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 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:
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 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.
The analysis for adhesive/air gaps requires that one of the following conditions be met:
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 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 analysis requires a layer of type stiffener that defines the boundary of the stiffener by a closed outline or surface.
Line width changes in Bend area are not allowed. |
|
Line Changes direction in Bend Area are not allowed. |
|
Lines not perpendicular 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 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.
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.
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 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 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.
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.
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.
Lines that overlap will be reported in the See Line Overlap (Spatial Overlap)category.
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.
Any connection between lines that is less than a defined angle will be reported in the See Acute Angle (Joints)category.
If the minimum distance is not kept, the distance will be reported in the See Silver Close Profile (Silver Mask)category.
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.
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.
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 drill that is too close to the Silver Mask area will be reported in the See Silver Close NPTH (Silver Mask)category.
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.