Simplifying geometry

Estimated time to complete: 5–15 minutes

In this tutorial, you will use basic geometry idealization and abstraction commands to simplify a model in preparation for meshing. You will use the Split Body command to partition the model and then remove features from the geometry, including edge blends and a slot that are not significant to the analysis.

1: Setup

Before starting the tutorial, you must download the part.

  1. On your desktop or the appropriate network drive, create a folder named geometry_cleanup.

  2. Click the link below:

    Download the part

  3. Extract the files to your geometry_cleanup folder.

  4. Start Simcenter 3D or NX.

  5. Open disk_fem1.fem.

2: Reset dialog box memory

The options you select in dialog boxes are preserved for the next time you open the same dialog box within a given session. Restore the default settings to ensure that the dialog boxes are in the expected initial state for each step of the activity.

File

Preferences→User Interface

  • Options

  •   Reset Dialog Memory

  • OK

     
3: Display the idealized part

You can remove sliver surfaces, along with features such as fillets, in preparation for a finite element mesh. You perform this idealization on the idealized part, which is an assembly instance of your master part. You do not make these changes directly on the master part.

  Simulation Navigator

  •   disk_fem1_i.prt

  •   Load

  •   disk_fem1_i.prt

  •   Make Displayed Part

  • OK

     Idealized Part Warning

    The warning alerts you to the fact that you must first promote or WAVE-link the body you are working with before you can perform any idealization command.

The idealized part is now displayed in the Simulation Navigator.

4: Split the geometry

Because the disk is symmetrical, you can decrease the solve time by splitting the body and analyzing only half of it. For simplicity, we are splitting the body in half, but you could also split it into quarters for even greater efficiency.

Before you can split the body, you must promote it.

  Promote (Home tab→Start group)

  •   the part

  • OK

     

 Split Body (Geometry Preparation group)

  •   the part

  • Because there is no partitioning geometry, you will create a datum plane.

    Tool Option

    New Plane

  • Specify Plane

      XC-ZC Plane

  • OK

     
5: Hide half of the disk

  Hide (Top border bar→Show/Hide Drop-down list)

  •   the left half of the disk

  • OK

     
6: Delete the edge blends

The edge blends on your part are not significant to your analysis, so you will remove them.

  Delete Face (Synchronous Modeling group)

  •    

  • OK

     

    The edges of the part are now sharp.

7: Examine the geometry

You will examine the geometry for tiny surfaces that may cause meshing problems.

  Menu 

  •   Analysis→Examine Geometry

  •   Drag a box around the entire part.

  •  

  •   Tiny

  •  

  • Distance

    3.0

    For this analysis, you can assume a “tiny” surface to be about 1/100 of the radius of the disk. The overall radius of the disk is 270 mm, so 3 mm is a good value to use.

  • Angle

    0.5

  • Examine Geometry

     

    The entire part is highlighted and the Highlight Results check box appears under the Object Checks / Post Check Status group.

  •   Highlight Results

    Note the tiny slot that is highlighted on the bottom face of the part (zoom in on the slot if necessary).

  • Close

     

  Refresh (graphics window)

8: Remove the slot

The disk is supported by the small slot around the outside edge. The slot is needed for a boundary condition, but it will interfere with meshing. You will remove the slot and replace it with an edge to which you can later assign the boundary condition.

  Delete Face  (Synchronous Modeling group)

  • Type

    Face

  • Face Rule (Top Border bar)

    Slot Faces

  •     any face in the slot; zoom in if necessary

  • OK

     

  • The slot is removed.

9: Display the FEM file

  Simulation Navigator

  •  

  •   disk_fem1

  •   Make Displayed Part

  •   the Information window

The FEM file is now displayed in the Simulation Navigator. It is also the work part.

10: Suppress the small edge

In the FEM file, you can use abstraction tools to further prepare your part for meshing. You will suppress an edge that will distort elements created along the curved face.

  Merge Face (Polygon Geometry group)

  •  

  • OK

     
11: Create a 3D mesh collector

Mesh collectors let you organize your model by grouping your meshes logically. Each mesh collector references a physical property table. They are especially valuable when working with complex, non-homogenous models because you can use them to control the mesh display properties, such as element color, shrink percentage, and so on.

  Mesh Collector (Properties group)

  • Element Family

    3D

  • Name

    Polycarb

  •   Create Physical (Solid)

  •   Choose material (Material)

  • Materials

    Polycarbonate

  • OK

     all dialog boxes 
12: Create the 3D mesh

You are now ready to mesh the part.

 3D Tetrahedral (Mesh group)

  • the part

  • Type

    CTETRA(10)

  •   Automatic Element Size (Element Size)

    Clicking this button calculates the element length based on the geometry you selected.

  •  

  •   Automatic Creation

  • Mesh Collector

    Polycarb

    This is the mesh collector you created in the previous step.

  • OK

     

 

 

 Save

At this point, you could add loads and constraints, solve the model, and display results.

 

File

  • Close→All Parts