Altium Designer Documentation

リジッドフレキシブル デザインの 3D 表示

Modified by Phil Loughhead on Jan 6, 2021

Rigid-Flex is under active development. New Board Region and Bending Line features are available, and new Layer Stack Manager features are under development and will be released soon.

Use of the new rigid-flex features requires the following change in the Advanced Settings:

  • Disable the Legacy.PCB.RigidFlex option to access the new Region definition and Bending Line features.

What is Rigid-Flex?

As the name suggests, a flexible printed circuit is a pattern of conductors printed onto a flexible insulating film. Rigid-flex is the name given to a printed circuit that is a combination of both flexible circuit(s) and rigid circuit(s), as shown in the image.

Flexible circuit technology was initially developed for the space program to save space and weight. It is popular today as it not only saves space and weight - making it ideal for portable devices such as mobile phones and tablets - it can also reduce packaging complexity, improve product reliability, and reduce cost.

Flexible circuits are normally divided into two usage classes: static flexible circuits, and dynamic flexible circuits. Static flexible circuits (also referred to as use A), are those that undergo minimal flexing during assembly and service. Dynamic flexible circuits (also referred to as use B), are those that are designed for frequent flexing, such as a disk drive head, a printer head, or as part of the hinge in a laptop screen. This distinction is important as it affects both the material selection and the construction methodology. There are a number of layer stackup configurations that can be fabricated as rigid-flex, each with their own electrical, physical and cost advantages.

Mechanical Rigid-Flex Design

Designing a flex or rigid-flex circuit is very much an electromechanical process. Designing any PCB is a three-dimensional design process, but for a flex or rigid-flex design, the three-dimensional requirements are much more important. Why? Because the rigid-flex board may attach to multiple surfaces within the product enclosure, with the attaching and folding process happening as the product is assembled.

The traditional approach to confirm that the folded board fits within its enclosure has been to create a mechanical mockup (known as a paper doll cut out). By its very nature, it's difficult to achieve the accuracy and realism required with this approach. Altium is helping to solve this challenge with CoDesigner, a sophisticated mechanical - to - electronic design interface technology. CoDesigner allows the engineers to pass the board shape and component changes back and forth between the ECAD and MCAD design domains.

Overview of Altium's MCAD CoDesigner technology

Technical reference, learn More about ECAD-MCAD CoDesign

Learn more about transferring a rigid-flex design to SOLIDWORKS

  • Altium Designer also supports including rigid-flex boards as part of a multi-board design. Learn more about Designing Systems with Multiple Boards.
  • For an engaging discussion on the materials, technologies, and processes, as well as the challenges involved with the production of a rigid-flex board, download and read the free Rigid-Flex Guidebook.

Designing a Rigid-Flex PCB

Use of the new rigid-flex features requires the following change in the Advanced Settings:

  • Disable the Legacy.PCB.RigidFlex option to access the new Region definition and Bending Line features.

A printed circuit board is designed as a series of layers stacked on top of one another. For a traditional rigid printed circuit board, the board shape defines the board in the X-Y plane, and the stack of layers defines the board in the Z plane. The X-Y board shape is defined in the main PCB editing window, and the layers are configured in the Layer Stack Manager.

In a rigid-flex PCB, there is more than one zone or Region in the finished printed circuit board, and each Region can use a different set of layers. To prepare a rigid-flex board, you need to:

  • Enable the Rigid-Flex mode (Layer Stack Manager, Tools » Features » Rigid-Flex command)
  • Define the Substack needed for each Region of the board, and configure how those Substacks align with each other in the Z plane.
  • Define the shape of each Region, connect the Regions to each other in the X-Y plane, and assign the correct Substack to each Region.

These tasks can be done in any order, if the Regions are defined before the Substacks then you'll need to assign the correct Substack to each Region once the Substacks have been defined.

Enabling Rigid-Flex

To support the complex structures present in a modern rigid-flex printed circuit board, the Z plane editor - the Layer Stack Manager, provides different display modes for editing the structure of your board. Select the Design » Layer Stack Manager command to open the Layer Stack Manager, where you can create and align the Substacks needed in your rigid-flex design.

When the Layer Stack Manager opens, it will show the Stackup of the board. For a new PCB, this will be a simple two-layer board. To enable the features needed to design a rigid-flex board, select Rigid-Flex from the Tools » Features sub-menu.

Enable the Rigid-Flex mode to configure a Rigid-Flex board.
When you do, the display will change from Stackup mode (shown above) to Board mode (shown below). Use the Navigation bar at the upper right of the Layer Stack Manager to move back and forth between the Stackup and Board modes, as highlighted in the image below.

Board mode is currently in closed Beta, Open Beta builds will present the multiple layer stack selector used in previous versions.

The Board mode of the Layer Stack Manager is used to align the substacks in a rigid-flex design. (closed Beta builds only)

The Board mode of the Layer Stack Manager is used to:

  • Add additional substacks (you actually add Sections, which can contain one or more substacks - more on this later).
  • Align the substacks in the Z-plane.
  • Configure the relationships between layers in adjacent substacks - do they share layers (Common), or are the layers unique in that substack (Individual).
  • Configure if adjacent layers intrude into the neighboring substack.
  • Add additional Branches (Branches are used when the design has a rigid section that has more than two flex sections radiating from it - more on this later).

Configuring the Layer Stacks

A Board can include any number of Sections, and each Section can include one or more Substacks. Regardless of the type of board, the approach is to define a Substack for each Region of the board. The video below shows a rigid-flex board with five regions and five Substacks.

Learn more about defining Board Regions

Board mode is currently in closed Beta, Open Beta builds will present the multiple layer stack selector used in previous versions.

Note that Board mode is only available in closed Beta builds.

Each Substack is created within a Section. Why do you need Sections? Because you can also create multiple Substacks within one Section, a feature you use when you are creating a bookbinder-style rigid-flex board (two rigid regions connected by multiple flex regions).

A bookbinder style rigid-flex PCB, note that the center Section has two Substacks. Note that Board mode is only available in closed Beta builds.

Working in the Layer Stack Manager:

  • Once Rigid-Flex mode has been enabled, the Layer Stack Manager opens in Board mode, where new substacks are added and aligned with the adjacent substacks.
  • To edit the layers and layer properties of the selected substack (selection is indicated by a pale blue outline, as shown above), either double-click on the Substack or use the Layer Stack Manager navigation bar to select the required substack and open the Stackup editor. Add and configure the layers as required.
  • To return to the Board mode after editing a substack, click the Home button  in the Layer Stack Manager navigation bar.

Adding and Mating a New Substack

As well as being used to add new substacks, Board mode is also used to align the adjacent substacks and define the various junctions between the different regions of the board.

Board mode is currently in closed Beta.

Note that Board mode is only available in closed Beta builds.

Creating and aligning Substacks:

  • To add a new substack, click the  button and select the appropriate command to position the new Section (substack) in the required location.
    • Section before - place the new Section and substack to the left of the currently selected Section
    • Section after - place the new Section and substack to the right of the currently selected Section
    • Section in - place the new Substack within the currently selected Section
    • Branch - create a new branch, starting from the currently selected Section. More about branches below.
  • After clicking the required command a small dialog will appear (as shown above), use this to: define the Number of shared (copper) layers, and optionally include or exclude Coverlays and Adhesive layers.
  • The new section will be created, double-click on the Substack to open it in the Stackup editor.
  • Configure the layers as required, then click the Home button  in the Layer Stack Manager navigation bar to return to the Board mode.
  • Edit the Substack Name in the Properties panel to reflect their function in the overall design.
  • If required, the last step is to mate the new Substack with the previous Substack (position them relative to each other in the Z plane). This is done by:
    • Selecting the substack
    • Displaying the Properties panel
    • Setting the Mapping Layer (the key layer on the selected Substack) to suit the Reference Layer (the key layer on the previous Substack)
  • Continue to add a Substack for each Region in the rigid-flex design, aligning each new Substack with the previous Substack.

In previous versions it was necessary to enable the Is Flex option to configure a Substack as Flex, this is no longer required.

After adding a Substack, mate it to the previous Substack and configure the name. Note that Board mode is only available in closed Beta builds.

Material Usage

A rigid-flex design often has copper and dielectric layers that are common through the rigid and flex regions, but different outer dielectric layers, such as the coverlays. To help the designer manage this, the Properties for the selected substack includes a Material Usage option.

  • Common - material usage means: all layers in the substack with the least layer count must have identical layers (and properties) as the layers in adjacent substacks. This includes both the common copper/dielectric layers as well as any special purpose outer dielectric layers, such as coverlays.
  • Individual - enable the Individual mode to allows different combinations of materials in this substack.

Creating a Branch

If the design has a rigid section that has more than two flex sections radiating from it, you will need to create a Branch. In the example below, there are four flexible sections radiating from the main board, and each flex region has a small rigid region at the end.

Branches require Board mode, which is currently in closed Beta.

In a design with Branches, Substacks are assigned to Regions in the same way.

This board requires the use of the Branch feature. A Branch grows from a section, one section can have multiple branches radiating from it. In this example the MainBoard section has four branches; FirstFlexBranch, SecondFlexBranch, ThirdFlexBranch and ForthFlexBranch.

Use the controls in the Navigation Bar to switch from one Branch to another. Note that Board mode is only available in closed Beta builds.

Working with Branches:

  • A Branch is created with the currently selected Substack as its base, select the required Substack before adding a Branch.
  • Click the  button and select Branch from the menu. The new Branch will appear, containing just the common Substack being branched from. Enter a suitable Branch Name in the Properties panel.
  • Add new Substacks to the Branch, as required.
  • Use the Layer Stack Manager's Navigation Bar to switch from one Branch to another.

Defining the Board Shape and Regions

The layer stack defines the board in the vertical direction, or Z plane. In the PCB editor, the area that the board occupies in the X and Y planes is defined by the Board Shape. The board shape can be a polygonal region of any shape, with straight or curved edges that lie at any angle, that can also include cutouts (internal holes) of any shape.

There are two techniques that can be used to defining the overall board shape and the various rigid and flex regions:

  1. Define the overall board shape, and then slice it into regions. Learn more about defining the Board Shape.
  2. Place each rigid and flex board region in the workspace to build up the final board shape. Learn more about placing Board Regions.

The final shape can be created using a mixture of the two techniques.

Defining the Board Shape

  • The board shape can be defined interactively in Board Planning Mode (View » Board Planning Mode), or it can be defined based on an existing outline in 2D layout mode (View » 2D Layout Mode).
  • To define the board shape from an existing outline, select the outline in 2D layout mode and run the Design » Board Shape » Define from selected objects command (or the Tools » Convert » Create Board Region from selected primitives command). The software will trace along the centerline of the selected track/arc objects to define the outer edge of the board shape.
  • To define the board shape interactively, switch to Board Planning Mode and select the Place » Board Region command (or click the  button on the Active Bar). The standard region object placement behaviors apply, use the Snap Grid and workspace Guides to help with this process. Enable the Board Shape option in the Snap Options palette to give the best level of control during Board Region editing. Learn more about Understanding the Snap Behavior.
  • Place the required number of Regions. Regions can be drawn so they are overlapped, note that this does not define the extent that a flex region overlaps into a rigid region, that is defined by the Intrusion values in the Stackup definition.
  • To define the Name and assign a Layer stack for each region, select the region and edit the properties in the Board Region mode of the Properties panel.
  • To slice a Board Region into two smaller regions, use the Design » Slice Board Region command (or click the  button on the Active Bar). The Slicing tool uses the standard line placement cornering modes, including 45°, 90°, 45° arc, 90° arc and any angle, press Shift+Spacebar to change the mode during slicing.
  • The location and shape of an existing Board Region can be edited, using the standard polygonal object editing techniques.
  • In earlier versions of the software, the boundary between two Board Regions was defined by placing a Split Line. Split Lines are not used anymore, now the edge of the Board Region defines where one substack ends and the adjacent substack begins. If two Board Regions are overlapped (and those regions have common layers), then the stack with more layers is applied in the overlapping area.
  • When overlapped regions do not have common layers they can be folded independently.
  • More settings to control this behavior will be available soon in the Layer Stack Manager.

Learn more about defining the Board Shape

Defining the Bends

A bend in a flexible section of a rigid-flex board is defined by placing a Bending Line. A bending Line is a linear object, whose properties are edited in the Bend mode of the Properties panel.

Placing Bending Lines

  • Bending Lines are placed in Board Planning Mode (1 shortcut).
  • To place a Bending Line run the Place » Define Bending Line command (or click the  button on the Active Bar). Place the Bending Line across the flexible Board Region. It is not necessary to precisely touch each edge of the region with the start and end of the Bending Line, the software will automatically extend it (if too short) or reduce it (if too long). At least one end of the Bending Line must touch or pass over the edge of the Region.
  • To edit the properties of a Bend, select it and edit the settings in the Bend mode of the Properties panel:

    • The Bend zone is displayed in a green-orange color, click anywhere within the zone to select that Bend.

    • Each Bend can be named so it can be easily identified.

    • Confirm that the Bend is being applied to the correct Substack Region, available regions are listed in the Stack Regions section.

    • Set the Bend Zone Radius and Bend Angle as required.

    • Bends are folded in the order of their Fold Index, use this feature when the folding order is important to check.

  • To move a Bending Line, click and drag on each end handle.

  • Bending Lines can be applied to board cutouts edges.

  • A selected Bend can be removed by clicking and holding on one of the vertices, then pressing Delete on the keyboard.

Learn more about placing Bending Lines

Displaying and Folding a Rigid-Flex Design in 3D

The PCB editor includes a powerful 3D rendering engine, which allows the presentation of a highly realistic three-dimensional representation of the loaded circuit board. This engine also supports rigid-flex circuits, and when used in combination with the Fold State slider in the PCB panel, it allows the designer to examine their rigid-flex design in the flat state, the fully folded state, and anywhere in between.

To switch to the 3D display mode, press the 3 shortcut key (press 2 to return to 2D or 1 to return to Board Planning Mode). The board will be displayed in 3D. If the component footprints include 3D body objects that define the mounted component, these will also be displayed. In the image below, you can see that the board includes a battery and a battery clip.

To apply all of the Bending Lines, slide the Fold State slider in the PCB panel when set to Layer Stack Regions mode as highlighted in the image below. Note that the bends are applied in the order defined by their sequence number. Bending Lines can share the same sequence number; it simply means that those bends will be folded at the same time when the Fold State slider is used. The board can also be folded/unfolded by running the View » Fold/Unfold command (or by pressing the 5 shortcut).

Use the Fold State slider (or the 5 shortcut key) to apply all Bending Lines in the order defined by their sequence value (Fold Index).

3D Movie Maker Support for Rigid-Flex Designs

The ability to fold a rigid-flex design can also be captured as a 3D movie. It is very simple to do and does not require the use of movie key frames during the folding sequence.

Refer to the PCB 3D Video page for a detailed description of how to make a 3D movie. As a basic guide:

  1. Switch the PCB editor to 3D mode.
  2. Open the PCB 3D Movie Editor panel and create a new video by clicking the New button. Click the newly-created video in the Movie Title region then give it a suitable name.
  3. Create an initial Key Frame showing the board in its unfolded state.
  4. Slide the Fold State slider to show the rigid-flex design in its folded state, then position the folded board as required.
  5. Now create a second Key Frame for this view and set the time. Consider how long you want it to take to fold the rigid-flex design (the Duration setting); typically this would be a few seconds.
  6. To check that the video captures the folding process correctly, click the play button (located in the player controls at the bottom of the panel.
  7. To generate a movie file, add a PCB 3D Video Documentation Output in an Output Job file. Remember to configure the video format options in the Video settings dialog.
  8. Click the Generate Content link in the Output Job file to create the movie file.

The video below was created using this process. It has the two key frames described above, plus one additional key frame that was added at the end to hold the final position for a second.

A simple 3D movie created from three key frames; the folding behavior is defined by the Bending Line Sequence values.

Learn more about 3D PCB Video

Design Considerations

Below is a summary of key design areas that must be considered when designing a rigid-flex PCB:

  • Conductor routing - choice of corner style for routes traveling over a flex region is important; avoid sharp corners; use a curve for least stress.
  • Pad shape and area - use fillets (teardrops) with rabbit ears (anchoring spurs) for single-sided flex. The objective is to capture some of the pad shape with the coverlayer.
  • Through holes - try to avoid through holes in the bend area, particularly in a dynamic application.
  • Coverlayer - avoid stress risers (exposing the incoming track); reduce opening in coverlayer to 250um.
  • Planes - crosshatched, if possible.
  • Staggered lengths - to avoid bookbinding (layer buckling when flexed), stagger the layer lengths by approx 1.5 times the layer's thickness.
  • Service loop - make the flex region slightly longer to help with assembly/disassembly and to allow for product dimensional variations (the extra length is referred to as the service loop).
  • Conserve copper - consider how the flex circuit will be panelized; it might be better to adjust the design to ensure best material usage.
  • Panelization - orient the flex regions to suit the grain of material (bend along the grain).
  • Tear resistance - curved corners; drilled hole at corner; hole in slit; leave metal in corners.
  • Routing - stagger the routes on two layer boards to avoid I beaming, and widen the routes through the bending zone (this is especially important for permanent bends).
  • Static Bend Ratio - setting the ratio of the bend radius to the circuit thickness. Ideally, multi-layer circuits should have a bend ratio of at least 15:1. For double-sided circuits, the minimum ratio should be at least 10:1. For single-layer circuits, the minimum ratio should also be at least 5:1. For a dynamic application, aim for a bend ratio of 20-40:1.
  • Rolled annealed copper is more ductile; plated copper is not the best choice for flexible regions.

Documentation and Drawing Requirements

Typical suggested documentation requirements include: 

  1. The Flex PCB shall be fabricated to IPC-6013, class (your requirement here) standards.
  2. The Flex PCB shall be constructed to meet a minimum flammability rating of V-0 (if required).
  3. The Flex PCB shall be RoHS compliant (if required).
  4. The rigid material shall be GFN per IPC-4101/24 (if using epoxy material).
  5. The rigid material shall be GIN per IPC-4101/40 (if using polyimide material).
  6. The flexible copper clad material shall be IPC 4204/11 (flexible adhesive-less copper clad dielectric material).
  7. The covercoat material shall be per IPC 4203/1.
  8. The maximum board thickness shall not exceed (your requirement here) and applies after all lamination and plating processes. This is measured over finished plated surfaces.
  9. The thickness of acrylic adhesive through the rigid portion of the panel shall not exceed 10% of the overall construction. See comments on this above.
  10. Pouch material can be used for ease of manufacturing and must be removed from the flexible portion of the board prior to shipping.
  11. The flexible section thickness shall be (your requirement here). Do not add this note if this thickness is not critical.
  12. Minimum copper wall thickness of plated through holes to be (your requirement here; .001” average is recommended) with a minimum annular ring of (your requirement here; 002 is recommended).
  13. Apply green LPI soldermask (if required) over bare copper on both sides in the rigid sections only of the board. All exposed metal will be (specify your surface finish requirement here).
  14. Silkscreen both sides of the board (if required) using white or yellow (most common) non-conductive epoxy ink.
  15. Marking and identification requirements.
  16. Electrical test requirements.
  17. Packaging and shipping requirements.
  18. Impedance requirements.

Additional Drawing Detail

  1. A drill table detailing finished hole size, associated tolerances and plated/not plated.
  2. A dimensional drawing, including reference datum(s), critical dimensions, rigid to flex interfaces, bend location and direction markers.
  3. Panelization detail, if required.
  4. Construction and Layer detail, detailing material used for each layer, thicknesses and copper weights.


Flex Circuit Design Guide - Epec Engineering Technologies

Flexible Circuit Technology - Joe Fjelstad

Flex Circuits Design Guide - Minco Products Inc

Machine Design website:


Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.



We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
You are reporting an issue with the following selected text
and/or image within the active document:
Altium Designer 無償評価版
Altium Designer 無償評価版
Altium Designerを使用していますか?

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited


弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited


ボタンをクリックして、最新のAltium Designerインストーラをダウンロードしてください。

Altium Designerインストーラをダウンロードする

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

Altium Designerの新規ライセンスのお見積もりをご希望の場合、下記のフォームに入力してください。


Altium Designerサブスクリプションをご利用中の場合、評価版ライセンスは不要です。

お客様がAltium Designerサブスクリプションの有効なメンバーではない場合、下記のフォームに入力して無償評価版をダウンロードしてください。


Altium Designerを評価する理由を下記から選択してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited



Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.


その場合、Altium Designerビューワーの無償ライセンス(有効期間6か月)をダウンロードできます。





試してみる場合、こちらをクリック してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

その場合、Altium Designerビューワーの無償ライセンス(有効期間6か月)をダウンロードできます。