The Thickness Mapping Tool is an Abaqus/CAE plugin that allows an user to map thickness data from Excel files to an Abaqus/CAE shell element model.
In the petrochemical refining, processing and nuclear industries routine scans performed on a section of a vessel can reveal loss of thickness due to various damage mechanisms. This thickness loss data, typically in a rectangular grid, is presented in Excel file format. As part of assessing a structure against codes such as API 579, reliability engineers have a need to map thickness data from scans onto finite element meshes. As part of a Level-3 Fitness-for-Service assessment of a pressure vessel with corroded thickness using a finite element model, the thickness loss must be adequately captured for an accurate representation of the model. For this purpose, the Thickness Mapping Tool was developed that allows users to map thickness data on to a shell element model. The mapping tool can be invoked through Abaqus/CAE and can be assessed in the Part and the Property modules.
Figure 1. Thickness mapping plugin.
The plugin has three sections A, B, & C as indicated in the figure below, that require user input. Section A requires input about the type of pressure vessel surface for which the data is available and mapping is to be performed. Two surface type options are available; Cylindrical Surface and Curved Surface. The Cylindrical Surface option is applicable for drum sections and shell sections whereas the Curved surface is applicable for head sections. The Curved surface is applicable for head sections with double curvatures.
In addition to selecting the type of surface, Section A requires input selection on the type of algorithm needed for mapping purposes. Two options, Linear and Nonlinear, respectively, are available. The Linear algorithm is generally applicable for spherical or flat surfaces. The Nonlinear algorithm is applicable for highly curved or doubly-curved surfaces, typically head sections. However, the algorithms can be switched along with partitioning the surfaces to achieve the desired mapping accuracy.
Figure 2. Section A of the plugin.
Section B of the plugin requires selecting the surface geometry in the finite element model for which mapping is to be performed. In addition, shell section definitions with the mapped thickness and a specific material definition can be created automatically. By checking the Create face set name option, a shell section can be assigned to the selected faces; the plugin lists the material definitions available in the model under the Material drop down menu. The Surface offset drop-down menu has three options TOP SURFACE, MIDDLE SURFACE, and BOTTOM SURFACE and is used to indicate the mesh surface location with respect to the shell thickness. For instance, MIDDLE_SURFACE would imply that the finite element mesh represents the middle surface of the structure.
Figure 3. Section B of the plugin.
For each of the surfaces, Point - A, Point - B, & Point - C can be picked from the vertices to define the surfaces. Point - O is a datum point on the axis of the vessel. If a datum point is not available, it can be created using Datum tools.
Figure 4. Points A, B, & C to be selected for the plugin.
Section C of the plugin requires thickness readings input from the Excel file. However, the assumption is that data in the Excel file is arranged in a rectangular grid analogous to how the
scan data was obtained. That is, the data must be arranged in the convention indicated in Figure 6.
Figure 5. Section C of the plugin.
Figure 6. Thickness data format in the Excel file for use with the plugin.
The figure below describes the different options needed for selecting the data from the Excel file. The mapping can be verified by performing a datacheck analysis and probing the shell thickness output variable STH using the Quilt option in the Contour Options. Note that the variable STH is not requested by default for output.
Figure 7. Plot of STH output on a surface.
Plugin Download
The attached zip file contains the Thickness Mapping Tool plugin for Abaqus CAE, built and intended for use with Abaqus CAE 6.14+. The zip file also contains installation instructions document and an usage guide with an illustrative example.
***NOTE:
BY DOWNLOADING THIS FILE (“DOWNLOAD”) YOU AGREE TO THE FOLLOWING TERMS:
THIS DOWNLOAD IS MADE AVAILABLE ON AN "AS IS" BASIS WITHOUT WARRANTY OF ANY KIND, WHETHER EXPRESS OR IMPLIED, ORAL OR WRITTEN, INCLUDING, WITHOUT LIMITATION, ANY IMPLIED WARRANTIES OF MERCHANTABILITY, FITNESS FOR A PARTICULAR PURPOSE, TITLE OR NON-INFRINGEMENT.
DASSAULT SYSTEMES SIMULIA CORP., ANY OF IT AFFILIATES (COLLECTIVELY “DS:”), AND ITS LICENSORS SHALL HAVE NO LIABILITY FOR DIRECT, INDIRECT, INCIDENTAL, CONSEQUENTIAL OR PUNITIVE DAMAGES, INCLUDING WITHOUT LIMITATION CLAIMS FOR LOST PROFITS, BUSINESS INTERRUPTION AND LOSS OF DATA, THAT IN ANY WAY RELATE TO THIS DOWNLOAD, WHETHER OR NOT DS HAS BEEN ADVISED OF THE POSSIBILITY OF SUCH DAMAGES AND NOTWITHSTANDING THE FAILURE OF THE ESSENTIAL PURPOSE OF ANY REMEDY.
YOUR USE OF THIS DOWNLOAD SHALL BE AT YOUR SOLE RISK. NO SUPPORT OF ANY KIND OF THE DOWNLOAD IS PROVIDED BY DS.
