3D Geometry

1
3D Geometry

• Chapter 4

2
3D GeometryContents

• Bodies and Parts
• 3D Features
• Boolean Operations
• Feature Direction
• Feature Type
• Feature Creation
• Workshop 4-1, Catalytic Converter

3
3D GeometryBodies and Parts

• DesignModeler is primarily intended to provide
  geometry to an analysis environment. For this
  reason we need to see how DM treats various
  geometries

• DesignModeler contains three different body
  types
• Solid body body has surface area and volume
• Surface body body has surface area but no volume
• Line body body consists entirely of edges, no
  area, no volume
• By default, DM places each body into one part
  by itself

4
3D GeometryBodies and Parts

• There are two body states in DM
• Active
• Body can be modified by normal modeling
  operations (cannot be sliced)
• Active bodies are displayed in blue in the
  Feature Tree View
• The body's icon in the Feature Tree View is
  dependent on its type - solid, surface, or line
• Frozen (gtToolsgtFreeze)
• Two Purposes
• Provides alternate method for Sim Assembly
  Modeling
• Provides ability to Slice parts.
• A Frozen body is immune to all modeling
  operations except slicing
• To move all active bodies to the Frozen state,
  use the Freeze feature
• To move individual bodies from the frozen to
  active, select the body and use the Unfreeze
  feature
• Frozen bodies are displayed lighter in the Tree
  View

Active
Frozen
5
3D GeometryBodies and Parts

• Body Suppression
• Suppressed bodies are not plotted.
• Suppressed bodies are not sent to Design
  Simulation for analysis, nor are they included in
  the model when exporting to a Parasolid (.x_t) or
  ANSYS Neutral File (.anf) format.
• In the tree view an X is shown near suppressed
  bodies

Unsuppressed
Suppressed
6
3D GeometryBodies and Parts

• Parts
• By default, the DesignModeler places each body
  into one part by itself.
• You can group bodies into parts
• These parts will be transferred to Design
  Simulation as parts consisting of multiple bodies
  (volumes), but with shared topology.
• To form a new part, select two or more (or RMB
  Select All) bodies from the graphics screen and
  use gtToolsgtForm New Part
• The Form New Part option is available only when
  bodies are selected and you are not in a feature
  creation or feature edit state.

7
3D GeometryBodies and Parts

• Why multi-body parts?
• Example
• In DM 3 parts, 3 bodies consisting of 3 solids
• In Sim 3 solids with 2 contact regions
• Each solid meshed independently
• Nodes are not shared
• Nodes do not line-up

DM
Sim
DM
8
3D GeometryBodies and Parts

• Example (continued)
• In DM 1 part, 1 body consisting of 1 solid
• In Sim 1 solid (no contact)
• Entire solid meshed as one
• One material
• No internal surfaces

DM
Sim
DM
9
3D GeometryBodies and Parts

• Example
• In DM 1 multi-body part, 3 solids
• In Sim 3 solids (no contact)
• Each solid meshed independently but node
  connectivity among solids is preserved

DM
Sim
DM
10
3D Geometry3D Features

• Typically, the generation of a 3D feature (like
  Extrude or Sweep) consists of two steps
• (a) Choose the desired feature and specify its
  details
• (b) Generate the feature bodies
• Each 3D feature creation is controlled via the
  associated details
• The last step in creating 3D features is to click
  Generate

11
3D Geometry3D Features
3D Feature
Frozen Bodies in model?
Its all in the details!
12
3D GeometryBoolean Operations

• You can apply five different Boolean operations
  to 3D features
• Add Material creates material and merges it
  with the active bodies.
• It is always available
• Cut Material removes material from active bodies
• Slice Material slices frozen bodies into pieces.
  
• Available only when ALL bodies in the model are
  frozen
• Imprint Faces Similar to Slice, except that only
  the faces of the bodies are split, and edges are
  imprinted if necessary (no new bodies created)
• Add Frozen Similar to Add Material, except that
  the feature bodies are not merged with the
  existing model but rather added as frozen bodies
• Line bodies are immune to Cut, Imprint, and Slice
  operations

If frozen
13
3D GeometryBoolean Operations

• Boolean Add

Choose feature and Boolean operation to be
performed on the active sketch
Extrude Add Material shown here
Note If bodies already exist, add results in
merged geometry after Generate
14
3D GeometryBoolean Operations

• Boolean Cut

Existing solid (shown in wire frame for
clarity) Revolve with Cut operation
Active Sketch
Axis of revolution
15
3D GeometryBoolean Operations

• Boolean Imprint Faces
• Imprint Face operation allows continuous surface
  to be segmented (see below). Useful for applying
  FE boundary conditions at arbitrary locations.

Active sketch to extrude Extrude with Imprint
Faces operation.
16
3D GeometryBoolean Operations

• Boolean Add Frozen
• Similar to add operation but results in separate
  bodies (or single frozen body)

Active sketch to extrude Extrude with Add
Frozen operation
17
3D GeometryBoolean Operations

• Boolean Slice (all bodies must be frozen)
• Slices frozen bodies leaving new (frozen) body in
  the slice region

New frozen body Active sketch to
Extrude Extrude with Slice operation
18
3D GeometryFeature Direction

• Direction

Direction is with respect to the sketch
plane Some operations (e.g. cut) result in
automatic change in direction
19
3D GeometryFeature Type

• Fixed
• Fixed extents will extrude the profiles the exact
  distance specified by the Depth property. The
  feature preview shows an exact representation of
  how the feature will be created

Fixed
20
3D GeometryFeature Type

• Through All Type will extend the profile through
  the entire model
• When adding material the extended profile must
  fully intersect the model

21
3D GeometryFeature Type

• To Next
• Add will extend the profile up to the first
  surface it encounters.
• Cut, Imprint, and Slice will extend the profile
  up to and through the first surface or volume it
  encounters

22
3D GeometryFeature Type

• To Faces allows you to extend the Extrude
  feature up to a boundary formed by one or more
  faces
• For multiple profiles make sure that each profile
  has at least one face intersecting its extent.
  Otherwise, an extent error will result
• The To Faces option is different from To
  Next. To Next does not mean to the next face,
  but rather through the next chunk of the body
  (solid or sheet)
• The To Faces option can be used with respect to
  faces of frozen bodies

23
3D GeometryFeature Type

• To Surface option is similar to To Faces, except
  only one face can be selected. The extent is
  defined by the underlying and possibly unbounded
  surface of the selected face (see below).
• In this case a single face is selected and its
  underlying surface is used as the extent. The
  underlying surface must fully intersect the
  extruded profile or an error will result.

Unbounded surface selected as extent
24
3D GeometryFeature Creation

• Extrusions
• Extrusions include solids, surfaces, and
  thin-walled features
• To create surfaces, select as thin/surface and
  set the inner and outer thickness to zero
• The active sketch is the default input but can be
  changed by selecting the desired sketch in the
  Tree View
• The Detail View is used to set the Extrude depth,
  direction, and Boolean operation (Add, Cut,
  Slice, Imprint, or Add Frozen)
• The Generate button completes the feature
  creation
• Note the previous section (Feature Type) shows
  various extrusion examples

To Create Surface
25
3D GeometryFeature Creation

• Revolve
• Active sketch is rotated to create 3D geometry
• Select axis of rotation from details
• If there is a disjoint (free) line in the sketch,
  it is chosen as the default axis of revolution
• Direction Property for Revolve
• Normal Revolves in positive Z direction of base
  object
• Reversed Revolves in negative Z direction of
  base object
• Both - Symmetric Applies feature in both
  directions. One set of angles will apply to both
  directions
• Both - Asymmetric Applies feature in both
  directions. Each direction has its own angle
  property
• The Generate button completes the feature creation

Sketch with Disjoint Line
26
3D GeometryFeature Creation

• Sweep
• Solids, surfaces, and thin-walled features can be
  created by using this feature to sweep a profile
  along a path
• Scale and Turns properties can be used to create
  helical sweeps
• Scale tapers or expands the profile along the
  path of the sweep
• Turns twists the profile as sweeps along the
  path
• A negative value for Turns will make the profile
  rotate about the path in the opposite direction.
  Turns Rotates counterclockwise
• See documentation for other restrictions
• Alignment
• Path tangent reorients the profile as it is
  swept along the path to keep the profile in the
  path's tangent direction
• Global the profile's orientation remains
  constant as it is swept along the path,
  regardless of the path's shape
• Examples . . .

27
3D GeometryFeature Creation

• Sweep example 1

Path Tangent alignment profile remains tangent
to path
Sketch1 profile to sweep
Sketch2 sweep path
Global Axes alignment profile orientation
remains constant
28
3D GeometryFeature Creation

• Sweep example 2

Sweep details Scale 0.5 Turns - 4
Sketch1 profile to sweep
Sketch2 sweep path

• Scale and Turns restrictions
• Scale The sweep path must be an open chain AND
  smooth
• Turns The sweep path must be smooth
• if the sweep path is a closed loop, then Turns
  must be an integer
• If the sweep path is an open chain, then any
  value for Turns is acceptable
• The default values for Scale and Turns are 1.0
  and 0.0 respectively

29
3D GeometryFeature Creation

• Skin/Loft
• Takes a series of profiles from different planes
  to create 3D geometry fitting through them (must
  select two or more profiles)
• A profile is a sketch with one closed or open
  loop or a plane from a face
• All profiles must have the same number of edges
• Open and closed profiles cannot be mixed
• All profiles must be of the same type
• Sketches and planes can be selected by clicking
  on their edges or points in the graphics area, or
  by clicking on the sketch or plane in the feature
  tree
• After selecting an adequate number of profiles, a
  preview will appear showing the selected profiles
  and the guide polygon
• The guide polygon is a gray poly-line which shows
  how the vertices between the profiles will line
  up with each other
• Skin/Loft operation relies heavily on RMB menu
  choices
• Examples . . .

30
3D GeometryFeature Creation

• Skin/Loft example 1
• Three 5 sided sketch profiles have been created
  on three offset planes
• After selecting each profile (hold CTRL key) the
  guide polygon is displayed
• RMB for guide polygon options
• Continue through all profiles

31
3D GeometryFeature Creation

• Skin/Loft example 1
• Add operation generates 3D solid
• Guide Polygons
• Use RMB options to realign if necessary
• Can result in unexpected shapes when misaligned

Result
32
3D GeometryFeature Creation

• Skin/Loft reordering
• During creation or when editing selections the
  order of the profiles may be adjusted
• Highlight profile to reorder and RMB
• Choose from options menu

33
3D GeometryFeature Creation

• Point Features
• The Point feature allows for controlled and fully
  dimensioned placement of points relative to
  selected model faces and edges
• Select a set of base faces and guide edges
• Select the Point (Analysis) Type
• Spot Weld Used for welding together otherwise
  disjointed parts in an assembly (only those
  points that successfully generate mates are
  passed as spot welds to Sim)
• Point Load Used for hard points (nodal ponts)
  in the analysis (all points successfully
  generated are passed to Sim as vertices
• Construction Point No points of this type are
  passed to Sim

Point Type
34
3D GeometryFeature Creation

• Select from three possible Point Definition
  options each with certain placement definitions
• Single Sigma and Offset
• Sequence By Delta Sigma, Offset, Delta
• Sequence By N Sigma, Offset, N, Omega
• From Coordinates File Formatted text file,
  similar to 3D curve (later)
• Sigma the distance between the beginning of the
  chain of guide edges and the placement of the
  first point
• Edge Offset the distance between the guide edges
  and the placement of the spots on the set of base
  faces
• Delta the distance, measured on the guide edges,
  between two consecutive points, for the Sequence
  By Delta option
• N the number of points to be placed, relative to
  the chain of guide edges, in case of the Sequence
  By N option
• Omega the distance between the end of the chain
  of guide edges and the placement of the last
  spot, for the Sequence By N option
• Some examples follow . . .

35
3D GeometryFeature Creation
Sequence by N placement options
Sigma
Base Face Guide Edge
36
3D GeometryFeature Creation
Sequence by Delta placement options
Guide Edge
Base Face
Delta
Above Guide edge 50 mm Delta 10 mm Note
all other placement options, Sigma, Omega, etc.
are the same as in the previous example
Points 6 (Guide edge/Delta beginning point)
37
Workshop 4-1, Catalytic Converter

• Goals
• Create the catalytic converter model shown below.
• Create separate sketches and perform a skin/loft
  operation to make the converter body.
• Use a Thin/Sheet operation to shell out the solid
  for future simulation.

38
Workshop 4-1, Catalytic Converter

• Use gtFilegtNew, or Launch ANSYS Workbench and
  choose to start New Geometry
• When prompted specify centimeters for length
  unit

39
Workshop 4-1, Catalytic Converter

• 3. Create the flange sketch 1 on XY Plane.
• Click on gtXYPlane in Tree
• Toolbar gtNew Sketch
• Sketch1 will be created on XYPlane
• In the Details view, rename Sketch1 to
  BaseCircle.
• Toolbar gtLook At
• Sketching gtDrawgtCircle
• Move the cursor over the sketch origin, then when
  the P is displayed (auto-constraint), click on
  the left mouse button. Click again to define the
  radius.
• Sketching gtDimensionsgtRadius
• Click on the circle to select it, then click
  again on the screen to define where to place the
  dimension.
• In the Details view, modify gtR1 to be 2.5.

40
Workshop 4-1, Catalytic Converter

• Create the flange sketch 1 (contd)
• Sketching gtModifygtSplit at Select
• Right click anywhere on the Model view and select
  Split Edge into n Equal Segments from the
  pop-up menu.
• The Split tool will now change to Split Equal
  Segments. Enter 8 for the textbox n.
• In the Model View, select the circle. It will
  now be split into eight segments.
• Notes
• In this step, we split and reoriented the
  circle.
• We will create the surfaces of the flange by
  lofting four sketches using this one as our
  basis.
• In order to do so, we must have the same number
  of divisions on each sketch, all oriented
  appropriately.

41
Workshop 4-1, Catalytic Converter

• Create the flange sketch 1 (contd)
• Sketching gtDraw
• Using the Box Select option, select the points
  and edges of the circle.
• Sketching gtModify gtMove
• In the text boxes next to the Move tool, change
  r to 22.5 and f to 1.
• Right-click on the Model View and select Use
  Plane Origin as Paste Handle. This will make
  the moving reference point as the original,
  relative location of the sketch origin.

42
Workshop 4-1, Catalytic Converter

• Create the flange sketch 1 (contd)
• Right click anywhere on the Model View and select
  Rotate by r Degrees. This makes the moving
  operation include a rotation, as specified by the
  value of 22.5 degrees entered earlier.
• Right click anywhere on the Model View and select
  Paste at Plane Origin.
• Right click, gtEnd
• This completes the move operation by moving the
  model to the origin.
• Since the reference point was the origin, this
  results in no translation but only a rotation,
  specified by r22.5.

43
Workshop 4-1, Catalytic Converter

• Create the flange sketch 1 (contd)
• On the Selection Toolbar, select the New
  Selection icon. Looking at the segments, one
  can see that they are now rotated 22.5 degrees.
• Using the Box Select option, select the points
  and edges of the circle. We will copy this sketch
  profile to be used for the next one.
• Sketching gtModify gtCopy
• Click on the Copy tool to copy this profile.
• Right-click anywhere on the Model View and select
  Use Plane Origin as Paste Handle to make the
  paste operation use the original, relative
  location of the sketch origin as the pasting
  point.

44
Workshop 4-1, Catalytic Converter

• 4. Create the flange sketch 2
• Toolbar XYPlane
• Toolbar gtNew Plane
• Select the New Plane icon from the Active
  Plane/Sketch Toolbar. This creates Plane4 based
  on XYPlane.
• In the Details view, create an Offset Z and set
  FD1 to 1.
• Toolbar Generate
• Sketching gtModifygtPaste
• Enter 0 for r and 1.05 for f.
• Right-click anywhere on the Model View and select
  Scale by factor f. This will scale the
  original sketch profile by a factor of 1.05 for
  our new sketch.

45
Workshop 4-1, Catalytic Converter

• Create the flange sketch 2 (contd)
• Right-click on the Model View and select Paste
  at Plane Origin. Our reference point was the
  sketch origin from BaseCircle, and the pasting
  location is the origin on Sketch2, so this
  essentially copies the original circle onto
  Sketch2 with a scale factor of f1.05.

46
Workshop 4-1, Catalytic Converter

• Create the flange sketch 2 (contd)
• In Tree, Click on gtBaseCircle
• Right-click on BaseCircle and select Keep
  visible
• In Tree, Click on gtPlane4 gtSketch2
• Right-click on Sketch2 and select Keep Visible.
  
• This keeps both sketches visible so we can easily
  see that one circle is the same as the other
  except for the Z offset and the 1.05 scale
  factor.

47
Workshop 4-1, Catalytic Converter

• 5. Create the flange sketch 3
• Toolbar XYPlane
• Toolbar gtNew Plane
• Select the New Plane icon from the Active
  Plane/Sketch Toolbar. This creates Plane5 based
  on XYPlane.
• In the Details view, create an Offset Z, and set
  FD1 to 5.
• Toolbar Generate
• Sketching gtDraw gtRectangle
• Check Auto-Fillet checkmark next to the Rectangle
  tool.
• Click once to define one corner of the rectangle,
  click again to define its diagonal, and click a
  third time to define the fillet radius.

48
Workshop 4-1, Catalytic Converter

• Create the flange sketch 3 (contd)
• Sketching gtDimensions gtGeneral
• Dimension the sketch as shown at right.
• In the Details view, change Dimensions gt H1 to
  10, L4 to 10, L5 to 6, R3 to 5, V2 to
  2.
• Using the Box Select option, select the points
  and edges of the flange on Sketch3.
• We will copy this sketch profile to be used for
  the next one.
• Sketching gtModify gtCopy
• Right-click anywhere on the Model View and select
  Use Plane Origin as Paste Handle.

49
Workshop 4-1, Catalytic Converter

• 6. Create the flange sketch 4
• Modeling gtConverter gtPlane5
• Toolbar New Plane
• Select the New Plane icon from the Active
  Plane/Sketch Toolbar. This creates Plane6 based
  on Plane5.
• In the Details view, create an Offset Z, and set
  FD1 to 1.
• Toolbar Generate
• Sketching gtModify gtPaste
• Enter 0 for r and 1.05 for f. Right-click
  anywhere on the Model View and select Scale by
  factor f. (scales the original sketch profile
  by a factor of 1.05).
• Right-click on the Model View and select Paste
  at Plane Origin. Our reference point was the
  sketch origin from Plane5, and the pasting
  location is the origin on Plane6, so this copies
  the rectangle onto Plane6 and scales it by 1.05.

50
Workshop 4-1, Catalytic Converter

• Create the flange sketch 4 (contd)
• Modeling gtConverter gtPlane5 gtSketch3
• Right-click on Sketch3 and select Keep Visible
• Modeling gtConverter gtPlane6 gtSketch4
• Right-click on Sketch4 and select Keep Visible.
  This makes both sketches visible at the same
  time, so we can easily see that the original
  profile is indeed scaled by a factor of 1.05.

51
Workshop 4-1, Catalytic Converter

• 7. Create the flange
• Toolbar Skin/Loft
• Select the Skin/Loft icon
• and the Details view, Profiles should be active.
• Hold the CTRL key and, from the graphics window
  select the four edges shown at the right in the
  direction noted by the solid arrow. They will
  highlight in yellow.
• Note it is only necessary to select one line
  from each sketch.
• Apply
• A grey line appears showing the lofting behavior.
  In this case, the lofting is not correct, as it
  will twist the geometry. If your grey line
  does not seem correct, this can be resolved by
  right-clicking anywhere on the Model View and
  selecting Fix Guide Line.

52
Workshop 4-1, Catalytic Converter

• Create the flange (contd)
• Select the two top edges that the arrows point to
  on the top-right image. This redefines the
  lofting guide such that the model will not
  twist.
• After selecting the two edges, the guiding
  profile, shown in grey, is now defined correctly
  as shown in the bottom-right image.

53
Workshop 4-1, Catalytic Converter

• Create the flange section (contd)
• Toolbar Generate
• The resulting solid is plotted.
• Toolbar View gtWireframe Display
• The wire frame display is shown below.
• Toolbar View gtShaded Display
• Modeling gtConvertergtXYPlanegtBaseCircle
• Right-click on BaseCircle and select Dont keep
  visible
• Repeat the above command to turn off Sketch2,
  Sketch3, and Sketch4

54
Workshop 4-1, Catalytic Converter

• 8. Create the pipe bend
• Modeling gtConverter gtXYPlane
• Toolbar New Sketch
• Sketch5 will be created on XYPlane
• Choose the Look At icon
• In the Details view, rename Sketch5 to
  RevolveAxis.
• Sketching gtDraw gtLine
• Create a single line as shown on the
  bottom-right. Make sure it has an
  auto-constraint of V (vertical).
• Sketching gtDimensions gtGeneral
• Dimension the distance of the line from the
  vertical axis as 15.

55
Workshop 4-1, Catalytic Converter

• Create the pipe bend (contd)
• Modeling gtConverter gtXYPlane gtBaseCircle
• Toolbar Revolve
• In the Details view, the Base Object should be
  set to BaseCircle.
• Add RevolveAxis as the Axis by selecting the
  line and then pick Apply.
• Look at the Model View. The revolution operation
  is in the wrong direction, so change Direction to
  Reversed with the pull-down menu.
• Change FD1, Angle (gt0) to 45. The revolve
  preview should look similar to the top-right
  image.
• Toolbar Generate
• This will generate the pipe bend.
• Select the end circular surface for our next step.

56
Workshop 4-1, Catalytic Converter

• 9. Create the pipe end
• Make sure the end circular surface is highlighted
  (from step 8).
• Sketching gtDraw gtCircle
• A new sketch is automatically created. Create a
  circle the same size as the end circle of the
  pipe bend. Use of auto-constraints, as shown on
  the top-right image, will ensure that the circle
  sketch will match the end surface.
• Toolbar Extrude
• In the Details view, change FD1, Depth (gt0) to
  10
• Toolbar Generate
• The straight end of the pipe should be generated.

57
Workshop 4-1, Catalytic Converter
Surface 1

• Create the pipe end (contd)
• Select the 2 end surfaces (see right)
• Create a Surface model
• Toolbar Thin/Surface
• In the Details view, change Selection Type to
  Faces to Remove and FD1, Thickness (gt0) to 0
• Toolbar Generate
• The result is a surface model that can be meshed
  using shell elements during FE simulation.

Surface 2
58
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