1. Introduction

The AKSELOS Structural Performance Management (SPM) for Flanges tool is a specialized simulation tool that supports engineers in evaluating the structural behavior and sealing performance of bolted flange joints during hot bolting procedures, refers to the sequential loosening and retightening of bolts while the flange remains pressurized, which introduces complex interactions between gasket compression, bolt preload, and flange deformation.

In this article, is to guide users through the process of creating a complete flange joint model using the tool and performing a full integrity assessment based on a specific real-world use case. 

This article is part of a larger tutorial series designed to help users build confidence and proficiency in using the tool through practical, step-by-step examples:

1. SPM for Flanges - User Manual
2. Case study: Flange Tightening Sequence Optimization
3. Case study: Full Bolting vs. Partial Bolting Configurations 
4. Case study: Risk-Based Hot/Half Bolting Procedures

To help you better understand how the SPM for Flanges tool is used in practice, the following workflow outlines the full modeling and assessment process for this case study — from geometry input and load definition to results interpretation and performance evaluation of the gasket, bolts, and flange.

Figure 1.1. SPM for Flanges user journey

Note: This article is based on the SPM for Flanges tool – Version 2025.04. If you need assistance with installation or setup, please don’t hesitate to contact our support team.

2. Problem Statement and Objectives

Full Bolting vs. Partial Bolting Simulation of a Class 150 NPS 20 Flange Joint

This case study examines the structural behavior of a bolted flange joint where one bolt is intentionally left untightened. The joint is designed according to ASME B16.5 (2020) standards (Class 150, NPS 20) with a total of 20 bolts. Only 19 bolts are preloaded using a one-time tightening sequence. The internal pressure is then gradually increased in stages—50%, 80%, and 100%—to observe how the flange responds as it approaches normal operating conditions. The objective is to assess whether the joint can function safely under real-world pressure without all bolts fully engaged.

Figure 2.1. FLANGE WITH ONE INACCESSIBLE BOLT

Summary of Model Configuration

• Geometry: Flange assembly with 20 bolts, spiral wound gasket, and connected pipe/weld (included in flange body).
• Materials: SA-105 for flange/pipe/weld, SA-193 B7 for bolts, graphite-based spiral wound gasket.
• Boundary Conditions & Loads: One bolt untightened; remaining 19 tightened in a one-time sequence. No clamp or pipe-end loads. Internal pressure applied in 3 stages: 50%, 80%, and 100%.

Focus of This Case Study

The focus is on bolt stress evaluation under partial bolting conditions. Von Mises stress is assessed using post-processing tools, with particular attention to whether the remaining bolts can carry the load without exceeding material limits.

Figure 2.2. THE STRESS RESULT OF THE FLANGE

3. Before we start

Before diving into model creation, there are a few essential steps to ensure you have the proper setup and access required to work with the SPM for Flanges tool. Follow these steps carefully to avoid issues during the modeling and assessment process.

Step 1: Set Up Your Account and Access. You’ll need an Akselos account with appropriate access permissions to the correct location. This is necessary to download the tool, create new model collections, and manage your simulations. If you haven’t already, review the following articles:

• [Create Akselos Portal Account] – Required to access the platform and use the tool.
• [Akselos Portal for New Users] – Provides an overview of the platform’s features and interface.

Step 2: Install the Latest Akselos Modeler. Ensure you have the most up-to-date version of the Akselos Modeler installed. If you’re unsure or need help obtaining it, please contact Akselos support for assistance.

Step 3: Organize Your Working Folder. Efficient data management is key to a smooth workflow. Follow the best practices outlined in the article below to set up your simulation folders properly:

• [Working Folder and Data Management] – Recommendations for organizing files and managing simulation data on your local drive.

Step 4: Start with a New Model Collection. Once your environment is ready, you can begin building your model by creating a new collection and importing it for workspace preparation. Refer to:

• [Start Building Your Model with a New Collection] – Step-by-step instructions on how to set up and manage a new model collection in the portal.

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.

Bonus Track
As an additional resource, we’ve prepared a sample collection that demonstrates how the setup and simulation are structured within the Akselos environment. This example can serve as a helpful reference as you follow the tutorial or build your own model. You can access the sample collection here:

• Case Study 1: Full Bolting vs. Partial Bolting Configurations

4. Model Creation

Step 0: Preparation

Create a New Collection on Akselos Portal

On the Akselos Portal, a blank collection is the starting point for building any simulation model. A collection acts as a container for your project data and exists in two locations:

• Locally on your drive (where you build the model)
• On the cloud (where the solver engine runs)

These two are kept synchronized through a sync process (see Step 6).

To get started:

Step 1: Log in to the Akselos Portal (https://portal.akselos.com) using your account.

Step 2: Go to your workspace (e.g., your organization or team space like: https://portal.akselos.com/SPM_for_Flanges_Trial/<Your _Folder>).

Step 3: Click New Collection, enter a name (e.g., Case_study_1).

Note: Avoid using spaces in the name. Use underscores (_) instead to prevent errors.

FIGURE 4.1. CREATING NEW COLLECTION

Step 4: Wait for the collection to be successfully created.

Connect SPM for Flanges to the Cloud

To import collections, sync data, and submit simulation jobs, you need to connect your software to the cloud.

Step 1: In the SPM for Flanges software, go to the top left corner: Cloud ➔ Server Authentication.

FIGURE 4.2. OPENING THE SERVER AUTHENTICATION WINDOW

Step 2: In the authentication window, enter your Akselos username and password/token.

Step 3: Click Check and wait for the indicator light to turn green      

FIGURE 4.3. CHECKING THE STATUS OF SERVER CONNECTION

Common Connection Errors:

• Yellow light      : Internet connection issue
• Red light      : Incorrect username or password/token

Import the Collection into SPM for Flanges

Once connected to the cloud:

Step 1: Navigate to Collections ➔ Import Collection.

FIGURE 4.4. OPENING THE IMPORTING COLLECTION WINDOW

Step 2: In the pop-up window, locate your newly created collection (e.g., Case_study_1) and click Import Collection.

FIGURE 4.5. IMPORTING the collection to the local machine

Step 3: Wait for the import to finish. You’ll know it’s complete when the collection name appears in the title bar of the software interface.

FIGURE 4.6. The importing collection process notification

Download the Material Library

The material library is stored on the cloud and must be downloaded each time you launch the software (more details in Step 3).

Note: The material library requires special access permissions. If you’re unable to download it at this step, please contact our support team at [email protected] to request access. We’ll assist you in the shortest time possible.

Step 1: Geometry setup

This example demonstrates how to create a flange joint model based on ASME B16.5 (2020) with a Class 150 rating and a Nominal Pipe Size (NPS) of 20 inches. The resulting flange has an outer diameter of 698 mm and includes 12 bolts. This model does include the pipe and weld line.

FIGURE 4.7. SPM for flanges - define geometry

How to Input:

Step 1: In the Akselos Modeler, select Flange Hot Bolting Tool from the tool drop-down list.

Step 2: Navigate to the Geometry Tab.

Step 3: Input the following parameters:

• Standard: ASME B16.5
• Class: 150
• NPS: 20

Step 4: Select Include Pipe and Weld options.

Step 2: Define Materials

This flange joint model consists of five main components: the flange, bolt, gasket, pipe, and weld lines. Each part is assigned specific material properties to accurately represent typical industrial conditions. The flange, pipe, and welds are modeled using carbon steel forgings, following the ASTM SA 105 specification with UNS designation K03504. The bolts are defined using ASTM SA 193 Grade B7 alloy steel, which is suitable for high-temperature and high-pressure environments. The gasket is modeled as a spiral wound type from the graphite group, chosen for its ability to maintain sealing performance under elevated temperatures and in contact with process fluids.

FIGURE 4.8. SPM for flanges - download material database

To input material data in the Akselos Modeler:

Step 1: Navigate to the Material tab

Step 2: Download Material Library

• Go to the Material tab.
• Download the full materials library.
• Once the download is complete, the Define button will become available.

Note: Access to the material library requires permission. If you are unable to download it at this step, please contact our support team at [email protected] to request access. We’ll assist you in the shortest time possible so you can continue your setup without interruption.

Step 3: Assign Material to Pipe, Weld, and Flange.

FIGURE 4.9. SPM for flanges - define and assign material to pipe, weld, and flange

• Click Define and enter the following:
  • Behaviour: Elasticity Materials
  • Product Form: Forgings
  • Spec. No: SA-105
  • Type/Grade: undefined
  • Alloy desig./UNS No: K03504
  • Class/Cond./Temper: undefined
• Click Apply to save.

Step 4: Assign Material to Bolt.

FIGURE 4.10. SPM for flanges - define and assign material to bolt

• Behaviour: Elasticity Materials
• Product Form: Bolting
• Spec. No: SA-193
• Type/Grade: B7
• Alloy desig./UNS No: G41400
• Class/Cond./Temper: undefined

Step 5: Assign Material to Gasket.

FIGURE 4.11. SPM for flanges - define and assign material to gasket

• Behaviour: Gasket Material
  • Material Group: Graphite
  • Name: Spiral Wound Gasket

FIGURE 4.12. SPM for flanges - materials assigned to parts

You can view detailed material properties such as thermal expansion or Young’s modulus by clicking the information button in the material library window. The corresponding values will be automatically shown in the table and chart panel.

Step 3: Defining Loads and Boundary Conditions

In this simulation model, only internal pressure is applied, specifically on the inner surfaces of the flanges and pipe. There is no pipe load or clamp load considered in this setup. Bolt torque is not applied directly; instead, it is converted into pretension load on the bolts based on the given torque value. Contact interactions are defined at the flange–gasket and bolt–flange interfaces to accurately simulate the physical behavior during operation.

FIGURE 4.13. SPM for flanges - set up boundary conditions

To input the simulation conditions:

Step 1: Set Internal Pressure

• Apply 3 MPa on the inner surfaces of the flanges and pipe only.

Step 2: Set Temperatures

• Environment temperature: 22°C
• Assembly temperature: 22°C
• Operating temperature: 100°C

Step 3: Set Bolt Torque

• Torque: 800 Nm
• Nut factor (torque coefficient): 0.16

Step 4: Set Contact Condition. Leave general contact settings as default.

• Flange–Gasket contact: Frictional
• Bolt–Flange contact: Bonded

Note: In this case, pipe loads and clamp loads are excluded to isolate the effect of pressure and bolt pretension.

Step 4: Load Sequence Setup

As mentioned earlier, this flange follows ASME B16.5 Class 150 with a Nominal Pipe Size (NPS) of 20, which means the model includes a total of 20 bolts. However, in this scenario, one of the bolts is located in a position where it cannot be tightened. The remaining 19 bolts will be tightened using a one-time tightening sequence. After that, internal pressure will be gradually increased in steps to observe how the model behaves under operational conditions.

FIGURE 4.14. SPM for flanges - set up load sequence

To set this up:

Step 1: Define the Untightenable Bolt

• Select Bolt 1 as the untightened bolt in the load sequence setup.

Step 2: Tightening for the Remaining Bolts

• Set the tightening option for the remaining 19 bolts to One Time Pattern.
• Set the Bolt Relaxation Factor to 0.16 (representing 16% relaxation of bolt pretension after assembly).

Step 3: Gradual Increase of Internal Pressure

• You will simulate the increase in internal pressure in three stages: 50%, 80%, and 100% of the design pressure.
• To do this, create additional steps in the load sequence:

• Hit Add Row to create Step 5 and Step 6.
• In Steps 4 to 6, set the Piping Load Factor and Clamping Load Factor to 0 (to keep them inactive).
• Adjust the Internal Pressure Factor for each step as follows:
  1. Step 4: 0.5
  2. Step 5: 0.8
  3. Step 6: 1.0

Optional: Users may choose to label each step as 50%, 80%, and 100% to help clearly identify and distinguish the results during post-processing.

Step 4: Hot Bolting Not Included

FIGURE 4.15. SPM for flanges - remove the hot bolting step

• This case does not include hot bolting, so you can remove Step 7 (if auto-generated).
• To do this, select Step 7 and click Remove Row.

Step 5: Final Check

• Review the setup using the Load Sequence Summary Table to ensure all steps and values are correctly defined.

FIGURE 4.16. SPM for flanges - check the load sequence summary table

Step 5: Automatic model creation

Once all input parameters are completed, users should review all settings before clicking Create Model. The software will then automatically generate a fully configured model, eliminating the need to manually go through the CAD and meshing stages.

After the model is created, users can review all predefined settings directly in the Model Structure Tree under the Model Ribbon. This is a good opportunity to confirm that all setup parameters have been correctly applied before proceeding.

FIGURE 4.17. Model created from the Spm for flanges tool

Final Checks After Model Creation:

Check Created Components

• There will be three main components in the model: Flange, Bolt, and Gasket.
• The Pipe and Weld are considered part of the Flange component.

Check Materials

• Go to Components, then select a component (e.g., Bolts).
• Under Subdomain, choose the specific part you want to inspect.
• Material details will be shown in the property panel below.

Check Boundary Conditions

• Constraints: Navigate to Boundary Conditions > Geometry Constraints. Selecting a constraint will highlight its location in the model.
• Contact Settings: Go to Contact Interactions, then click a contact surface to view its type and assigned settings.

Check Loads

• In the Load Cases section, use the drop-down menu to browse through all defined loads.
• Although the tool may automatically create multiple load cases (typically five), in this tutorial, you only need to focus on the internal pressure case.

5. Analysis Results & Assessment Metrics

Step 6: Data synchronization

Once the model is fully created and all settings have been verified, the next step is to save the model and sync it to the cloud, where the Akselos solver engine operates. This step is essential for ensuring that the solver has access to the complete model data. After the solve, results will be automatically sent back to the SPM for Flanges software for visualization and further examination.

Saving the Model

The simulation model will be saved within the aks_files folder, with the format of *.aks: Partial_bolting.aks for example.

To save the file: Go to File > Save, or press Ctrl + S

Important: Do not use spaces in the file name, as this may cause errors. Instead, use underscores (_).
Example: model_name.aks

Syncing the Model to the Cloud

Step 1: Go to Collections ➔ Sync with Portal.

Step 2: Click Commit and Close to complete the sync process.

Step 3: Log in to the Akselos Portal and open your collection to verify that the model has been uploaded successfully and is ready for solving.

Submit solve

Step 1: Navigate to Solution ribbon

Step 2: Click Solve to send the job to the cloud solver.

FIGURE 4.18. Solving model

This model is relatively detailed, with nearly three million degrees of freedom (DOFs), so the simulation may take approximately 30 minutes to complete. Once finished, the solution will automatically download and display in the graphics window for visualization.

Progress can be monitored in the Solutions Panel, where each child solution is labeled according to the steps defined in the Load Sequence tab:

1. Tightening: One Time – Pre-load
   
2. Tightening: One Time – Relaxation
   
3. Tightening: One Time – Lock
   
4. 50% Pressure
   
5. 80% Pressure
   
6. 100% Pressure

These pressure steps are particularly important for evaluating bolt stress behavior under operational conditions.

Step 7: Bolt Stress & Relaxation Monitoring Assessment

In this assessment, the focus is on bolt stress, particularly to evaluate whether the flange joint can operate under normal conditions despite having one untightened bolt.

FIGURE 4.19. Checking the von Mises stress result of the model

Checking Von Mises Stress of the Bolts

To examine the stress distribution:

Step 1: Go to the Solution Fields tab.

Step 2: Select Von Mises as the result type.

Step 3: Change selection mode to subdomain, right-click on the bolt component,  and choose Isolate to clearly view stress distribution across the bolts

FIGURE 4.20. Isolating the selected subdomains/components

Using the SPM for Flanges Tool - Results tab

This tool calculates bolt stress based on data extracted from the middle surface of each bolt, providing both average and maximum stress values. These values are compared with the yield strength and visualized on a polar chart.

FIGURE 4.21. SPM for flanges - the bolt stress

Steps to check bolt stress:

Step 1: Navigate to the Result tab.

Step 2: In the Component dropdown, select Bolt, in the Results dropdown, select Bolt Stress.

Step 3: On the left panel under the Solution section, choose a child solution (e.g., Step 4: 50% Pressure).

Step 4: Click Compute Bolt Stress Data to generate the chart.

Below are the polar charts corresponding to the assembly phase and the three internal pressure levels (50%, 80%, and 100%) during operation. These visuals help assess how the load is distributed among the bolts and whether any bolt exceeds the material’s yield strength.

FIGURE 4.21. SPM for flanges - the bolt stress of step 1, 2, 3

FIGURE 4.22. SPM for flanges - the bolt stress of step 4, 5, 6

As the charts indicate, during the Pre-Load step of the assembly phase, eight bolts exhibit high stress levels, suggesting that they are carrying a larger share of the preload. Once relaxation occurs, the stress levels decrease below the yielding threshold. During the pressure loading steps no bolts exceed the yield strength in either maximum and average stress. 

FIGURE 4.22. SPM for flanges - the bolt stress of step 4, 5, 6

This observation leads to the following considerations for improvement:

• Reduce bolt pretension load: Lowering the applied torque could help balance load distribution more evenly across all bolts

• Consider changing bolt materials: Using bolts with higher yield strength or more favorable elastic properties may help accommodate higher pretension without exceeding stress limits.

• Switch to a multi-stage tightening sequence: While this case used a one-time tightening method, adopting a staged approach (e.g., cross-pattern with multiple torque rounds) could lead to a more even stress distribution in real-world applications.
  

These insights are useful for refining both assembly strategy and operational load planning.

6. Conclusion

This tutorial demonstrated how to build and assess a flange joint model with partial bolting using the SPM for Flanges tool in Akselos. By simulating one untightened bolt and gradually increasing internal pressure, users can evaluate whether the joint remains safe under typical operating conditions. The analysis showed that while no bolts exceeded the yield limit during operation, some carried excessive load during assembly, highlighting opportunities to optimize bolt pretension. This case reinforces the importance of load distribution checks in bolted joint design and validates the tool’s effectiveness for practical integrity assessments.

Disclaimer:
These tutorials are intended for instructional purposes only, to help users understand how the FHB tool operates within the SPM for Flanges software. The models and results presented here are not based on any real-world flange assemblies, and should not be used as the basis for evaluating or validating any actual engineering designs.
All input parameters used to create and simulate the model are conceptual examples. Users are responsible for independently verifying and validating all input data and ensuring its suitability for their specific use cases or engineering assessments.