Mechanical enables you to run two-dimensional (2D) simulations for structural and thermal analyses. Two-dimensional simulations can save processing time and conserve machine resources for models and environments that involve negligible effects from a third dimension. You specify your analysis as two-dimensional on the Workbench project page (Analysis Type property for the Geometry cell set to ). However, as desired, you can change the setting of the Analysis Type property to switch your analysis to 3D at any time.
Important:
Switching your analysis from 2D to 3D (or vise versa) could invalidate certain specifications you have defined in your analysis. Specifically, if you have defined parameters, they may become invalid and although it would display in the Parameter Manager, it would not be available in Mechanical.
When you are performing a 3D simulation on shell bodies (only), you can specify a shell body as 2D using the Dimension property of the Body object.
For a line body in a 2D thermal analysis, you can set the Model Type property to .
Go to a section topic:
Specify 2D Analysis in Workbench
For a 2D analysis, Mechanical supports surface and line bodies that are planar bodies on the X-Y plane. To create a 2D analysis:
Add an analysis to the Workbench Project page
Open your model in the appropriate Ansys application, such as Discovery, or another supported CAD system, and specify that the model's orientation is in the x-y plane.
On the project page, select the Geometry cell of the analysis system and set the Analysis Type property to (Advanced Geometry Options).
Open the model in Mechanical.
Define the 2D Behavior of Geometry
Specify the 2D Behavior property of the Geometry object. Options include:
(default): Assumes zero stress and non-zero strain in the z direction. Use this option for structures where the z dimension is smaller than the x and y dimensions. Example uses are flat plates subjected to in-plane loading, or thin disks under pressure or centrifugal loading. A Thickness field is also available if you want to enter the thickness of the model.
: Assumes that a 3D model and its loading can be generated by revolving a 2D section 360o about the y-axis. The axis of symmetry must coincide with the global y-axis. The geometry must lie on the positive x-axis of the x-y plane. The y direction is axial, the x direction is radial, and the z direction is in the circumferential (hoop) direction. The hoop displacement is zero. Hoop strains and stresses are usually very significant. Example uses are pressure vessels, straight pipes, and shafts. You may wish to review the Axisymmetric Loads and Reactions section, of the Mechanical APDL Basic Analysis Guide, for a description about how to apply constraints in order to prevent unwanted rigid-body motions.
Note: Certain CAD applications automatically increase the bounding box size beyond the exact limits of the geometry and can cause the geometry to appear in the negative X plane. This causes Mechanical to generate an error and prohibit a solution. In this scenario, you can change the error setting to a warning in order to perform a solution. You use the Geometry preference 2D Axisymmetric Check in the Options dialog to change this setting.
: Assumes zero strain in the z direction. Use this option for structures where the z dimension is much larger than the x and y dimensions. The stress in the z direction is non-zero. Example uses are long, constant, cross-sectional structures such as structural line bodies. behavior cannot be used in a thermal analysis (steady-state or a transient).
Note: Since thickness is infinite in plane strain calculations, different results (displacements/stresses) will be calculated for extensive loads (that is, forces/heats) if the solution is performed in different unit systems (MKS vs. NMM). Intensive loads (pressure, heat flux) will not give different results. In either case, equilibrium is maintained and thus reactions will not change. This is an expected consequence of applying extensive loads in a plane strain analysis. In such a condition, if you change the Mechanical application unit system after a solve, you should clear the result and solve again.
: Assumes a finite deformation domain length in the z direction, as opposed to the infinite value assumed for the standard option. provides more practical results for deformation problems where a z direction dimension exists, but is not considerable. See the next section, Using Generalized Plane Strain, for more information.
The option requires you to specify the following properties:
: Sets the length of the extrusion.
: Sets the rotation of the extrusion end plane about the x-axis.
: Sets the rotation of the extrusion end plane about the y-axis.
: Enables you to set the (with option), , or options for individual bodies that appear under Geometry in the tree. If you choose , then click an individual body, these 2D options are displayed for the individual body.
Review Requirements and Limitations
- Requirements for Specifying Boundary Conditions
For a 2D analysis, you use the same procedure for applying loads and supports as you would use in a 3D analysis. However, the loads and results are in the x-y plane and there is no z component. All loads and supports, except the following:
Line Pressure
Simply Supported
Fixed Rotation
Important: When your 2D analysis includes any of the following boundary conditions, the results may not be accurate in certain cases where more than one element type has already been created on the scoped surface.
Hydrostatic Pressure
Force (Applied By property set to Surface Effect)
Pressure (Applied By property set to Surface Effect)
Bearing Loads
Elastic Support
Heat flux
Radiation
Convection
Please review the output file carefully for related messages before looking at the results. See the SURF151 and SURF153 sections in the Mechanical APDL Element Reference for more information.
- General Limitations
Note the following limitations:
A Pressure load can only be applied to an edge.
A Bearing Load and a Cylindrical Support can only be applied to a circular edge.
For analyses involving axisymmetric behavior, Rotational Velocity loads can only be applied about the y-axis.
For loads applied to a circular edge, the direction flipping in the z axis will be ignored.
Only Plain Strain and Axisymmetric are supported for Explicit Dynamics analyses.
Mechanical does not support Cyclic results for a 2D Analysis.