3. Modeling A#
3.1. TP implementation#
3.1.1. Geometry#
3.1.2. Read the entire statement carefully before you start#
The geometry is created with the Salome-Meca platform, Geometry module.
The « Sketcher » tool (New Entity Menu → Basic → 2D Sketch) allows you to build the outline of the upper disk: \(A2\), \(B2\), \(D2\) and \(C2\). The arc of the circle is done in 2 times so that the point \(D2\) is created during the construction of the outline. For \(B2D2\), we give the radius to 50 and angle to -45° using Direction and Perpendicular, and for \(D2C2\), we give the radius to -50 and angle to 45° using Direction and Tangent.
You can then build a face from this outline (New Entity Menu → Build → Face).
By symmetry, we can generate the second sphere (Menu Operations → Transformation → Mirror Image) by choosing the X axis to achieve the symmetry.
It remains to assemble the two spheres to form a single object GEOM (Menu New Entity → Build → Compound ). Warning: In this object, there are always two points, \(\mathit{C1}\) and \(\mathit{C2}\), that overlap. On the contrary, the two points merge if the operation is Partition,
Finally, groups must be created on this geometry (with the names suggested in the figure above) (Menu New Entity → Group → Create Group). Attention should be drawn to the fact that the groups are created last.
Create groups for the surfaces of hemispheres \(\mathit{SPHHAU}\) and \(\mathit{SPHBAS}\)
In order to create groups for the superimposed points \(C1\) and \(C2\), we use the functionality to select a sub-element of an entity GEOM: check « Only Sub-shapes of the Second Shape », then for \(\mathit{C2}\) for example, select as « Second Shape » the upper hemisphere in the object tree as « Second Shape » the upper hemisphere in the object tree, and only its points are underlined.
Create groups for applying boundary conditions: along the axisymmetry axis (\(\mathit{A1A2}\)) and on the parts of the upper and lower hemispheres (\(\mathit{A1B1}\) and \(\mathit{A2B2}\)).
For contact modeling, you will need groups of cells representing potential contact surfaces: create groups \(\mathit{CONT}1\) and \(\mathit{CONT}2\).
3.1.3. Meshing#
We use the Mesh module. The mesh is defined by the menu Mesh→ Create Mesh with the geometry to be meshed. The meshing will be carried out in triangles, and the automatic meshing hypotheses « Assign a set of hypotheses → 2D: Automatic Triangulation » will be used, and a maximum length of 2mm will be used.
We calculate the mesh (Menumesh → Compute). A mesh containing approximately 3000 triangles and 1500 knots is then obtained.
We will then import the groups from the geometry (Menu Mesh → Create Groups from Geometry).
The mesh will be imported in MED format.
Illustration 3.1: Mesh obtained for modeling A
3.1.4. Command file#
We use the AsterStudy module. Then in the left column, click on the Case View tab.
The command file for the calculation case is defined. (right click on CurrentCase and choose Add Stage).
Note: To add orders: Commands menu → Show All.
By using command STAT_NON_LINE, build the command file for the test case by not taking the contact into account at first.
What can we see about convergence? What would it take to converge?
Index: how is the convergence criterion by default constructed?
Help to build the command file:
Define material: Command DEFI_MATERIAU.
Assign material to all elements: Command AFFE_MATERIAU.
Define the finite elements used: Command AFFE_MODELE to affect the MECANIQUE phenomenon and the AXIS modeling.
Affect boundary conditions/mechanical loads: AFFE_CHAR_MECA/DDL_IMPO for axial symmetry and unit imposed displacements that will then be multiplied by a ramp function over time.
Define the loading ramp (imposed displacement) with the DEFI_FONCTION command. For example, the function varies between \((\mathrm{0.,}0.)\) and \((\mathrm{2.,}2.)\).
Create time discretization using commands DEFI_LIST_REEL. For example, 20 steps from 0s to 2s.
Resolve the problem with command STAT_NON_LINE. We put COMPORTEMENT/RELATION =” ELAS “, the list of times defined previously in INCREMENT, the materials in CHAM_MATER, MODELEetégalement the boundary conditions and the loading (CHARGE + FONC_MULT) in EXCIT.
Bonus question: how many rigid body movements are there in axisymmetric modeling?
Reminder: a rigid body movement is a movement with zero deformation.
Add the contact definition: orient the surfaces, define the contact load with the DEFI_CONTACT command and adapt the nonlinear solver options.
An alarm appears when calculating with contact. We will keep the contact method by default at first ( FORMULATION =” DISCRETE “and” ALGO_CONT =” CONTRAINTE “) .
Define contact: Command DEFI_CONTACT. We will keep the contact method by default at first (FORMULATION =” DISCRETE “and” ALGO_CONT =” CONTRAINTE “). Groups CONT1 and CONT2 are assigned to the pair of contact zones (master and slave).
Adapt the contact option in STAT_NON_LINE.
3.1.5. Hertz pressure#
Numerical application: calculate by hand with the problem data, the value of the Hertz pressure and the contact half-width (see chapter 2). Compare them to the values obtained by the calculation.
What are we seeing? Why this discrepancy?
Note: we will take as a first approximation the component \(\mathit{SIYY}\) d u field SIEF_NOEU (calculated with the command CALC_CHAMP/CONTRAINTE) as contact pressure
Plot the contact pressure as a function of the radius in the contact zone, compare it to the analytical solution.
Calculate the constraint field by elements at the nodes (* SIEF_NOEU *): command CALC_CHAMP/CONTRAINTE.
Create a group of nodes with an oriented curvilinear abscissa: command DEFI_GROUP. We will keep the same mesh name with reuse. We will use the option CREA_GROUP_NO/OPTION =” NOEUD_ORDO “giving the mesh group (\(\mathit{CONT}1\)) and the starting point (\(C1\)).
Extract component \(\mathit{SIYY}\) from field SIEF_NOEU into a table at the last moment: command POST_RELEVE_T. We will specify the name of the node group, the moment, the field and its component using the EXTRACTION operation.
Create function \({\mathrm{\sigma }}_{\mathit{YY}}=f(x)\): command RECU_FONCTION. We will define the curvilinear abscissa (ABSC_CURV) as PARA_Xet SIYYcomme PARA_Y.
Building the analytical solution:
Calculate the pressure at points \(C1\) and \(C2\), \({P}_{0}\) and the contact half-width \(a\)
Create the analytical formula:command FORMULE. It depends on the curvilinear coordinate \(x\) (NOM_PARA =”x”/VALE =”P0* sqrt (1.-x * x/a/a) “).
Create a list of the real values of \(x\): Command DEFI_LIST_REEL. For example, 100 values from 0 to 10mm.
Interpolation of the formula from the list in \(x\): command CALC_FONC_INTERP.
Print both functions in the format XMGRACEpar the IMPR_FONCTION command.
3.1.6. Von Mises constraint#
Show the Von Mises constraint on the deformed configuration with Salome. How does this constraint vary in the sphere? Where is the maximum?
You can print the results in the format MED using the command IMPR_RESU in order to visualize the constraint field in Results or*in* Paravis and the maximum position (Edit → Find Data menu).
3.2. Tested sizes and results#
Identification |
Reference type |
Reference value |
Tolerance |
\({\sigma }_{\mathit{yy}}\) point \(\mathit{C1}\) |
“ANALYTIQUE” |
\(\mathrm{-}\mathrm{2798,3}\mathit{Mpa}\) |
|