Abstract 3D geometry to 2D plane and apply 2D thickness

Learn how to abstract a cyclically symmetric 3D gas turbine strut assembly into a 2D model and apply thickness definitions for thermal and structural simulation efficiency.

Download and extract the part files.

Introduction

3D gas turbine components often exhibit cyclic symmetry or axisymmetric behavior. In such cases, modeling the thermal and structural response in 2D can significantly reduce simulation time while maintaining accuracy.

The workflow includes:

Creating an idealized part.
WAVE-linking the geometry.
Generating curves with the Revolve Outline command.
Creating surfaces using the Bounded Plane tool.
Dividing sheet bodies into multiple faces.
Review how to display and evaluate free edges.
Assign 2D thickness values derived from the original 3D geometry.
Verify the 2D element volume against the 3D model to ensure accuracy.

Open the part file

Open the part file and reset the dialog box settings.

Choose File→Open and open abstraction\strut.prt.
Choose File→Preferences→User Interface and on the Dialog and Precision page, reset the dialog box memory.
Click OK.

Create the idealized part

Use an idealized part to simplify and modify geometry for simulation while keeping the original CAD model unchanged.

On the Application tab, click Pre/Post .
In the Simulation Navigator, right-click the strut.prt file and choose New Idealized Part.
Click OK twice.

Create an associative copy of the geometry

On the Application tab, click Modeling .
Newly created idealized parts open in the Pre/Post environment by default. Switching to the Modeling environment allows you to access the complete set of modeling tools.
Choose Assemblies > Interpart Link > Wave Geometry Linker to create an associative copy of the geometry you want to modify to isolate the analysis geometry while keeping a link to CAD updates.
Select the Body type from the list, in the graphics window select one of the two bodies, and click OK.
Repeat the wave linking process for the second body.

After WAVE linking, the model contains four bodies.
In the Assembly Navigator, right-click the strut part, and choose Replace Reference Set > Empty to remove the master part from the idealized part, since it is not required for meshing or simulation.
This ensures that only the relevant bodies remain available for meshing and for defining boundary conditions, reducing the risk of selecting unintended geometry.
Verify that only two wave-linked bodies remain visible in the Part Navigator.

Create the 2D sheet bodies

Use the Revolve Outline command to create a 2D representation of a cyclically symmetric 3D gas turbine strut.

Choose Curve > Derived > More > Revolve Outline to project 3D geometry onto the axisymmetric plane.
Select each body individually to generate curves.
In the Part Navigator, hide the linked bodies.
Choose Surface > Base > More > Bounded Plane to create a bounded plane using the outer curves.
Select the outer 12 curves as shown.
Repeat the steps 3 to 5 to create bounded plane for the second body.

12 curves are selected.
Choose Surface > Combine > More > Divide Face to subdivide sheet bodies into multiple faces.
For the first body, select the shown one face.
Select the shown 14 objects.

You can verify that three faces are created.
For the second sheet body select the following one face.
Select the shown 16 objects.

You can verify that nine faces are created.

Tip:
On the Top toolbar, from the Type Filter list, select Face, then select the model to identify and explore the newly created faces.
12 faces are created.

Split the body

Split the 3D bodies to obtain accurate, region-specific volumes that will later be used to define 2D thicknesses. By splitting the body:

Each 3D region corresponds directly to a specific 2D face.
Features like holes, inner/outer cylinders, or thickness changes are isolated.
Volume measurements become physically meaningful for each 2D region.

In the Part Navigator, display only the linked bodies.
Choose Home > Base > More > Split Body to divide the wave-linked bodies using edge extrusions.
Select the shown body as a target body.
From the Tool Option list, select Extrude, and select the shown curves.
Repeat the steps 2 to 4 for the second linked body. Select the shown curves.

These curves are selected because they define the radial limits of the regions that must be isolated to obtain accurate, region-specific 3D volume measurements for 2D thickness definition.
To accurately measure volumes in regions containing holes, the second body must be split twice in the XY plane. Choose Home > Construction > Datum Plane to create datum planes in the XY plane to perform this additional subdivision.
From the list, select At Distance and select the shown surface.
In the Distance box, type 32.49, and click Reverse Direction, if the plane does not cross the model.
Rotate the model by 180 degrees and repeat the same process on the opposite side.
Split the shown inner and outer cylinders using the created datum planes.

Measure volumes and create measurements

Measure volumes for the 3D regions and create measurement expressions for the measured areas of all corresponding 2D regions.

Choose Menu > Analysis > Measure to measure volumes for the 3D regions.
Use the Object Set option, when selecting more than one solid body for the volume measurement.
On the Top border bar, from the Type Filter list, select Solid Body, and select the shown bodies.
Click the P button to save each volume measurement as an expression that will be referenced later in FEM.
Notice that the Measure Body is created in the Part Navigator.

Repeat the same process for all bodies shown below.

Open the Expressions dialog box by using Ctrl+E.

In the Part Navigator, click on the Measure Body and rename the created expression as follows:


Body
Expression name	V_strut_shield	V_strut	V_inner	V_outer

Create area measurements for the corresponding 2D regions, by:
- Displaying only the bounded planes.
- Measuring areas of all corresponding 2D regions.

Rename created expressions as follows:


Face
Expression name	A_strut_shield	A_strut	A_inner	A_outer

Create thickness expressions by dividing volume expressions by area expressions as follows:


Thickness expression	Formula
thk_inner	V_inner/A_inner
thk_outer	V_outer/A_outer
thk_strut	V_strut/A_strut
thk_strut_shield	V_strut_shield/A_strut_shield

Create the FEM and apply thicknesses

Create a 2D FEM, apply axisymmetric and plane stress meshes with thickness expressions, and verify that the 2D model matches the 3D volume within acceptable tolerance.

Choose Application > Simulation > Pre/Post .
Right-click the idealized part, select New FEM, and choose Simcenter 3D Multiphysics environment.
In the Solver Environment group:
- Analysis Type to Thermal
- 2D Solid Option to ZX Plane, Z Axis to specify a plane on which you create axisymmetric elements and the axis of rotation.
- Select the Create Cyclic CSYS check box to set the global cyclic analysis coordinate system as the default coordinate system for boundary conditions.
Choose Menu > Preferences > Model Display.
From the list, select Polygon Edges and select the Display Free Edges check box.

The two sheet bodies are now displayed with their free edges. Identifying free edges is important because edges in contact do not conduct heat by default. This view helps determine where thermal couplings must be defined or where edge stitching is required to ensure proper heat transfer.
Choose Home > Mesh > 2D Mesh to apply a 2D axisymmetric mesh to the appropriate regions.
Select the shown regions.
From the Type list, select Axysimmetric Linear Quadrilateral.
Next to Element Size, click Automatic Element Size to let the software to compute it.
For the strut, inner, and outer rings, create a 2D mesh using Plane Stress Linear Quadrilateral elements with the automatic element size.
Select the shown regions.
Create separate meshes for each face by setting Create Separate Meshes to On - For Each Face. This approach allows to assign varying thicknesses to each region.
For the remaining faces, create a 2D mesh using Plane Stress Linear Quadrilateral elements with the automatic element size but without creating separate meshes. These faces are grouped together because they share the same thickness definition.
Import thickness expressions from the idealized part the Expression command.
Click Create Multiple Interpart Expressions and select the idealized part.
In the Source Expressions, select all thickness expressions, and click Add to Destination .
Right-click each plane stress mesh and select Edit Mesh Associated Data.
In the Thickness group, from the Thickness Source list, select Field/Expression, and in the Thickness box, assign the appropriate thickness expression.
In this case, the geometry is represented using a single instance, consistent with how the 3D volume was measured.

Verify a volume check on the meshes

Verify that the 2D model matches the 3D volume within acceptable tolerance. From the volume measurements in 3D, the total volume is 8539473 mm³.

Choose Home > Checks and Informations > Solid Properties Checks and select the whole 2D model to obtain the 2D volume.
The resulting 2D volume is 8539681 mm³ which is approximately 0.003% higher than the 3D volume. This level of deviation is generally acceptable. If greater accuracy is required, you can either refine the 2D mesh or apply a scaling factor to the thickness definitions.
In the Simulation Navigator, right-click the 2D Collector and select Plot Thickness Contours to visually verify thickness definitions.

Subdivide geometry further if thickness varies significantly in radial or axial directions. Use constant or manually defined thickness values if associativity with 3D geometry is not required.