6. D modeling#
6.1. Workflow of the TP#
The aim is to perform the elastic simulation without meshing the hole, using the X- FEM method.
To do this, we use the concept of interface (delimiting the hole), an interface being seen as an « infinite » crack (no crack front). The interface is then represented by a single Level Set (Normal Level Set), separating two solids, without contact on the interface. A hole (empty) is thus modelled because the solid inside is isolated from the rest of the structure on which the pressure load is applied.
The geometry and the mesh and the AsterStudy command file will be generated using the Salome-Meca platform.
Modeling is C_PLAN elastic. A quarter of the plate is modelled.
6.1.1. Geometry#
The geometry is the top right quarter of the rectangular plate, with no holes.
Start the Geometry module.
The main steps to build this geometry are as follows:
To create the face, you can, for example, use the « rectangle » tool (Menu New Entity/Primitives/Rectangle), then possibly translate it (Menu Operations/Transformation/Translation).
Build the edge groups on which the boundary conditions (symmetries and loading) will be based (Menu New Entity →Group →Create Group). Select the type of geometric entity (here the line, edge) and select the edge directly in the graphics window. Then click on Add. An object number should then appear. You can change the name of the group before validating it by Apply. Thus, build the 3 edge groups useful for the calculation: left for edge \(\mathit{AG}\), top for edge \(\mathit{GF}\) and bottom for edge \(\mathit{BD}\).
6.1.2. Meshing#
A plane mesh of the upper right quarter of the plate will be created, in elements of order 2, to have sufficient precision.
Start the Mesh module.
The main steps to generate the mesh are as follows:
Build the mesh (Menu Mesh → Create Mesh). Select the geometry to be meshed, then the algorithm NETGEN 1D - 2Davecl “hypothesis NETGEN 2D Parameters. In this case, select Fineness → Fine and check the Second Order box.
Calculate the mesh (Mesh → Compute menu).
Create the mesh groups corresponding to the geometric groups (Menu Mesh → Create Groups from Geometry). Select all geometric groups. 3 groups of edges are obtained on the mesh.
Export the mesh in MED format.
6.2. Creation and launch of the calculation case (via asterStudy)#
Start the AsterStudy module.
Then in the left column, click on the Case View tab.
The command file for the calculation case is defined.
Note: To add orders: Commands menu → Show All.
The main steps for creating and launching the calculation case are as follows:
Read the mesh in MED format: Command LIRE_MAILLAGE.
Orient the mesh to the edge affected by the load: Command MODI_MAILLAGE/ORIE_PEAU_2Den using the top group.
Define the finite elements used: Command AFFE_MODELE for 2D plane stress modeling (C_PLAN).
Define the interface: DEFI_FISS_XFEM with the crack shape (FORM_FISS/ELLIPSE) and the type of discontinuity.
Create rich finite elements (MODI_MODELE_XFEM). And name a new model name X - FEM.
Define material: Command DEFI_MATERIAU.
Assign material: Order AFFE_MATERIAU on model X- FEM.
Affect mechanical boundary conditions and loading: AFFE_CHAR_MECA on the X- FEM model:
for traction: FORCE_CONTOUR.
Solve the linear static mechanical problem: Command MECA_STATIQUE on the X- FEM model.
Create the mesh: Command POST_MAIL_XFEM. And name a new name for the mesh.
Define the finite elements used: Command AFFE_MODELE for 2D plane stress modeling (C_PLAN). And name a new model name.
Create visualization result: Command POST_CHAM_XFEM. And name a new name for the result.
Calculate field: Command CALC_CHAMP.
We will enrich the concept resulting from POST_CHAM_XFEM by using the same concept name.
for calculating the field of equivalent constraints by elements at the nodes: CRITERES/SIEQ_ELNO.
for calculating the field of equivalent stresses by elements at Gauss points: CRITERES/SIEQ_ELGA.
Print calculation results in format MED: Command IMPR_RESU.
To launch the calculation case, in the left column, click on the History View tab.
Note:
The rigid modes of the hole are blocked by the symmetry conditions applied. In the case of modeling the entire plate, it would have been necessary to block the rigid modes of the plate and also those of the hole.
6.3. Post-processing of results#
Start the ParAvis module.
The deformation of the plate and then the stresses at the edge of the hole will be visualized by comparing with the reference solution.
Import the results file (Data Files tab → Open in ParAvis with the generateVectors option).
Visualize the deformation of the plate (Menu Filters → Common → Warp By Vector).
It is possible to add an automatic mesh refinement step to improve the precision of the results.
Note:
The rigid modes of the hole are blocked by the symmetry conditions applied. In the case of modeling the entire plate, it would have been necessary to block the rigid modes of the plate and also those of the hole.
6.4. Tested sizes and results#
Value of the stress components at points A and B:
To do this, we calculate field SIGM_NOEU. Attention, the concept of SIGM_NOEU is particular for X- FEM because the elements generated for visualization (by POST_CHAM_XFEM) have double nodes that are not connected. So we have several values for a node position. In the present case, we have two nodes located at point A (plate side) and two nodes located at point B (plate side). So we test the min and the max for each point.
Location |
Identification |
Reference (Analytics) |
Tolerance |
Knot \(A\) |
Constraint \(\mathit{SIXX}\) |
-100.0 |
|
Node \(B\) |
Constraint \(\mathit{SIYY}\) |
303.0 |
|
These tests on analytical values are supplemented by non-regression tests.