Introduction

This tutorial shows how to create a simple 2D square mesh in Gmsh with some physical groups and then use the MoFEM tool read_med to generate a MoFEM-compatible input mesh for analysis.

The steps will be as follows:

Create geometry, physical group and mesh in Gmsh
Create a seperate config file to add attributes to blocksets (physical group)
Use read_med to generate a MoFEM-compatible input mesh

The data presented in this tutorial can be found at the directory /mofem_install/mofem-cephas/mofem/users_modules/tutorials/msh-1

Geometry and physical group

Among a number of tutorials on Youtube regarding Gmsh, a tutorial presenting how to create a 2D mesh can be found here. This is a good starting point.

Geometry

In order to create a geometry of a square, from the panel on the left, choose Modules -> Geometry -> Elementary entities -> Add -> Rectangle. Then provide the geometry inputs including location (X, Y, Z) and dimensions (DX, DY) as shown in Figure 1 and click Add and then press q on the keyboard to finish.

Figure 1: Input location (X, Y, Z) and dimensions (DX, DY) for the square.

Note: Other tools in Modules -> Geometry -> Elementary entities -> Add can be used to create wide variaty of 2D geometries. For example, points and lines can be used to create a L-shape surface.

Physical group

Physical groups are used to define groups of entities that later will be given attributes including inputs of names, material properties, loading conditions, contrainsts, etc. These attributes will be read by MoFEM during analysis.

As a demonstration, in this part, physical groups of edges and surface of the 2D square will be defined as shown in Figure 2 and Figure 3. It can be done by choosing, from the left panel, Modules -> Geometry -> Physical groups -> Add -> Surface/Curve. Then give name of a physical groups in the box Name, select entities to add to the corresponding groups and finally press e to end the selection.

Figure 2: Define physical group of the surface.

Figure 3: Define physical group of curves (edges) for boundary definition.

Mesh generation

Create the mesh

Go to Tools -> Options -> Mesh, in the General tab, choose the meshing algorithms and change the element size factor, e.g. 0.5 as shown in Figure 4, then close the window. To create the 2D mesh for the square, on the left panel, choose Modules -> Mesh -> 2D.

Figure 4: Mesh generation.

Export mesh in MED format

A preferred mesh format that will be exported is MED. This can be done by go to File -> Export ... then choose the file type Mesh - MED (*.med) and give a file name, e.g. square.med

MoFEM-compatible input mesh

The mesh created by Gmsh in the previous step is not immediately compatible in a MoFEM analysis. We would need to provide additional information to the defined physical groups (blocksets) and convert the mesh to *.h5m format. We can do it by the following steps

Create a config file to add information (block name, material properties, boundary conditions, loadings) to the defined physical groups (blocksets)
Generate MoFEM-compatible input mesh in *.h5m format using read_med tool

Create config file

As mentioned above, the mesh created by Gmsh does not contains attributes that may be needed for some tasks for analysis in MoFEM, e.g. blockset with a specific name to add material properties, boundary conditions, loadings. We need to know the exact ID of the physical group (blockset) in the MED file in order to add attributes to that blockset, we can check the IDs by running the read_med as follows

read_med -med_file square.med

which would show that the defined physical groups square and boundary have the ID of 1 and 2, respectively, as in the following output message

[0] <inform> MoFEM version 0.11.0 (MOAB 5.2.1 Petsc Release Version 3.11.4, Sep, 28, 2019 )
[0] <inform> git commit id 0ac8895b15c4ad41ea5e7077c4d011f7efb50f13
[0] <inform> [MedInterface] Reading MED file V4.1.0 using MED library V4.1.0
[0] <inform> [MedInterface] Check mesh square nsteps 1
[0] <inform> [MedInterface] Reading mesh square nsteps 1
[0] <inform> [MedInterface] Read number of nodes 107
[0] <inform> [read_med] Print all meshsets (old and added from meshsets configurational file
[0] <inform> [read_med] meshset 12682136550675316737 type BLOCKSET UNKNOWNNAME msId 1 name square
[0] <inform> [read_med] meshset 12682136550675316738 type BLOCKSET UNKNOWNNAME msId 2 name boundary 

We would then use these IDs in the config file, named square.config, as below

[block_1]
# `square` block - Add isotropic elastic material properties
id=100
add=BLOCKSET
name=MAT_ELASTIC
young=1
poisson=0.1
 
[block_2]
# `boundary` block - Add block and give it a specific name
id=110
add=BLOCKSET
name=BOUNDARY_CONDITION

where [block_1] and [block_2] use the blockset IDs in the MED mesh which cannot be changed. Meanwhile, id=100 and id=110 are the IDs, specified by user at this step, of the new blocksets that will be created in the next step. The remaining of each block are the attributes that will be added, e.g. material properties or even just a blockset with a specific name that will be used in some MoFEM program.

Generate MoFEM-compatible mesh

Once the MED file and config file are ready, the final mesh file in *.h5m format that contains necessary information and can read by MoFEM can be generated by running the command below

read_med -med_file square.med -meshsets_config square.config -output_file square.h5m

After running this command, the square.h5m file will be created and the main part of the output message would look like this

[0] <inform> [read_med] Print all meshsets (old and added from meshsets configurational file
[0] <inform> [read_med] meshset 12682136550675316737 type BLOCKSET UNKNOWNNAME msId 1 name square
[0] <inform> [read_med] meshset 12682136550675316738 type BLOCKSET UNKNOWNNAME msId 2 name boundary                       
[0] <inform> [read_med] meshset 12682136550675316739 type BLOCKSET MAT_ELASTICSET msId 100 name MAT_ELASTIC
[0] <inform> [read_med] meshset 12682136550675316740 type BLOCKSET UNKNOWNNAME msId 110 name BOUNDARY_CONDITION

As can be seen, along with the original blocksets 1 and 2, the output mesh square.h5m now contains the two new blocksets 100 and 110 with the names MAT_ELASTICSET and BOUNDARY_CONDITION, respectively, with additional attributes. Using the same concept, more blocksets for different purposes can be added to the mesh.

Once the final square.h5m mesh is generated, it can be used directly as an input in MoFEM programs, e.g. SCL-1: Poisson's equation (homogeneous BC).

Table of Contents