My flexible PCB design requires a stiffener. Since the stiffener is a separate component from the flex circuit itself, I’m unsure about the best way to define it in my PCB design files. Should I use a dedicated mechanical layer to outline the stiffener placement, or would it be more appropriate to define it as part of the coverlay layers? What’s the recommended industry practice for documenting stiffeners in flex PCB designs?
1 Like
Don’t include stiffeners in the layer stack. Instead, define the stiffener outline on a mechanical layer, with a clear callout in the documentation (and sometimes a matching 3D model if needed). This aligns with how stiffeners are typically manufactured, since they’re applied as a post-fabrication step by the fabricator.
1 Like
I usually define stiffeners on a non-copper layer that isn’t used for anything else, and then add a clear fabrication note pointing out that it’s for the stiffener.
1 Like
In my flexible PCB designs, I define the stiffener outline on a mechanical layer and document its purpose in the fabrication drawings. I also generate a STEP model or extrusion to capture the stiffener thickness so it shows up in 3D exports, which helps our mechanical team visualize the final assembly. This approach has worked well when coordinating with a PCB assembly house.
1 Like
In my flexible PCB projects, I make sure the stiffener details are crystal clear in the files I send to manufacturing. Along with the Gerbers, I add:
- A 3D PDF showing what the finished board should look like.
- Mechanical PCB layers for adhesives and stiffeners.
- A fab drawing that embeds the manufacturer’s stackup (since flex stackups often need adhesive/stiffener layers shown explicitly).
I also label the Gerber PCB layers in the fab notes (e.g., “.GM4 = Bottom Flex Stiffener”) and add callouts such as “Polyimide stiffener, 0.2 mm thick, bonded with epoxy adhesive.” This helps the printed circuit board company to apply the right material at the right location.
2 Likes
When documenting stiffeners in a flexible PCB, I like to separate each type of information onto its own PCB layer. For example, I’ll keep the outline, stiffener details, assembly notes, and rigid-flex regions on different layers, and even dedicate one PCB layer just for the routing tool path. This makes it obvious to the fabricator what each element represents and prevents overlap or confusion.
To add clarity, I also generate 3D details and an isometric printout that shows the final intent. Sharing that along with the Gerbers has worked well in practice, since it gives the design house a complete picture of how the stiffeners and flex regions should be built.
1 Like