1. Chapter 5 Advanced 3D Geometry
DesignModeler

2. Contents Modifying 3D Geometry 3D Curve Feature Planar Bodies
Boolean Operations
Named Selection Base Objects
Pattern Feature
Advanced Features
Advanced Tools
Body Operations
Mid Surface Extraction

3. Modifying 3D Geometry Thin/Surface:
The Thin/Surface feature has two distinct applications:
Create thin solids (Thin).
Create simplified shelling (Surface).
Selections available from Details:
Faces to Remove: Selected faces will be removed from their bodies.
Faces to Keep: Selected faces will be kept, while unselected faces are removed.
Bodies Only: The operation will be performed on the selected bodies without removing any faces.
When converting solids into thin solids or surfaces, you can specify a model's thickness in one of three offset directions:
Inward
Outward
Mid-Plane

4. Thin/Surface details:
Modifying 3D Geometry…
Thin/Surface details:
Basic operation
Direction for thin solid or offset
Thickness or Thickness/Face Offset
IMPORTANT! To create surface geometry (NOT thin solids) the Thickness field must be set to zero (0).
Examples . . .

5. Modifying 3D Geometry…
Using the simple block shown here, let’s look at basic Thin/Surface behavior.

6. Modifying 3D Geometry… After generating the feature, notice that:
The end face is removed
Thickness = 2 m
Direction is toward original solid’s center (inward)
Result is still a solid
By changing the thickness field to zero and re-generating:
True surface model results

7. Modifying 3D Geometry… Notes on Thin/Surface:
The Thin/Surface feature supports thickness > 0 if the selected faces are part of surface bodies.
This allows for the “thickening” of an imported surface.
Mid Plane Option:
This does not mean mid-plane extraction.
Bodies will be hollowed, such that the inner and outer walls of the bodies are offset equal distances from the original faces.
Example :
Resulting offset is in both directions.
Solid body selected for Thin/Surface midplane

8. Modifying 3D Geometry… Fixed Radius Blend:
The Fixed-Radius feature allows you to create blends on model edges.
You can select or pre-select 3D edges and/or faces for blending.
Face selection applies blend to all the edges from that face.
When pre-selecting, additional options are available from a RMB context menu
(face edge loop selection, smooth 3D edge chain)
You can edit the blend radius in the Detail View. Clicking Generate completes the feature creation and updates the model.
Variable Radius Blend (same as above plus):
Use the Detail View to change the start and end blend radius for each edge.
Also, the Detail View can set the transition between blends to smooth or linear. Clicking Generate completes the feature creation and updates the model.
Vertex Blend: allows surface or line body blending.
Vertex must belong to surface or line body.
Must connect to exactly 2 edges.
Geometry surrounding vertex must be planar.

9. Modifying 3D Geometry… Examples . . . Face selected for fixed blend.
All edges receive blend
Details specify blend radius
Edges selected for fixed blend.

10. Modifying 3D Geometry… Smooth Transition Linear Transition
Variable radius blend
If multiple edges selected for VR blend, each is listed in Detail

11. Modifying 3D Geometry… Chamfer:
The Chamfer feature allows you to create planar transitions (or chamfer face) across model edges.
You can select or pre-select 3D edges and/or faces for chamfering.
If a face is selected, all the edges from that face are chamfered.
When pre-selecting, additional options are available from a right
mouse button context menu (face edge loop selection, smooth 3D edge chain)
Every edge on a face has a direction. This direction defines a right and left side.
Chamfer is defined either by two distances from the edge for the planar transition (chamfer face), or by a distance (left or right) and an angle.
The type of chamfer is set up in the Detail View along with the distances and angle.

12. Modifying 3D Geometry…
Examples . . .
Chamfer options (3):
Left
Right

13. 3D Curve Feature Open Curve Closed Curve > Concept > 3D Curve
3D Curves can be used for:
Base Object in Modeling a Feature (must be a Named Selection first)
Custom curves for Concept Modeling
Create 3D curves (Line Bodies) from:
Existing Model points
Coordinates (text) File
Curve passes thru all points in the chain.
All points must be “unique”
Curves may be either open or closed.
Open Curve
Closed Curve 13

14. 3D Curve Feature - Existing Points
In the Details View: Definition>Point Select
Select (and >Apply) existing model points
Hold <CTRL> key to select multiple points.
Points selected can be 2D sketch points, 3D model vertices or ‘point feature’ points
Refer documentation for more on ‘Point Feature’ points
Curves may be either open or closed. (RMB)
Resulting curve passes thru all selected points.
RMB 14

15. 3D Curve Feature – From Coordinates File
>Definition>From Coordinates File
3D curve created by XYZ coordinates in a text file.
Format of Coordinates (text) File
# indicates Line is a comment
Empty lines are ignored
A data line consists of 5 fields, separated by spaces or tabs
A) Group # (integer)
B) Point Number (integer)
C) X coordinate
D) Y coordinate
E) Z Coordinate
Notes:
A data line with the same group # and Point # is in error. Must be unique
For a closed curve, the point number of last line should be zero.
Coordinate fields of last point ignored.
#Group 2, closed curve example file
#A B C D E
2 0
Click here to import the coordinates file 15

16. 3D Geometry Planar Bodies
Planar bodies are surface bodies in the XY-plane. [Can be Created via Thin/Surface Option]
Planar bodies created in DM are used to perform 2D Simulation.
Plane Strain, Plane Stress, Axisymmetry
Numerically more efficient Simulation models compared to “full” 3D models.
Solid
Planar
Planar bodies are distinguished by their flat icon in the body branch of the tree. 16

17. Subtract lower 2 bodies from upper
Boolean Operations
Use the Boolean feature (Create>Boolean) to Unite, Subtract or Intersect existing bodies.
Bodies can be Solid, Surface, or (for Unite only) Line bodies.
Surface bodies must have consistent normals.
Bodies are referred to as “target” or “tool” depending on operation type.
Examples (using 3 bodies shown below): . . .
Target Bodies
Subtract lower 2 bodies from upper
Tool Bodies

18. Boolean Operations Intersect all bodies Union of all intersections
Union of all intersections preserving input bodies

19. Named Selection Named Selections:
Can group entities under a single name
Select Entities, Right Click and click on Named Selection. Change the name in the details view. The “-” character not allowed.
The named selection may contain either Bodies, Faces, Edges, or Points.
Named Selections may be transferred to other Workbench applications, including the Meshing Application if Named Selections are toggled on from the Project page [See next Slide]
Named Selections cannot be made invisible in DesignModeler, however, they can be made invisible in Meshing Application
RMB 19

20. Toggling Named Selection on Project page
1. Click This
2. Highlight This
The prefix name of the Named Selections must include the characters defined in the Named Selection Key in order for the Named Selections to be transferred to another application. In this example, “NS” must be the prefix for the name, eg. NS_Face

21. Named Selection Base Objects
Named Selections can be used as base objects (Groups) for basic modeling features.
Required for using a 3D Curve as base object in a modeling feature.
Example1:
Extruding a circular profile along a 3D-Curve path
Create 3D curve & circular profile
3D- Curve
Circular Profile 21

22. Named Selection Base Objects
With the 3D Curve selected, create a Named Selection called “SweepPath”.
Create a ‘Sweep’ operation, with the circle as the profile and the Named Selection (SweepPath) as the path
Select Named Selection from the ‘Model Tree’ 22

23. Named Selection Base Objects
Example 2: Extruding faces
Create a named selection using the face of a solid
Create an ‘Extrude’ feature.
For ‘Base Object’ select the named selection from the ‘Model Tree’
Define a ‘Direction Vector’ using an axis or edge and ‘Generate’ 23

24. Pattern Feature Linear Circular Rectangular
Pattern feature allows you to create copies of faces or bodies in:
Linear pattern (direction + offset distance)
Circular pattern (rotation axis + angle)
Can set angle=zero to get auto-calculated evenly spaced instances
Rectangular pattern (two sets of directions + offsets)
For face selections, each copied instance must remain coincident with the originating body (must touch same base region).
Each copied face incidence must not touch/intersect each other
Linear Circular Rectangular 24

25. Total # of Patterns = Copies +1
Pattern Creation
Total # of Patterns = Copies +1
1 Face selected
Z-axis selected 25

26. Advanced Features Target Bodies:
Two Advanced Feature Properties described in this section apply selectively to the 3D Features:
Target Bodies: Extrude, Revolve, Sweep, Skin/Loft, Slice, Import & Attach.
Merge Topology: Extrude, Revolve, Sweep, & Skin/Loft.
Target Bodies:
allows users to specify which bodies are operated on during a Cut, Imprint, or Slice operation.
Cut operation applied only to Selected Bodies 26

27. Advanced Features…
Merge Topology: Details property for Extrude, Revolve, Sweep, & Skin
A Yes/No detail option that gives control over feature topology.
>Yes: optimizes the topology of feature bodies.
>No: leaves the topology of feature bodies unaltered.
The default setting for Merge Topology differs depending on the 3D feature you are using:
Extrude: default is Yes
Revolve: default is Yes
Skin/Loft: default is No
Sweep: default is No
Example follows . . . 27

28. Advanced Features… Example Topological Control
Merge Topology = >Yes
Merge Topology = >No
Setting the value to >Yes optimizes all topology of the feature body. It is however, recommended to leave this setting as >No (default) for the Skin/Loft and Sweep features.
Use caution when changing the value of the Merge Topology property.
Once other features depend on this, faces and edges may appear or disappear and cause failures and invalid selections for subsequent features. 28

29. Advanced Tools
Advanced operations are available via the >Create and >Tools Menu:
Freeze
Unfreeze
Enclosure
Fill
Symmetry
Surface Extension
Pattern
Body Operation
Boolean
Slice
Face Delete
Edge Delete
Merge
Connect
Projection 29

30. Normally, a 3D solid feature operates like this:
Advanced Tools…
Normally, a 3D solid feature operates like this:
Create the bodies of the 3D feature (e.g., an Extrude feature)
Merge the feature bodies with the existing model via Boolean operations: Add Material, Cut Material, Imprint Faces
Freeze
The Freeze feature allows you to control the second step acting as a separator in the construction history as displayed in the Feature Tree.
Bodies created from features before a Freeze will become frozen
Frozen bodies are denoted by the ice cube icon next to the body’s branch of the Feature Tree
All frozen bodies are ignored by Add, Cut, or Imprint Material operation for any features following the Freeze 30

31. Advanced Tools… Freeze Example Modeling history:
Model began with imported geometry consisting of two bodies.
An extrusion was added
A freeze was inserted
A second extrusion was created from the imported geometry
Frozen
Only 2 solids now frozen
Second extrusion is an independent solid. Without the freeze this geometry would have been merged with the import
Unfrozen 31

32. Advanced Tools… Unfreeze
Unfreeze allows one to selectively “remove” the freeze from single or multiple bodies (freeze is a global operation)
Assembly notes:
By default if you import an assembly from a CAD package, the assembly will remain as separate parts in DM without freezing
Any subsequent 3D modeling operation however will result in a merge of any touching bodies in the assembly
This can be avoided with the Freeze and Unfreeze tools 32

33. Advanced Tools… Enclosure:
Creates surrounding region around bodies to facilitate simulation of field regions
CFD, EMAG, etc
Box, sphere, cylinder or user defined shapes can be employed
Cushion property allows the boundary extent to be specified (must be > 0)
Apply enclosure to all bodies or only selected targets
Merge property allows for automatic multi-body part creation
Ensures original part and enclosure will have nodal match up when meshed

34. Advanced Tools… Enclosure Example: Circuit board model
Cutaway view of enclosure
Enclosure created using box option

35. Two Methods for Fill operation
Advanced Tools…
Fill:
Creates frozen bodies that fill interior voids such as holes
Works with active or frozen bodies
Works only with solid bodies
Useful in CFD applications for creating flow volumes
Two Methods for Fill operation
By Cavity
By Caps

36. Example: Fill by Cavity
Advanced Tools…
Example: Fill by Cavity
Goal is to model the interior (fluid region) of the valve block shown here
The desired (37) interior faces are selected then the Fill is inserted by clicking Generate

37. Example: Fill by Cavity (cont.):
Advanced Tools…
Example: Fill by Cavity (cont.):
Resulting fill is a frozen (meshable) body
Interior region, now isolated, can be taken to the Mesher for meshing

38. Advanced Tools… Example: Fill by Caps
Goal is to model the interior (fluid region) of the hollow pipe shown here
Steps:
Create surfaces and close both ends of the pipe.
Use > Concept > Surfaces from Edges to create the end surfaces
Use Fill by Caps to create the interior flow region

39. Advanced Tools…
Example Fill by Caps (cont.): 2 1
Closed End surface 3

40. Interior Fluid Body Created
Advanced Tools…
Example Fill by Caps (cont.): 2 1
Interior Fluid Body Created

41. Advanced Tools… Surface Extension:
Creates a surface extension [ Tools> Surface Extension ] based on edge selection
Extension can be fixed or to selected faces /
surface/Next
Example:
The model is converted to a mid plane surface model. The result is a gap at the intersection of the 2 parts
A thin solid model
Extending the circular edge closes the gap

42. Example (delete blends and hole feature):
Advanced Tools…
Face Delete [> Create > Face Delete]:
Can remove features such as blends and cuts by removing faces from the model - - then heal the resulting “wound”
If a suitable extension cannot be determined, the feature will report an error stating that it cannot heal the wound.
Can choose healing types: automatic, natural, patch or no healing (see next page).
Example (delete blends and hole feature):
Select the highlighted surfaces
After “Face Delete” the result is no blends, cavities or holes

43. Selected faces for delete
Advanced Tools…
Healing options:
Patch healing
Selected faces for delete
Natural healing
See Documentation for more Details

44. Advanced Tools… Slice feature [ > Create >Slice ]:
Slice is only available when the model consists entirely of frozen bodies
Slice has four options:
Slice By Plane: Select a plane and the model is sliced by this plane.
Slice Off Faces: Select faces on the model and DM will “slice off” these faces & then attempt to create a separate body from them.
Slice Off Edges: Select Edges on the model and DM will “slice off” these edges & then attempt to create a separate Line body from them.
Slice by Surfaces: Choose a “target” surface as a slicing tool to slice bodies.
Result is 3 solids. Each blend becomes solid region
Original geometry, one solid
2 blends chosen for slice

45. Advanced Tools… Symmetry feature [ Tools > Symmetry ]:
Performs slicing to create a symmetry model.
Up to three symmetry planes can be defined.
Material on the positive side of each plane is retained, while material on the negative side is cut away
Example: one and two plane symmetry

46. Body Operations Body Operation:
allows users to manipulate bodies via 11 different options (not all will be available at all times):
Any type of body can be used with Body Operations, (active or frozen).
“Point Feature” points, attached to the faces or edges of the selected bodies, are not affected by the Body Operation
Bodies and Planes are selected via the Details View
Options include:
Mirror, Move, Delete, Scale, Sew, Simplify,
Translate, Rotate, Slice Material, Cut Material, Imprint Faces
Each described next . . .

47. Body Operations… Mirror: User selects bodies and a mirror plane.
DM creates copies of the selected bodies that are reflections of the original bodies in the mirror plane.
Active bodies that are reflected will be merged with the active model.
Frozen bodies that are reflected will not be merged.
By default, the mirror plane is initially the active plane.
Example: selected surface here is mirror plane.

48. Body Operations… Move: 1 1,2 2
Users select bodies and two planes: a Source Plane and a Destination Plane.
Design-Modeler will transform the selected bodies from the Source Plane to the Destination Plane.
This is especially useful for aligning imported or attached bodies.
Example:
Two imported bodies (a box and a lid) don’t align.
Maybe they were exported separately from a CAD system in two different coordinate systems.
Problem is corrected using the “>Move” Body Operation. 1
1,2 2

49. Body Operations… Delete: Scale:
Users select bodies to delete from the model.
Scale:
Users select bodies to scale, then select a scaling origin through the Scaling Origin property.
This property is a combination box with three options:
World Origin: The origin of the global coordinate system is used.
Body Centroids: Each body is scaled about its own centroid.
Point: User can select a specific point, (2D sketch point, 3D vertex, or PF Point) to use as the scaling origin.

50. Body Operations… Cut Material:
Users select bodies for a cut operation from the active bodies in the model.
Body Operation's Cut Material option works the same way as Cut Material does for any of the basic features.
Example:
A body is selected to cut from the block to form a mold:
After the Cut

51. Body Operations… Imprint Faces:
Body Operation's Imprint Faces option works the same way as Imprint Faces does for any of the basic features.
This option is available when active bodies exist in the model.
In this example, the selected body is used to imprint the faces of the block:
After the Face Imprint

52. Body Operations… Slice Material:
Slice operations are performed on a completely frozen model.
Body Operation's Slice Material operation works the same as Slice Material does for any of the basic features.
Option is available only when all bodies in the model are frozen.
Example of a slice operation: airplane body is selected to slice the block

53. Body Operations… Sew: Example: . . .
Select surface bodies for sewing operation, DM will attempt to sew surfaces together at common edges (within given tolerance).
Options:
Create solids: will sew surfaces together and create a solid from the closed surfaces.
Tolerance: Normal, loose or user defined.
User tolerance: dimension used for sewing operation.
Example: . . .
2 sketches are used to create 2 surface bodies (note dimension separating surfaces is contrived to illustrate
Following the sew operation, a single surface is stitched together forming one surface

54. Original body contains NURBS surfaces
Body Operations…
Simplify:
Allows geometry and/or topology simplification:
Geometry: Simplifies surfaces and curves into analytic geometry where possible (default = yes).
Topology: Will remove redundant faces, edges and vertices where possible (default = yes).
Simplify operation turns NURBS into planes merges surfaces to form a single cone
Original body contains NURBS surfaces

55. Body Operations… Translate:
Select Bodies to Translate in a specified direction
Direction Specification:
Selection: Specify the Distance along a Direction Selection
Coordinates: Specify the x, y, z offsets

56. Body Operations… Rotate:
Select Bodies to Rotate about a specified axis and by a specified angle
Axis Specification:
Selection: Specify the Distance along a Direction Selection
Components: Specify the x, y, z components of a vector

57. Mid-Surface representation
Mid-Surface Creation
Mid-Surface Tool:
Reduces 3D geometry of constant thickness to a simplified “shell” representation
Automatically places surface body at mid point between 3D face pairs
Allows shell element type meshing in MECHANICAL.
3D Model
Mid-Surface representation

58. …Mid-Surface Creation
Manual Mid-Surface creation:
Face Pairs: With “Apply/Cancel” buttons active, choose the face pair
Note the order of selection determines the surface normal direction
Notice the first surface picked is displayed in purple, the second is shown in pink
1st Pick
2nd Pick
Normal Direction
Resulting Surface Body

59. …Mid-Surface Creation
Selection Note: While in select mode (Apply/Cancel active), the color scheme described in the previous slide is in effect. When the selection is finalized the selected pairs are displayed in dark and light blue colors.

60. …Mid-Surface Creation
Mid-surface details:
Multiple surface pairs may be selected for a single mid-surface operation, however they must be selected as opposing pairs (see picture)
Adjacent face pairs will be grouped together if within the “Thickness Tolerance” (see below) 3 1 5 4 6 2 T1 T2
If │T1 – T2│ < Thickness Tolerance: surfaces are grouped

61. …Mid-Surface Creation
Mid-surface details:
If gaps exist in adjacent face pairs, they will be sewn together within the “Sewing Tolerance”
Sewing Tolerance: If Gap < Sewing Tolerance: Surfaces are grouped
Gap

62. …Mid-Surface Creation
Automatic mid-surface creation:
Switching the “Selection Method” from Manual to Automatic exposes several additional options
Bodies to search: Limits search to visible bodies, selected bodies or all bodies
Minimum and maximum threshold sets search range (thickness) for face pairs
Extra trimming provides options for situations where trimming problems with surface bodies occur (described later)
Preserve bodies allows you to save the solid bodies from which surfaces are created (default is No)

63. …Mid-Surface Creation
Automatic mid-surface example:
Solid body is 5 mm thick
When the mid-surface tool is inserted we switch to “Automatic”
Note: The “Face Pairs” field used in manual mode is left “0”
With a constant thickness throughout we set the min/max threshold values to 5 mm
Using the drop down choice we choose “Find Face Pairs Now? = Yes”
Continued . . .

64. …Mid-Surface Creation
Automatic mid-surface example (continued):
When the search is complete the number of pairs detected is listed in the details and displayed graphically
Mid surface creation is completed by “Generating” the surface body

65. …Mid-Surface Creation
Mixing manual and automatic selection modes:
In some cases it is convenient to make an initial surface pair selection and let the automatic method complete the process
Example:
The model shown here contains 2 different thicknesses
In this case we’ll select, (manually) a face pair of each thickness
We will then allow the auto face detection to complete the selection
2 mm
1 mm

66. …Mid-Surface Creation
We begin by manually selecting the 2 face pairs shown here
Note the face pairs selected contain a 1 mm and a 2 mm pair
We now change the selection method to “Automatic”
Note the min/max threshold values are automatically defined based on our manual selections
Continued . . .

67. …Mid-Surface Creation
We now activate “Find Face Pairs Now”
Notice there are 2 options (due to the pre selection of face pairs)
Yes-Add to Face Pairs: adds auto detected faces to the existing face pairs selected
Yes-Replace Face Pairs: will use only the auto detected faces
Choosing to add face pairs allows us to complete the operation

68. …Mid-Surface Creation
Adding to, removing from or modifying “automatic surface selection”:
Examples:
In this case the maximum threshold was increased to intentionally detect unwanted surfaces

69. …Mid-Surface Creation
Clicking in the “Face Pairs” field activates selection mode (note the colors change to indicate this)
RMB in the graphics window provides the optional selection modes
In this case we can choose “Remove Face Pairs” then select one of the faces to be removed
When selection is complete “Generate” to update the model
Note when removing face pairs, selecting one of the faces will remove the pair

70. …Mid-Surface Creation
Trimming options:
In cases where trimming problems occur there are several options available to attempt corrections
Example:
Using the previous model we generate the surface model without removing the unwanted face pairs
Since the pairs created result in T junctions, trimming problems occur
Notice the mid-surface branch in the tree is displayed with a yellow check indicating there is a problem

71. …Mid-Surface Creation
Using the RMB option we can “Show Problematic Geometry”
The resulting plot shows regions where trimming problems have occurred
The default behavior is to intersect any untrimmed surfaces with the original solid body
Other options:
Delete untrimmed
No Extra Trimming