver Close Exposed Copper (Silver Mask)category.

  • Exposed Pad that is covered by Silver Mask area. Exposed Pad is defined as a Pad that is covered by either Solder Mask or Coverlay clearance. If both Solder Mask or Coverlay clearance exist in the job for a specific layer, both are taken into account.

In case Silver Mask fully or partially covers an exposed Pad, the exposed Pad is reported in the See Silver Touch Exposed Pad (Silver Mask)category.

Drill Layer vs. Silver Mask Layer
  • Plated/via holes are not allowed too close to the Silver Mask area.

Plated/via drill that is too close to the Silver Mask area will be reported in the See Silver Close PTH/Via (Silver Mask)category.

  • NPTH holes are not allowed too close to the Silver Mask area.

NPTH drill that is too close to the Silver Mask area will be reported in the See Silver Close NPTH (Silver Mask)category.

Notes:

If there is an NC/ROUT/PUNCH layer (context =board) which pierces only the Silver Mask or psa layer, this (accessory) layer will be used for the analysis. Otherwise, the action will use the psa/Silver Mask layer for the analysis.

Example

In the job matrix example seen here, the Air Gap analysis will use the airgap_pch layer, not the psa layer.


  • The Joints checks only analyze the joints of lines, and does not support joint to surface and other features.
  • EMI to Exposed Copper and EMI to SM check the same side (top or bottom) layer. For example: the top side EMI layer will be checked versus the top side SM and Signal layers.