1. Introduction

Flanged joints are a critical component in piping systems, used to connect pipes, valves, pumps, and other equipment. A typical flange assembly consists of two flanges, bolts, a gasket, and sometimes welded pipes. These joints are designed to withstand high pressures and temperatures while maintaining a tight seal to prevent leaks.

However, flanged joints are also frequent points of mechanical failure. Common issues include gasket degradation, bolt relaxation, corrosion, improper preload, and flange distortion. These failures can compromise joint integrity, cause leaks, and lead to costly unplanned shutdowns or safety incidents.

Figure 1.1. Flange Joint system

One such maintenance procedure is hot bolting, or single stud replacement, which involves removing and replacing bolts on a pressurized flange joint without system shutdown. Defined by ASME PCC-2:2022, hot bolting is widely used in the oil and gas, petrochemical, and refining sectors to safely replace degraded or corroded bolts while minimizing downtime. 

Traditionally, maintenance on bolted flanges required a full shutdown to ensure safety. Hot bolting enables continuous operation, reducing production losses and maintenance costs. For example, a 2019 campaign on 142 flanged joints reduced planned shutdown time from 14 days to just 3 days. Beyond bolt replacement, hot bolting is also used for material upgrades, correction of assembly defects, and mitigation of aging infrastructure.

To ensure safety during such operations, finite element analysis (FEA) is essential for understanding complex interactions in the joint, such as gasket compression, bolt stress variation, and load redistribution. Traditional FEA methods, however, are often time-consuming and require expert modeling skills.

1.1 Structural Performance Management (SPM) for Flanges Overview

To address the complexity and risks involved in flange joint assessment, Akselos developed the Structural Performance Management (SPM) for Flanges software, an automated finite element analysis (FEA) tool designed for evaluating the structural behavior of bolted flange connections. The software generates accurate simulation models of flanges, bolts, gaskets, and optional pipe and weld components using industry-standard geometry and material libraries.

Figure 1.2. SPM for Flanges interfaces

Its interface is divided into five key sections: Geometry, Material, Boundary Conditions, Load Sequence, and Result Assessment, allowing users to configure and analyze flange assemblies with minimal manual setup. Model variations, such as standard and root-diameter bolt definitions or the inclusion of pipe and weld extensions, offer flexibility in fidelity depending on the analysis objective.

This software includes a comprehensive set of features that simplify complex analyses and ensure consistent, standard-aligned results. Notable capabilities include:

• Automated FEA model creation based on ASME-standard geometries for flanges, bolts, gaskets, and optional pipe and weld elements
• Support for diverse scenarios, including bolt tightening sequences, gasket degradation, and hot or half bolting operations
• Integrated material and gasket property libraries, sourced from industry-recognized standards and databases
• Built-in result assessment tools, such as flange rotation charts, bolt stress polar plots, and gasket pressure risk matrices
• Ability to analyze shared solutions, making it easy to collaborate and review solved models without rebuilding them

1.2. Applications

The SPM for Flanges tool is built to help engineers manage the real-world challenges of maintaining and evaluating the integrity of bolted flange joints under operating conditions. It’s used across industries where safety, reliability, and minimizing downtime matter, especially in systems handling high pressure and temperature. By automating complex FEA tasks, the tool makes it easier to define realistic geometry, assign accurate materials, apply detailed loading conditions, and simulate scenarios ranging from assembly to full operational loads, including hot and half bolting cases.

The tool is currently being applied and tested in a variety of practical situations, such as:

• Bolt Torque Estimation: Finding the right torque range while avoiding overstress in the bolts or flanges.
• Tightening Sequence Optimization: Testing different bolt tightening methods to achieve even preload and reduce leak risks.
• Bolt Tensioning Strategies: Supporting hydraulic tensioning methods (both A and B), including multi-pass routines for better load control.
• Full vs. Partial Bolting: Studying how the joint performs when some bolts are removed or left untightened.
• Piping Thickness Effects: Going beyond standard ASME PCC-1 tables to assess bolt stress limits for non-standard pipe sizes.
• Hot and Half Bolting Procedures: Simulating bolt replacement under pressure using clamps, helping teams plan safer operations.
• Leak Probability Estimation: Using gasket stress results and field data to predict leak likelihood.
• Material and Design Changes: Evaluating how adjustments in gasket width, bolt material, or flange condition affect performance.
• Variable Load Risk Assessments: Running simulations under changing pressure, temperature, and external loads to support smarter maintenance planning.

2. Before we start

Before using the SPM for Flanges tool, it’s helpful to understand how it fits within the broader Akselos Integra® platform. Integra combines local modeling, cloud computing, and centralized data management to support an efficient simulation workflow. This architecture ensures that users can build, solve, and manage models smoothly across connected tools.

• Akselos Modeler (local desktop application): Used to build the flange model, define geometry, materials, and load conditions, and visualize results. It serves as the user interface for model setup and post-processing.
• Akselos Cloud (server back-end): Handles all simulation solving processes. Once models are synced from the local machine, the cloud performs high-speed computations without requiring local resources.
• Akselos Portal (web-based front-end): Used to manage collections, organize simulation jobs, track solve progress, and access shared results. It enables collaboration and centralized data control.

Figure 2.1. Akselos Integra

Once the model is built in Modeler, it is synced to the Cloud for solving. The Portal manages these synced collections and jobs, while the final results are returned to the Modeler for visualization or accessed through the Portal for review and documentation.

To ensure a smooth setup and workflow, it’s recommended to complete a few setup steps and review relevant support materials on the Akselos Portal.

Specifically, users should:

1. Create an Akselos Portal account and ensure access to the necessary workspace and collections. Reference: [Create Akselos Portal Account] – Required to access the platform and use the tool.
2. Set up a blank collection in the assigned workspace to serve as the foundation for your model.  Reference: [Start Building Your Model with a New Collection] – Instructions for setting up a new model collection.

Completing these steps and familiarizing yourself with the articles above will help ensure a stable starting point for building and analyzing your flange joint models using the SPM for Flanges tool.

3. SPM for Flanges - Features and Functionalities

3.1. Analysis Flow (User Journey)

The overall workflow for creating and analyzing a flange joint model using the SPM for Flanges tool consists of four main phases:

Figure 3.1. SPM for Flanges user journey

1. Preparation: Covered in the Prerequisite section, this step involves setting up your workspace by creating a collection on the Akselos Portal and importing it into the SPM software.
2. Model Input and Auto Generation: As described in Section 3.2, users define model parameters such as geometry, materials, and loading conditions. The tool then automatically generates a ready-to-solve simulation model.
3. Data Synchronization: Since solving is cloud-based, the created model must be synced to the Akselos Cloud under the user's Portal account. This ensures the model is ready for remote processing.
4. Analysis and Assessment: After syncing, users can launch multiple analyses, visualize simulation results, and perform performance assessments such as gasket pressure risk, bolt stress checks, and flange rotation directly within the SPM for Flanges software.

3.2. Industry Standards & Compliance

The SPM for Flange aligns with key industry standards to ensure compliance with best practices and enhance the safety and reliability of operations.

Table 3.1. SPM for Flanges standards and compliance

Note: The list above includes the official standards referenced by the SPM for Flanges tool, along with the specific publication year adopted in this version. From this point forward, any mention of a standard (for example, “ASME B16.47”) should be understood to refer to the specific edition listed here (i.e., ASME B16.47 (2020)). This ensures consistency throughout the documentation and aligns all calculations, inputs, and assumptions with the intended version of each standard.

Disclaimer: The predefined values available in the SPM for Flanges Tool, including geometry dimensions, material properties, and gasket specifications, are sourced from external databases and industry standards. These values must be imported from the Akselos Cloud by users with appropriate permissions. While they serve as a useful reference, it is the user's responsibility to validate and confirm their applicability before use.
Users are responsible for:
Verifying the accuracy and relevance of all predefined input values for their specific application.
Ensuring consistency with project requirements, engineering standards, and actual operating conditions.
Making adjustments where necessary to reflect real-world configurations or non-standard use cases.

3.3. Input Data Requirements

3.3.1. Geometry Definition

The tool supports weld neck flanges and automates model creation using standard dimensions defined in ASME. Within the Geometry Tab of the SPM for Flanges tool, users can define key dimensional parameters for flanges, bolts, gaskets, and optionally pipes with welds. The tool references industry standards to prefill geometry values but also allows user-defined inputs for specific dimensions that are not fully covered by the standards, providing flexibility while maintaining consistency.

Figure 3.2. SPM for Flanges - Geometry tab

Once in the Geometry Tab, users only need to select:

• Flange Standard
• Pressure Class
• Nominal Pipe Size (NPS)

Figure 3.3.geometry Key input parameters

Based on these selections, the tool automatically fills in the corresponding dimensions for flange, bolt, gasket, and weld (if applicable), significantly reducing manual input effort and ensuring alignment with the referenced ASME specifications. Once these selections are made, the tool automatically fills in the dimensions.

Dimension of Flanges

Figure 3.4. Flange dimension

Flanges are used to connect pipes, valves, and equipment in a piping system. Their dimensions determine compatibility with pipes and sealing efficiency.

• Diameter of Outer Flange (O): The total external diameter of the flange.
• Minimum Thickness of Flange (tf): The minimum thickness required to ensure the flange can handle the required pressure.
• Diameter of Hub (X): The width of the hub section that transitions from the pipe to the flange.
• Diameter of Neck Chamfer (Ah): The chamfered area at the transition between the hub and pipe for welding.
• Length Through Hub (Y): The total length of the hub, including the welding section.
• Bore (B)*: The inner diameter of the flange, matching the pipe ID.
• Diameter of Raised Face (R): The area where the gasket is placed for sealing.
• Height of Raised Face (t): The thickness of the raised face, ensuring proper gasket compression.

Bore Dimension(*)
In this version of the SPM for Flanges tool, users can edit the bore dimension for all flange classes in ASME B16.47 (2020) and ASME B16.5 (2020), except for Class 150 and Class 300 in ASME B16.5, where it remains fixed because these lower-pressure flanges follow standardized bore sizes to ensure compatibility with pipe schedules, prevent misalignment, and maintain gasket sealing integrity.

Dimension of Bolt

Bolts are critical in securing flanges, ensuring proper alignment and pressure distribution. Their key dimensions are:

Figure 3.5. Bolt dimension

• Diameter of Bolt Circle (W): The circular pattern where bolts are placed in a flange.
• Number of Bolts (BN): The total number of bolts used to fasten the flange.
• Diameter of Bolt Hole (BH): The hole size for bolts to pass through.
• Root/Diameter of Bolt (RBD): The smallest diameter of the bolt thread (measured at the thread valley), which is the weakest point and is used for stress calculations.
• Diameter of Head Bolt (HD): The width across the bolt head.
• Height of Head Bolts (HH): The thickness of the bolt head.

Use Root Diameter: This option is often checked in calculations when using the root diameter (RBD) instead of the major diameter. The root diameter is used in stress analysis because it represents the bolt's weakest section under tension.
Bolts used in flanges often follow Unified Thread Standards (UNS), categorized into two common types:
UNC (Unified National Coarse) threads have fewer threads per inch (TPI) for quick assembly and better stripping resistance.
UNF (Unified National Fine) threads have more TPI for stronger engagement and better vibration resistance.

Dimension of Gasket

Gaskets are used between flanges to prevent leaks. Their dimensions include:

Figure 3.6. Gasket dimension

• Diameter of Inner Gasket (IGD): The inner opening of the gasket, aligning with the bore.
• Diameter of Outer Gasket (OGD): The external diameter of the gasket.
• Thickness of Gasket (tg): The thickness of the gasket material, which affects its sealing performance.

Dimension of Pipe and Weld

Weld preparation ensures strong and durable welded joints between pipes and flanges. In this version of the SPM for Flanges tool, both the pipe material and the weld dimensions are only considered in stress and strength calculations when the "Include Pipe and Weld" option is turned on. Key dimensions include:

Figure 3.7. Pipe and weld dimension

• Length of Pipe (LP): The length of the connected pipe segment. Set at five times the bore size.
• Bevel Angle (BA): The angle of the beveled edges before welding to allow better penetration.
• Face Reinforcement (FR): The extra weld material on the face for added strength.
• Root Opening (RO): The gap between the pipe ends before welding to ensure complete fusion.
• Root Face (RF): A small flat section at the root of the weld to help control penetration.

3.3.2. Material Properties

The Material Tab in the SPM for Flanges Tool provides a material library and an assignment interface for different components. Users can assign different materials for the following components:

1. Flange : The primary structural element connecting the pipe.
2. Bolt : The fastening element securing the flange assembly.
3. Gasket : The sealing component placed between flange faces.
4. Pipe (if enabled in the Geometry Tab) : The conduit for fluid or gas transport.
5. Weld (if enabled in the Geometry Tab) : The welded joint between the flange and pipe.

Figure 3.8. SPM for flanges - Material tab

Material Library

The tool provides a material library that includes:

• Elastic Materials : Up to 583 temperature-dependent elastic materials, sourced from ASME BPVC Section II, Part D.
• Gasket Properties : Up to 261 nonlinear gasket materials, including Elastomer, Fiber, Graphite, Mica, and PTFE.

The SPM for Flanges Tool allows users to import material data from the Akselos Cloud. The following options are available:

Figure 3.9. download material database

• Minimal Database: Contains 10 elastic materials and 10 gasket materials, suitable for quick setup and testing.
• Full Database: Provides access to 583 elastic materials and 261 gasket materials, covering a wide range of industrial applications.

Import a database

1. Ensure your Akselos Portal account has permission to access the database ([email protected])
2. Click the download icon in the Material Tab.
3. Click the download icon next to the desired database option (Minimal Database or Full Database) in the dialog.
4. Wait for the database to be loaded into the tool.
5. Once imported, the materials will be available for selection in the Material Library (“Define” button is enabled)

Define material

Clicking "Define" opens the Materials Library, where users can select or modify materials based on engineering standards.

Elasticity material group

Figure 3.10. elasticity materials

The elastic properties of flanges and bolts change with temperature and must be considered in the analysis. User can define the material for flange, bolt, pipe and weld with these Material Information Fields:

• Product Form : Defines the material shape (e.g., bar, plate, forging).
• Specification Number (Spec. No.) : The material’s compliance with industry standards (e.g., ASME SA-276).
• Type/Grade : Defines the material classification (e.g., stainless steel, carbon steel).
• Alloy Designation/UNS No. : Specifies the material’s chemical composition.
• Class/Condition/Temper : Indicates heat treatment or processing conditions (e.g., solution annealed, normalized).

And the Mechanical and Thermal Properties, These properties define how the material behaves under stress, temperature changes, and mechanical loads:

• Young’s Modulus : Measures material stiffness and elasticity.
• Poisson’s Ratio : Describes how the material deforms under applied loads.
• Density : Defines mass per unit volume, affecting weight and load calculations.
• Thermal Expansion Data : Determines material expansion and contraction at different temperatures.
• Yield Strength : Indicates the stress at which permanent deformation occurs.
• Allowable Stress Data : Defines the maximum stress the material can withstand under ASME standards.

Gasket material Group

The gasket material exhibits nonlinear behavior, characterized by distinct loading and unloading curves that influence its deformation and sealing performance.

Figure 3.11. Gasket material

• Loading Curve: Describes how the gasket compresses under pressure.
• Unloading Curve: Defines how the gasket recovers when pressure is released.

Reference Temperature

By default, material properties (except for gaskets) are temperature-dependent. The tool provides a Material Converter Feature that allows users to convert them into temperature-independent values using a specified Reference Temperature, which helps verify material properties under specific conditions and simplifies material handling in the model.

Figure 3.12. material customization option - reference temperature

How to Use:

• Check "Allow Reference Temperature" to enable the feature.
• Enter the desired Reference Temperature.
• The tool will adjust the material properties accordingly.

Note: This feature applies only to elastic materials and does not affect gasket materials.

3.3.3. Boundary Conditions

This tab is used to define loading values applied to the model, as well as the contact settings between the flange-gasket and flange-bolt interfaces.

Figure 3.13. spm for flanges - boundary conditions

The configuration is based on recommendations and evaluation procedures from ASME PCC-1, ASME PCC-2, and ASME BPVC Section VIII, Division 2. These standards form the basis for the types of loads and constraints included in the SPM for Flanges model. Key assessments supported by the boundary condition setup include:

• Joint Pressure and Tightness Testing (ASME PCC-1)
• Pressure Testing Procedures (ASME PCC-2)
• Protection Against Plastic Collapse (ASME BPVC Section VIII, Division 2)

Figure 3.14. applied loads on model illustration

The Boundary Conditions Tab in the SPM for Flanges tool enables users to configure all necessary loads, constraints, and contact interactions in accordance with these standards. The following sections will guide users through the correct input setup.

Table 3.2. Applied loads position

Figure 3.15. boundary conditions key input parameters

Working Pressure

This is defined as internal pressure in the simulation model, representing the fluid pressure inside the flange and pipe. The value is user-defined and applied to the internal surfaces of the flange bore. If a pipe is included in the model, the pressure is also applied along the entire inner surface of the pipe.

Working Temperatures

This defines the temperature conditions applied to the flange, bolts, gasket, and pipe surfaces, affecting material properties and thermal expansion behavior.

The following temperature parameters are specified:

• Environment Temperature: Applied to the external surfaces of the flange assembly, representing ambient conditions.
• Assembly Temperature: Defined at the bolt locations, representing the temperature during tightening.
• Operating Temperature: Applied to all components, simulating in-service conditions.

Which temperature value is applied at each stage of the analysis is defined in the next step : Load Sequence.

Pretension Load

The Pretension section allows users to define the initial preload applied to the bolts through two options: direct pretension input or torque-based calculation.

Direct Pretension Input

This option allows users to define the pretension load in two ways:

• Manual : Enter a specific pretension load in kN based on design requirements.
• Auto : Press the 67% Yield button to automatically calculate the pretension load as 67% of the bolt's yield strength.

Bolt Torque Input

Instead of directly entering the pretension load, users can define it using torque (N·m) and a Torque Coefficient (Nut Factor). With the bolt diameter automatically retrieved from the Geometry Tab, the tool calculates and converts the applied torque into the corresponding pretension load, considering friction effects and thread engagement.

Piping Loads

Piping load represents the forces and moments transferred from the connected pipeline due to thermal expansion, internal pressure, and external constraints. The Piping Load in the tool is applied at the center top of the model to simulate these effects.

Defined inputs:

• Forces (X, Y, Z) : Axial and lateral loads applied to the pipe.
• Moments (X, Y, Z) : Bending and torsional effects from piping constraints.

Clamping Loads

In the hot/warm bolting process, a clamp is used as a tool to temporarily support and redistribute bolt load while individual bolts are loosened or replaced. The Clamping Load in the tool represents the total of multiple clamping forces, applied at the center top of the model, simulating this external support. This setup is acceptable when the model does not include a welded pipe and the Clamping Loads are symmetric about the flange axis.

Defined inputs:

• Forces (X, Y, Z) : External loads acting on the flange assembly.
• Moments (X, Y, Z) : Rotational effects from structural constraints.

Note: When the Pipe and Weld option is enabled in the Geometry Tab, the piping load and clamping load is applied to the top of the pipe end instead of the flange. The tool does not allow modification of this placement.

Contact Settings

Contact settings define the interaction between different components in the bolted flange assembly, influencing load transfer, deformation, and sealing behavior. These settings ensure proper simulation of mechanical constraints, friction effects, and separation behavior under operational conditions.

Table 3.3. default contact settings in som for flanges

The default contact settings are selected to provide the most accurate representation of the bolt-flange and flange-gasket interactions.

• For the Flange-Gasket Connection, Frictional Contact is recommended, as it best captures the sealing behavior. However, in cases where solver convergence issues arise, users may switch to Bonded Contact as an alternative.
• For the Bolt-Flange Connection, Bonded Contact should be maintained, as it ensures proper load transfer and structural integrity.

Recommendation: Users should follow the default settings unless a specific need arises, as deviations may lead to inaccurate results or solver instability.

The tool supports several advanced contact options to accurately simulate interaction between components in the flange assembly. These settings apply based on the selected Contact Type and interface location (e.g., Bolt–Flange or Flange–Gasket).

Bonded Contact: 

Touching surfaces behave as if they are permanently glued/welded together; no slip, separation, or penetration can occur. It is recommended that the independent surface is more finely meshed than the dependent surface.

• Influence Distance: Max initial separation beyond which no bonding will occur. This value will be used for all elements in this bonded zone. In some cases, increasing this value can help with solution stability and result quality by ensuring each node on the slave surface can bond with more nodes on the master surface.

Frictionless and Frictional Contact

Allows separation between surfaces:

• Frictionless Contact permits separation but prevents resistance to sliding.
• Frictional Contact includes both separation and sliding, with frictional resistance.

When using Frictionless or Frictional Contact, the following options are available:

• Enforcement Methods:
  • Augmented Lagrangian: An extension of the linear penalty method, this adds additional degrees of freedom and iterations to ensure the converged penetration is below the defined penetration tolerance. This approach is the most precise, but also the most computationally expensive.
  • Linear Penalty: Overclosure is corrected by applying the numerical equivalent of a stiff linear spring, where contact force scales with penetration distance. Some penetration will occur, but this can help with numerical stability and efficiency.
  • Nonlinear Penalty: Overclosure is corrected by applying the numerical equivalent of a stiff nonlinear spring, where contact force scales with penetration distance. Low initial stiffness typically results in better convergence and stability, and high stiffness at large overclosures avoids excessive penetration.
• Contact Type:
  • Node to Surface: Nodes on the slave side interact with a surface on the master side. Slave nodes cannot penetrate the master surface, but in some cases master nodes could penetrate the slave surface. Typically the master surface should be defined as the surface with a coarser mesh.
  • Surface to Surface: Contact penetration conditions are enforced over surface patches rather than individual nodes. In general this provides more accurate stress/pressure results on contact surfaces, and is less sensitive to the choice of master/slave surfaces.
• Additional Parameters:
  • Contact Penalty: Scaling factor for the contact penalty. This can have a large effect on the convergence of certain contact problems. Must be a value greater than 0.0.
  • Cₜ Parameter: Also called tangential contact stiffness, it controls the stick/slip transition: a higher value will result in faster transition to slip. This value is a scaling factor for the default tangential contact stiffness computed internally.
  • Friction Coefficient (μ): Coefficient of friction (μ).
  • Gap Function: The distance below which contact surfaces are considered to be touching.

3.3.4. Load Sequences

The Load Sequence Tab allows users to define which loads are applied at each step of the analysis. The process is divided into three phases: Tightening, Operation, and Hot Bolting. This is the final input step before generating the model for analysis.

Figure 3.16. spm for flanges - load sequences tab

With the input load values already defined in the Boundary Conditions tab, users can adjust the load sequence to match different analysis scenarios by changing the bolt state at each step, such as Load, Lock, or Open. External loads like internal pressure, clamping force, or piping load can be controlled using coefficient values. A coefficient of 1 applies the full load, 0 deactivates it, and intermediate values such as 0.8 apply a partial load. This setup allows engineers to simulate a wide range of flange behavior, from standard tightening procedures to detailed hot bolting sequences, while maintaining full control over the load progression.

table 3.4. stages in bolt tightening sequence

Tightening Stage

This section defines the bolt tightening sequence and initial pretension application in the SPM for Flanges Tool. The tightening process consists of multiple stages to ensure uniform preload distribution and prevent flange distortion.

Each bolt tightening or removal operation in the simulation consists of at least three steps (not necessarily in order):

• Load: The process of tightening the bolt with external force (e.g., wrench).
• Lock: The state where the bolt remains tightened even after the external force (e.g., wrench) is removed.
• Open: The state where the bolt is fully loosened and no longer applies clamping force.

Note: Removing a bolt in the SPM for Flanges Tool removes the effect of the tightened bolt but does not remove its geometry from the model.

Users can select different tightening options based on real-world applications.

• One time pattern:All bolts are tightened in a single step using auxiliary tightening machines
  • Bolt Relaxation: Accounting for preload loss when transitioning from Load to Lock condition. The relaxation factor is a percentage based on the input pretension load.
• Cross Pattern:This option allows users to apply the Tightening Sequence following ASME PCC-1, a structured process designed to ensure uniform bolt preload and prevent flange distortion. The maximum total rounds can be adjusted up to 7.

The sequence consists of three main stages:

1. Installation Round: Initial snug tightening.
2. Star Pattern Rounds: Incremental torque application using a cross-pattern. The pattern type and torque increment depend on the selected tightening method:
   • Legacy Pattern
   • Modified Legacy Pattern
3. Circular Clockwise Pattern Rounds (optional): final tightening pass to stabilize bolt preload and compensate for relaxation.

Table 3.5. Tightening Stages and Patterns

Note: By selecting a tightening sequence, the tool will automatically adjust the pretension load values according to the selected pattern. Users can review and verify these values in the Summary Table at the final step of the Load Sequence tab (see Section 3.3.4.5. Summary Table). This ensures that the pretension levels align with the intended tightening method before generating the model.

Non-tightenable Bolts

In real-world applications, certain bolts may be inaccessible and cannot be fully tightened due to space constraints or equipment obstructions. The Untightened Bolts feature allows users to represent this condition accurately in the simulation model.

When a bolt is marked as Untightened, the tool automatically sets its state to Open (0) in every load step. This means the bolt does not contribute to the preload or clamping force throughout the analysis. This feature ensures that the model reflects actual working conditions where certain bolts remain loose or non-functional.

Operation Phase

The Operation Phase activates external loads to simulate the normal working condition of the flange assembly. The first step in this phase represents the moment the flange enters service after the assembly is complete. At this point, users can adjust the following:

• Internal Pressure – Applied to represent the system’s internal pressure.
• Working Temperature – The value defined in the Boundary Conditions Tab is used here, replacing the Environment Temperature, to reflect actual operating thermal conditions.
• Piping Load – Applied if defined in the Boundary Conditions Tab.
• Clamping Load – Can be turned on or off based on user input.

By default, all loads (including Clamping Load) are active in the first operation step. Users can deactivate any load by setting its value to zero (0) under that load column.

Hot Bolting Phase

The Hot Bolting Phase is where users define all steps related to replacing bolts while the system remains in operation. This phase simulates the full hot or half bolting procedure under pressure and temperature. The steps are flexible and can be selected depending on the user’s case. Available actions are:

• Preparation (optional):
  • Apply clamping force
  • Reduce internal pressure
  • Reduce working temperature
• Bolt Removal:
  • Remove one bolt
  • Remove half of the bolts
  • Remove selected bolts
• Bolt Replacement:
  • Install new bolts
  • Remove clamps (if defined)
• Return to Normal Conditions (optional):
  • Restore original pressure and temperature values

These steps can be arranged and customized to simulate various hot or half bolting strategies, supporting accurate assessment of joint behavior during maintenance.

Summary Table

The Summary Table provides a complete overview of the applied loads and boundary conditions at each step of the load sequence. This allows users to verify the setup before generating the model.

Figure 3.17. load sequence key input parameters

Load Sequence for Hot Bolting example

Let’s walk through the steps of the Load Sequence tab using the example below to illustrate how a complete model is defined:

Figure 3.18. example hot bolting load sequence

1. Tightening Sequence: One Bolt at a Time (One Time)

When this option is selected, the tool automatically generates the following three steps:

• Bolt Pre-load: Applies 100% of the defined pretension value.
• Bolt Relaxation: Reduces the pretension to 84%, assuming a Bolt Relaxation Factor of 0.16, to simulate preload loss after tool removal.
• Bolt Lock: Maintains the remaining 84% pretension as the locked state.

2. Operation Phase

In this step, the model activates external loads, including:

• Internal Pressure
• Working Temperature

3. Hot Bolting Phase

 This phase simulates the replacement of a single bolt while the system remains in operation. The tool adds the following steps:

• Clamp Installation
• Bolt Removal and Replacement:
  • Open the old bolt
  • Load the new bolt (80% pretension load)
  • Lock the new bolt
• Clamp Removal

Figure 3.19. example hot bolting load sequence

4. Check summary table

Figure 3.20. example summary table

Update Boundary Conditions Feature

The Update Boundary Conditions feature allows users to modify and apply changes to the boundary conditions of the currently open model without creating a new one. This ensures that the latest settings are correctly applied before running the analysis and enables users to test different conditions efficiently.

Conditions for Use

This checkbox is disabled by default and becomes available only when an active model is open in the working window.

Geometry and Material settings must remain unchanged for this feature to function.

Notes: If the Class and NPS (Nominal Pipe Size) values do not match the currently open model, the feature cannot be used. To resolve this issue, update the Class and NPS values in the Geometry Tab before proceeding.

If users modify boundary conditions or load sequences, they can update the existing model or create a new simulation instance based on the revised settings.

3.3.5. Automatic model creation and validation

Create model

Once all inputs are confirmed, the Create Model function will utilise the configuration and automatically generate the analysis model based on the defined geometry, materials, and loading sequence. This process may take a few minutes. When complete, the fully configured model will appear in the graphics window, ready for the next steps in simulation and analysis.

Figure 3.21.automatic model creation

Model configuration final check

After the model is created, users can review all predefined settings directly in the model structure tree located in the Model Ribbon. This allows for a final check to confirm that all input parameters have been correctly applied before proceeding to the next step.

Figure 3.22. Model ribbon and structure tree

Check Materials

• Go to Components > select the component name (e.g., Bolts).
• Under Subdomain, select the specific part you want to check.
• The material properties will appear in the property panel below.

Check Boundary Conditions

• Constraints: Go to BC > Geometry Constraints. Selecting a constraint will highlight its position in the model.
• Contact Settings: Go to Contact Interactions, then select a contact surface to view its type and settings.

Check Loads

• In the Load Cases section, use the dropdown list to browse through all defined loads.
• Select each load to check the assigned values.

Tip: To visualize the load location, switch the Selection Mode in the graphic window. Load locations are stored using selection sets, which can be viewed directly on the model.

Once everything is verified and adjusted as needed, go to File > Save Model to save the setup. The simulation model created in Akselos software will be saved as Model_name.aks

Tip: If you plan to create multiple models for comparison, you can either:
Use the Update Boundary Conditions feature (see Section 3.4.4), or
Repeat the full model creation process and save each model with a unique name before moving on to data sync and solving.

3.4. Analysis Results

3.4.1. Data synchronization and solving

Data synchronisation

The Akselos solver engine is cloud-based, which means that, like all models assembled in Akselos Modeler—the flange joint model must be synced to the cloud before running any simulations.

Figure 3.23. collections > sync with portal

Steps to Sync the Model:

1. Go to Collections > Sync with Dashboard.
2. Click Commit and Close to finalize the sync process.
3. Open the Akselos Portal to verify that the model data has been successfully uploaded and is ready for solving.

Submit solve command

After confirming that the model data has been synced to the cloud, users can proceed to submit a solve.

How to Submit a Solve:

1. Go to the Solutions tab in Akselos Modeler.
2. Click Solve to send the job to the cloud solver.

Figure 3.24. solutions ribbon > solve

Depending on the mesh size and model complexity, the solving process may take anywhere from 5 minutes to over an hour. Once completed, the solution will automatically download and appear in the graphic window for visualization.

Users can track progress through:

• The Solutions Panel in Akselos Modeler
• The Jobs Page within the model’s collection on the Akselos Portal

Multiple Solve Submissions:

The platform supports submitting multiple solves simultaneously. To avoid data conflicts during this process, follow these best practices:

Figure 3.25. file > save as

Note: It is not recommended to modify and sync a model data while it is being solved to avoid data conflict on the Cloud.

When working with multiple models:

• Create and save each model with a distinct name:
  • Model 1 → Save as "1.aks"
  • Model 2 → Save as "2.aks"
• Go to Collections and sync both models to the Dashboard.
• Reopen each model individually and submit solves in sequence.

3.4.2. Analysis Results

Viewing and Interpreting the Solution

Once the solution is complete, results for each load step, from Step 0 to the final predefined step, are available in the Solutions tab. Users can select any step to examine the model's behavior during the tightening, operation, and hot bolting phases.

In the graphic window, the Solution Field dropdown provides several categories of results for visualization, including:

• Contact Data: information related to interface behavior such as pressure, gap, slip, and shear
• Displacement Fields: deformation values in the x, y, and z directions
• Gasket Behavior: closure and pressure response across the gasket
• Stress Fields: normal and shear stress components, including Von Mises
• Thermal Field: temperature distribution throughout the model

Save solution

After completing a simulation, users can save the solution for sharing, documentation, or future examination. The saved solution will be stored as a .asl file, which can be reopened at any time within Akselos Modeler.

How to Save a Solution:

1. In the Solution Ribbon, right-click on the desired solution scenario.
2. Select Save As.
3. Enter a name for the solution file.
4. Click Save.

The saved .asl file can be shared with collaborators or reloaded for review without needing to re-run the simulation.

Open a shared solution

A previously saved solution can be shared between users or reopened for further analysis. To do so, ensure that the related model and collection are properly set up on your local machine.

Steps to Reopen a Saved Solution (.asl):

1. Confirm that the corresponding collection is available locally.

   For example, to open Model_A.asl (saved solution) from the SPMFF_Ver1 collection, you must first import the collection SPMFF_Ver1 into your working directory using the SPM for Flanges software.

2. Go to File > Open File.
3. Locate and select the .asl file you want to open.
4. Once opened, the solution will load in the Solution tab for review, without requiring the model to be re-solved.

3.5. Assessment metrics

3.5.1. Results tab overview

The Results tab is designed to extract, compute, and present the necessary parameters for evaluating the condition of the gasket, bolts, and flange at each step in a selected load scenario. Users can choose to analyze either All Components at once or review each component Bolt, Gasket, or Flange in detail using the dedicated views that follow.

Figure 3.26. spm for flanges > results tab

When selecting All Components, the interface highlights the most important indicators from all three component types, providing a quick overview of joint integrity at the chosen step:

• Average Gasket Compressive Pressure: Displayed with a risk matrix, showing the minimum gasket pressure value and its associated severity level.
• Bolt Stress vs. Yield Strength: Identifies bolts exceeding allowable stress limits, showing the maximum bolt stress and its location.
• Flange Rotation: Shows the maximum flange rotation, compared to a limit (typically 1 degree), with a supporting chart for evaluation.

To generate results, users must first select a load step and then click Compute [Component] Results. The summary will include numerical values, severity classifications, and graphical comparisons such as line and polar plots.

Note: Users can also use the Results tab to perform evaluations on a shared solution, even if they did not generate the model themselves. See Section 3.4.2 for instructions on how to open and assess a shared .asl file.

For more detailed insights into individual components, users can switch to the next result sections for Gasket, Bolt, and Flange.

3.5.2. Gasket Performance Evaluation assessment

Risk Matrix

The Gasket Risk Matrix in the SMP for Flanges tool is a visual assessment framework used to evaluate sealing reliability based on gasket compressive stress. It helps engineers identify the likelihood and consequence of gasket failure during different stages such as assembly, operation, and hot bolting. By presenting this information in a structured format, the matrix supports safer decision-making and highlights areas that require further attention.

Figure 3.27. Risk Matrix Assessment Mechanism

The Risk Matrix is built upon stress results extracted from FEA simulations. It tracks compressive stress acting on the gasket at key steps in the load sequence and compares it to three threshold values: the minimum required stress for sealing during assembly, the minimum stress needed to prevent leakage during operation, and the maximum allowable stress to avoid permanent damage. These thresholds are based on ASME PCC-1 guidelines or manufacturer data. At each stage, the tool extracts stress values across the gasket width and determines the average. This average stress is then categorized into risk levels using a color-coded matrix. The matrix also considers the severity of potential failure, from minor leakage to severe safety risks. In future versions, the criteria used in the Risk Matrix will be configurable, allowing users to adjust threshold values based on their own company standards or internal engineering guidelines. This flexibility will enable more tailored assessments that align with project-specific requirements or operational practices. 

To generate the chart for a specific step:

1. Select the desired Child Solution (i.e., load step)
2. Click Compute Gasket Risk Matrix 

3.5.3. Bolt Stress & Relaxation Monitoring assessment

Polar chart comparison: Stress vs. Yield strength

The Bolt Stress Evaluation feature is designed to verify that bolts in the flange joint are operating within safe stress limits, ensuring reliable structural performance under loading. This assessment supports compliance with industry standards such as ASME BPVC Section VIII, Division 2 (2019) and ASME PCC-1 (2019). It provides both a numerical and visual overview of bolt stress behavior, helping engineers detect overstressed bolts and maintain the safety and functionality of the joint during tightening, operation, or hot bolting procedures.

Figure 3.28. bolt stress Assessment Mechanism

The evaluation begins by extracting bolt stress results from the solved FEA model. For each bolt, the tool calculates both the maximum and average Von Mises stress across its cross-section. These values are then checked against standard limits: the maximum stress should not exceed twice the allowable stress from ASME BPVC.VIII.2, and the average stress must stay below the bolt’s yield strength according to ASME PCC-1. Any overstressed bolts are flagged, and a visual comparison chart is generated for all bolts in the model.

This chart includes the following metrics for each bolt, extracted from the middle surface of the bolt body:

• Max Bolt Stress: the highest localized stress value on the evaluated surface
• Average Bolt Stress: the average stress across the entire mid-surface of the bolt
• Yield Strength: obtained from the assigned bolt material in the Material tab, based on temperature-dependent or independent properties

To generate the chart for a specific step:

1. Navigate to the Result tab.
2. In the Component dropdown, select Bolt, in the Results dropdown, select Bolt Stress.
3. On the left panel under the Solution section, choose a child solution.
4. Click Compute Bolt Stress Data to generate the chart.

This chart enables users to clearly identify bolts exceeding material limits, compare stress distribution across the joint, and assess bolt performance under operational or hot bolting conditions.

3.5.4. Flange Stress & Deformation Analysis assessment

Flange rotation

This assessment ensures that flange rotation remains within acceptable limits to prevent gasket leakage, loss of bolt preload, and structural failure. 

Flange rotation is primarily evaluated by calculating the flange moment under operating and gasket seating conditions and comparing it to permissible rotation limits based on gasket type. From the analysis results, flange displacements are extracted and used to calculate the flange rotation, which is compared against a default limit value.

Flange rotation limits vary based on flange type, size, gasket material, and design pressure. From ASME PCC-1–2019 provides recommended limits based on gasket material:

The mechanism works by evaluating displacement vectors on the flange surface and computing the angular deviation of each point relative to its original position. The tool scans around the flange to identify the location with the highest rotation angle. This maximum value is then displayed on a chart alongside the allowable limit, giving users a clear and visual comparison to assess whether flange deformation remains within acceptable bounds.

Figure 3.29. flange rotation Assessment Mechanism

To generate the chart for a specific step:

1. Navigate to the Result tab.
2. Under Component, select Flange. In Results, choose Flange Rotation.
3. Select the appropriate simulation step (e.g., Remove one bolt).
4. Click Load Flange Rotation Chart Data.

Figure 3.30. cOMPUTE flange rotation

Stress Classification Lines (SCL) results

The SCL (Stress Classification Line) Result Assessment is designed based on Section 5.2 – Protection Against Plastic Collapse of ASME BPVC.VIII.2-2019. To evaluate protection against plastic collapse, the results from an elastic stress analysis of the component under defined loading conditions are categorized and compared to associated limiting values.

Figure 3.31. stress classification line (scl)

Figure 3.32. scl Assessment Mechanism

The Stress Classification Line (SCL) evaluation begins by extracting stress tensor results from the flange using the solved FEA model. Based on these results, users define specific SCL paths at selected flange locations for detailed stress analysis. The tool then performs stress linearization along these paths, separating the membrane and bending stress components at each load step. Finally, the extracted values are compared against ASME-defined allowable stress limits to verify structural compliance and prevent the risk of plastic collapse.

To generate the chart for a specific step:

Figure 3.33. cOMPUTE scl RESULTS

1. Navigate to the Result tab.
2. In the Component dropdown, select Flange. In the Results dropdown, select SCL Result.
3. On the left panel under Solution, choose the desired load step (e.g., Remove one bolt).
4. Click Load Flange SCL Chart Data to generate the chart and result tables.
5. (Optional) Use the Slice Angle input or scan tool to locate the slice with the maximum SCL result. This helps identify the most critical stress path on the flange cross-section for further evaluation.

4. Conclusion and Support

Thank you for using the SPM for Flanges User Manual. We hope this guide has provided clear instructions and helpful context for setting up, solving, and assessing your flange joint models with confidence. If you encounter any issues or have additional questions, please don’t hesitate to reach out to our support team at [email protected]. We are here to assist you in ensuring a smooth and accurate simulation experience. For updates, training resources, or to provide feedback, please visit the Akselos Portal or contact your account representative directly.