Create Complex Surfaces

Transcription

1 Create Complex Surfaces In this lesson, you will be introduced to the functionalities available in the Generative Surface Design workbench. Lesson content: Case Study: Surface Design Design Intent Stages in the Process Create the Complex Surface Geometry Perform Fillet Operations Duration: Approximately 0.5 day 8-1

2 Case Study: Surface Design The case study for this lesson is a simplified B pillar. The chassis section is a part of the Cradle frame sub-assembly. The case study focuses on creation of surface features and performing surface operations that incorporate the design intent of the part. 8-2

3 Design Intent The model of the simplified B pillar must meet the following design intent requirements: The main junction surface (A) must pass through the four section curves. Create a multi-sections surface passing through the four section curves. Length of the base junction surface (B) must be 700mm. Create an extrude of Base_Junction_Curve. Sharp edges must not be present between the main junction surface and the base junction surface. Trim the surfaces and create an edge fillet of radius value 100mm. The front pillar surface (C) and the back pillar surface (D) must pass through the respective guide curves. Create sweep surfaces passing through two guide curves. The result must be a single surface. Move the final surface to the Result geometrical set. C A D B 8-3

4 Stages in the Process Use the following steps to create the model of the simplified B pillar: Create a Multi-Section surface. 2. Fill the surface and create a join. 3. Create an extruded surface. 4. Apply fillets to the sharp edges Create a sweep. 6. Join the surfaces to get a single result

5 Create the Complex Surface Geometry In this section, you will learn some to the common tools used to create surface geometry. Use the following steps to create the simplified B pillar: 1. Create the Complex Surface Geometry 2. Perform Fillet Operations 8-5

6 Computation of Sweep Sweep is a surface generated by sweeping a profile along a guide curve with respect to a spine. The profile can be a user-defined or pre-defined profile. Sweeping a profile along a guide curve with respect to a spine means, Spine Guide The Planes are calculated in regards to the tangent to the spine and to the mean plane of the spine. The sweep profile is repeated on these planes along the guide curve. Then a surface is swept passing through these profiles. This surface is the sweep (or swept surface). Profile Surface passing through the repeated sections Profiles repeated in the planes 8-6

7 Creating Swept Surface Explicit Subtype Swept Surfaces are created by sweeping a profile along a spine. The spine, by default, is the first selected guide curve. 1 Use the following steps to create a simple explicit type Swept Surface: 1. Select the Swept Surface icon. 2. Select the profile. 3. Select a guide curve. 4. Click OK to complete the feature

8 Creating a Swept Surface Reference Surface Option By default, a Swept Surface uses the mean plane of the spine as the surface the profile is swept along. A user-defined surface can also be used. 2 1 Use the following steps to apply a reference surface to a Swept Surface feature: 3 1. Select the With Reference Surface option from the dialog box. 2. Select the surface. 3. Enter an angle. This angle is measured between the profile and the reference surface

9 Creating a Swept Surface Second Guide Explicit swept surfaces can also be created using a second guide curve. 1 Use the following steps to add a second guide curve to a Swept Surface feature: 1. From the Subtype menu, select the With two guide curves option. 2. Select the profile. 3. Select the first guide curve. This guide curve, by default, will also act as the spine. 4. Select the second guide curve. 5. Click OK to generate the feature

10 Creating a Swept Surface - Spine A Spine can control the orientation of the profile as it sweeps along the guide curve(s). By default the first guide is used as the spine for the Swept feature. 1 If required, another element can be selected to act as the Spine. Use the following steps to change the spine: 2 1. Click on the Spine field. 2. Select the new element. 8-10

11 Creating a Swept Surface - Relimiters By default, the Swept Surface will be created along the total length of the spine. Using points or planes the surface can be longitudinally reduced. 1 2 Use the following steps to relimit the swept surface: 1. Click on the Relimiter 1 field. 2. Select the relimiting element. In this example, a point is selected. 3. Click on the Relimiter 2 field. 4. Select the second relimiting element. In this example, a plane is selected

12 Creating an Offset Surface (1/2) Use the Offset tool to create a surface offset from an existing surface. 1 Use the following steps to create an Offset Surface: 1. Select the Offset icon. 2. Select the reference surface. 3. Enter offset value. 4. If necessary, select Reverse Direction to change the direction of the offset. 5. Use the Both sides option to create offset surfaces on either side of the reference surface. 6. Select Repeat object after OK to create several surfaces separated by the same offset distance

13 Creating an Offset Surface (2/2) Use the following steps to create an Offset Surface (continued): 7. Click OK. 8. When the Repeat object after OK option is selected the Object Repetition dialog box appears. Enter the number of instances to be created. 9. The new instances will be created in a new open body. To create the instances in the existing open body, clear the Create in a new Open Body option. 10. Click OK to create the surfaces. The resulting offset surface is parallel to the reference surface. Side View

14 Creating a Fill Surface (1/2) Use the Fill Surface tool to create a surface inside a closed boundary. The boundary can consist of wireframe elements or edges of existing surfaces. 1 2a 2b 2c Use the following steps to create a fill surface: 1. Select the Fill icon. 2. Select the edges that will form the boundary. 3. Tangency can be applied at any boundary, by selecting the boundary from the Fill Surface Definition box and selecting the support surface. In this example tangency is applied to the last boundary. 4. Specify the type of continuity between the support surface and the fill surface. In this example Tangent continuity is selected. 3a 3b 2d

15 Creating a Fill Surface (2/2) Use the following steps to create a fill surface (continued): 5 5. If necessary, define a point though which the surface will pass. 6. If necessary, edit the boundary by adding additional elements to the boundary, replace or remove existing elements or support surfaces. 7. Click OK to generate the surface

16 Creating a Blend Surface (1/4) A blend surface is used to create a surface between two wireframe elements. 1 Use the following steps to create a blended surface: 1. Select the Blend icon. 2. Select the first curve. 3. If required, select the support for the first curve. 4. Select the second curve. 5. If required, select the support for the second curve

17 Creating a Blend Surface (2/4) Use the following steps to create a blended surface (continued): 6. If supports are specified, define the type of continuity for each side. Continuity can be defined as: a. Point b. Tangency c. Curvature 7. If required, select the Trim Support options. When selected, the support surfaces are trimmed to the curve and are assembled into the blended surface a 6b 6c 8-17

18 Creating a Blend Surface (3/4) Use the following steps to create a blended surface (continued): 8. If supports are specified, you can define tangency between the blended surface borders and the support surface borders. Tangency can be defined as: a. Both extremities b. None c. Start Extremity only d. End extremity only 8a 8b 8c First border Second support First support Second border 8d 8-18

19 Creating a Blend Surface (4/4) Use the following steps to create a blended surface (continued): 9. If required, specify tension at the blend surface limits. Tension can be specified as: a. Default b. Constant c. Linear d. S type 10. Click OK to generate the blend surface. 9 Changing Tension Surface 1 T4 T3 T2 T1 T1 Constant Surface

20 Blend Surface: Curves Orientation The curves used must be oriented in the same direction: One of the curves is oriented differently (use the arrow) You get a twist: Beware the curves orientation 8-20

21 Blend Surface: Coupling points Define how to get from one curve to the other using coupling points: Vertices and points correspondence Coupling points defined Without Coupling points definition 8-21

22 Creating a Multi-Sections Surface (1/6) A surface is computed by passing through two or more consecutive sections along a spine is called Multi-Section surface. The shape of the Multi-Section surface can be defined more precisely by specifying the sections. Guide curves Adjacent Surface During a certain design situation, you may need a shape which varies in its cross-section along its length. In such case you can create Multi-Section surface which passes through the defined sections along the spine or guides. Multi-Section surface helps you to attain a smooth transition surface between two or more varying sections and at the same time maintains the G1 continuity with adjacent surfaces. Adjacent Surface Sections curves 8-22

23 Creating a Multi-Sections Surface (2/6) Section are the user-defined profile. A section can be a 2D or a 3D curve. It is an elementary input to create a Multi-Section Surface. A Multi-Section surface passes through the set of consecutive sections to inherit their shape. Section Curves The Guide curve defines the path for the surface to transit between two sections. The guide curve is a point continuous curve and intersects with each consecutive section of a Multi- Section surface. Guide Curve Guide Curve to give the correspondence between these 2 vertices Section Curves 8-23

24 Creating a Multi-Sections Surface (3/6) Use the following step to create a Multi-Section Surface using other options (Guides, Spine, Relimitation, Canonical elements) 1 1. Select the Multi-Sections Surface icon. 2. Select the first section, second section and third section. 3. Select tangent surfaces for first and last section. 4. Ensure that the orientation of all the sections at closing points is same

25 Creating a Multi-Sections Surface (4/6) 5. In the Guides tab, select the guide curves. The resulting surface will respect these guide curves. 6. You can Replace, Remove or Add the guides during the edition of Multi-sections surface

26 Creating a Multi-Sections Surface (5/6) 7. In the Spine tab, select the spine. By default the spine is calculated automatically. The spine must be tangent continuous. 8. You can Replace, Remove or Add the spine during the edition of Multi-sections surface

27 Creating a Multi-Sections Surface (6/6) 9. In the Coupling tab, select Ratio type. Depending on the sections configuration, you can select the suitable coupling type In the relimitation tab, you can choose to limit the Multi-sections Surface only on the Start section, only on the End section, on both, or on none. By default the multi-sections surface is relimited at start and end sections

28 Exercise: Complex Surfaces Creation Recap Exercise 20 min In this exercise, you will open an existing model and use the tools learned in this lesson to create a surface geometry necessary for the shell of a car door panel. To save time, simple wireframe and surface elements have already been created for you. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a Swept surface Create a Connect curve Create a Projection Create a Boundary Create a Multi-Sections surface 8-28

29 Do it Yourself (1/11) 1. Load Ex8A.CATPart. Load Ex8A.CATPart. This part already has some curves and surfaces created for you. a. Notice all the wireframe elements have been created in a separate geometrical set. b. Ensure that the Surfaces geometrical set is active. 2a 2b 2c 2d 2e 2. Create a swept surface. Create a swept surface from a given profile and guide curve. This surface would form the inner panel of the door. a. Click the Sweep icon. b. Select Explicit option. c. Select subtype With Two Guide Curves. d. Select Profile as Section_1. e. Select Guide curve 1 as Parallel.1 f. Select Guide curve 2 as an edge of the OUTER PANEL WITH FLANGE. 2f 8-29

30 Do it Yourself (2/11) 2. Create a swept surface (continued). g. Select anchoring type as Two Point h. Select the first anchor point at the intersection of the profile and first guide curve. i. Select the second anchor point at the intersection point of the profile and second guide curve. j. Select Relimiter 1 as Plane.4. k. Select Relimiter 2 as Plane.1. 2j 2k Profile Relimiter 1 Anchor Point 2 Guide Curve 1 Guide Curve 2 Anchor Point

31 Do it Yourself (3/11) 2. Create a swept surface (continued). l. Click OK to create a swept surface. Sweep.1 Start point End point 8-31

32 Do it Yourself (4/11) 3. Create a second swept surface. Create a swept surface from a given profile and guide curve. This surface would form inner panel of the door. a. Click the Sweep icon. b. Select Explicit option. c. Select subtype With Two Guide Curves d. Select Profile as Section_2. e. Select Guide curve 1 as Parallel.2. f. Select Guide curve 2 as an edge of the OUTER PANEL WITH FLANGE. 3a 3b 3e 3d 3c 3f Relimiting Planes Guide Curve 2 Guide Curve 1 Profile 8-32

33 Do it Yourself (5/11) 3. Create a second swept surface (continued). g. Select anchoring type as Two Points h. Select the first anchor point at the intersection of the profile and first guide curve. h. Select the second anchor point at the intersection point of the profile and second guide curve. i. Select Relimiter 1 as Plane.3. j. Select Relimiter 2 as Plane.2. 3g 3h Guide Curve 2 Profile Anchor Point 2 Guide Curve 1 Anchor Point 1 Relimiter

34 Do it Yourself (6/11) 3. Create a second swept surface (continued). k. Click OK to create a swept surface. Sweep.2 End point Start point 8-34

35 Do it Yourself (7/11) 4. Create a 3D Guide curve. Create a connect curve between the two end sections of the swept surface created in previous steps. This curve would be later projected on the panel surface and used as a guide curve to create a Multi-Sections surface. a. Click the Connect Curve icon. b. Select the vertex of the first section (as shown). c. The default curve is automatically selected. d. Specify the tension value to 3. e. Select the vertex of the second section (as shown). f. The default curve is automatically selected. g. Keep the tension value as default. h. Click OK to create a connect curve. 4a 4b 4c 4d First Curve 4e 4f First Point 4g Second Curve Second Point 4h 8-35

36 Do it Yourself (8/11) 5. Project the curve Project the connect curve on the panel surface (Blue surface). Later you would use this projection as guide curve to create Multi- Sections surface a. Click the Project icon. 5a b. Select the connect curve to be projected. c. Select the OUTER PANEL WITH FLANGE surface (Blue surface) as support. d. Select ZX plane as projection direction. e. Click OK to create projection. 5b 5d 5c 5e Projected Curve Connect Curve 8-36

37 Do it Yourself (9/11) 6. Create a boundary. Create a boundary of the swept surfaces. These boundaries would be later used as section curves to create Multi-Sections surface between two swept surface. a. Click the Boundary icon. b. Specify the propagation type as Point continuity. c. Select the edge of the swept surface (as shown). d. Select first and second limit on the highlighted curve. 6a 6e 6c 6b 6d e. Click OK to create a boundary curve. Repeat the step to create a boundary for Sweep.1 surface. Boundary Sweep.1 Boundary Sweep

38 Do it Yourself (10/11) 7. Create a Multi-Sections surface. 7a Create a Multi-Sections surface between the two swept surfaces. a. Click the Multi-Sections surface icon. b. Select the boundary of the first swept surface. c. Select the first swept surface as Tangent. d. Select the boundary of the second swept surface. e. Select the second swept surface as Tangent. f. Select Project.1 as first Guide. g. Select an edge of the OUTER PANEL WITH FLANGE as second Guide (as shown). 7i h. Click on Coupling tab, Choose coupling type as Vertices. 7h 7c 7b 7d 7e 7f 7g 8-38

39 Do it Yourself (11/11) 7. Create a Multi-Sections surface. i. Click OK to create a Multi-Sections surface. 8. Close the part without saving it. Multi-section Surface Sweep.1 Sweep

40 Exercise Recap: Complex Surfaces Creation Create a Swept surface Create a Connect curve Create a Projection Create a Boundary Create a Multi-Sections surface 8-40

41 Exercise: Multi-Sections Surface Recap Exercise 10 min In this exercise, you will open an existing model consisting of wireframe and surface inputs. You will practice how to use the Multi-Sections surface tool. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a Multi-Sections surface. 8-41

42 Do it Yourself (1/2) 1. Load Ex8B.CATPart. Load Ex8B.CATPart. This part already has some curves and surfaces created for you. a. Observe that the two sections (flat and formed sections) are in different geometrical sets. b. Create a geometrical set called Multi- Section. 2. Create a Multi-Sections surface. Create a Multi-Sections surface from a given profile. Use manual coupling to guide the surface. Coupling Points Multi-Section Surface 8-42

43 Do it Yourself (2/2) 3. Hide the Multi-Sections surface created in the previous step. Connect Curve 4. Create the Guide curves. Create the guide curves between the two sections as shown. 5. Create a Multi-Sections surface. Create a Multi-Section surface from a given profile. Use the guide curves created in the previous step. Line 6. Close the part without saving it. 8-43

44 Exercise Recap: Multi-Sections Surface Create a Multi-Section Sweep using coupling points Create Multi-Section surface using guide curves Create a Multi-Section Sweep using coupling points Create a Multi-Section Sweep using guide curves 8-44

45 Exercise: Complex Surfaces Creation Recap Exercise 20 min In this exercise, you will create a thermal insulation cover using simple surfaces. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a Multi-Sections surface Create a Sweep surface Create an Extrude surface Create a surface Trim 8-45

46 Do it Yourself (1/4) 1. Load Ex8C.CATPart. Load Ex8C.CATPart. This part already has some curves created for you. 2. Analyze the model Study the model along with the specification tree to understand the sequence of the model construction. 8-46

47 Do it Yourself (2/4) 3. Create a main surface In Geometrical Set BASE SECTIONS, create Multi-Sections surface using section 1 and 2 as Profiles and Vertices as the coupling option. Multi-Section using Vertices option 4. Create rounded front wall In Geometric Set Rounded Surface, create a sweep surface as shown using Profile and Guide. Display the Split planes in the Start data Geometrical Set. Specify these planes as Relimiter 1 and 2 in the Sweep dialog box. 8-47

48 Do it Yourself (3/4) 5. Create upper Split surface In Geometric Set Split upper Surface create an extruded surface as shown. In Geometric Set Rounded Surface create the split as shown. Extrude Split Split Rounded Wall 8-48

49 Do it Yourself (4/4) 6. Create Final surface Create a Geometrical Set called Screen under the father node of the thermal screen. Create a trim between the main surface and the front wall surface Rename the trim surface as Screen. 7. Close the part without saving it. 8-49

50 Exercise Recap: Complex Surfaces Creation Create a Multi-Sections surface Create a Sweep surface Create an Extrude surface Create a surface Trim 8-50

51 Perform Fillet Operations In this section, you will learn how manipulate the surface geometry to create the final surface model. Use the following steps to create the simplified B pillar : 1. Create the Complex Surface Geometry 2. Perform Fillet Operations 8-51

52 Why Are Operations on Geometry Needed? After the basic surface geometry is created, it may be composed of construction elements that do not describe the finished shape. Operations such as trim, join, extrapolate, and transform are then performed to produce the required finished geometry. While performing operations, keep in mind the following key points: A. Operations are used to produce the finished geometry. Surface fillet operation B. Elements involved in an operation are kept in the history of the operation, but are hidden. Join Operation 8-52

53 Why Do You Need Joining Elements? Join operation is used when you want to concatenate or logically group the adjacent surfaces/wireframes together into a single element that can be used for future operations. It is a mechanical assembly of curves or surfaces to form a single entity in the tree. Advantages: 1. Only one feature to select in the tree 2. Some CATIA tools require only one element as input, in such cases Join operation can be selected. Bottle Top Bottle Body Bottle Bottom 8-53

54 Joining Elements Use the following steps to join elements: 1. Click the Join icon. 2. Select the elements to be joined. 3. Set options as necessary. a. When the Check tangency option is selected, the join feature will only be created if all elements to be joined are tangent. b. When the Check connexity option is selected, the join operation will only be performed if the elements to be joined are connected. c. The Simplify the result option reduces the number of resulting elements. d. The Ignore erroneous elements option ignores the elements that do not allow the join to be created. e. The Merging distance is the maximum distance below which two elements are considered as one. 3a 3c 3d 4 3e 3b 2a 1 4. Click OK to complete the feature. 2b 8-54

55 Joining Elements Exclude Sub-Elements While joining elements you can exclude some sub-elements from the joined surface. Use the following steps to exclude subelements: 1. Select the elements to be joined. 2. Select the Sub-Elements to Remove tab to exclude sub-elements from the joined surface. 3. Select the elements to exclude. 4. Check the Create join with subelements option to create a second join surface with the excluded sub-elements b 1a

56 Why Use Fillets? Fillets are used to remove sharp edges on the parts. Fillets, along with drafts, help to easily remove the material from molds. Fillets also help in reducing stress concentration in the parts. 8-56

57 Fillet Extremities By creating fillets using surfaces, you can have a better control on the resulting elements. For example, the connection between the fillet and the support surface(s) can be customized to create the desired geometry. There are four options available to control the extremities of a fillet: A B A. The Smooth option connects the fillet surface to the support surface with a tangency constraint. B. The Straight option connects the fillet with no tangency constraints. C. The Maximum option extends the fillet to the longest selected support edge. D. The Minimum option trim the fillet to the shortest selected support edge. C D 8-57

58 Fillet Propagation By selecting a propagation mode, the edge on which fillet has to be created can be propagated automatically. There are three options available to control the propagation of a fillet: A A. The Minimal option creates the fillet only on the selected edge. B. The Tangency option propagates the fillet to all adjacent tangency continuous edges. B Selected edge Fillet created on selected edge C. The Intersection Edges option propagates the fillet to all the edges that have been generated by intersecting the features Selected edge Fillet propagated on adjacent tangent continuous edges C Selected edge Fillet propagated on edges generated by intersection 8-58

59 Creating a BiTangent Shape Fillet Shape fillets are used to create a fillet between two surfaces. Use the following steps to create a BiTangent shape fillet: 1 1. Click the Fillet icon. 2. Select the two surfaces/faces. 3. Enter the radius value. 4. Ensure the red arrows point towards the concave side for the fillet. If not, select on the arrow to change its direction. 5. Specify the Extremities conditions. 6. Clear the Trim Support options so that the supporting elements 7. do not assemble into the fillet feature. 8. Click OK to create the shape fillet

60 Creating an Edge Fillet The Edge Fillet tool is used to provide a transitional surface along a sharp edge of a surface. Similar to the Edge fillets in the Part design workbench, here also you can select edges or faces to be filleted. 1 Use the following steps to create an edge fillet: 3 1. Click the Edge fillet icon. 2. Select the edge(s) of the surface to be filleted. 3. Enter the radius value. 4. Specify extremity conditions. 5. Click OK to generate the edge fillet

61 Creating a Variable Radius Fillet (1/2) Use the Variable Radius Fillet tool to create a fillet on a selected edge whose radius varies at selected points. 1 Use the following steps to create a variable radius fillet: 2 1. Click the Variable Fillet icon. 2. Select one or more internal edges of a single surface. 3. To add additional points, click inside the Point field then select anywhere on the edge to place the point, or select a preexisting point for better accuracy. 4. Double-click on a radius value to modify it

62 Creating a Variable Radius Fillet (2/2) Use the following steps to create a variable radius fillet (continued): 5. Select the Variation as Cubic. A Cubic variation helps in the smooth transition of one radius into another, while the Linear variation helps in linear transition as shown. 6. Click OK to complete the fillet. Cubic mode Linear mode

63 Creating a Face-To-Face Fillet The Face-Face fillet is used when there is no intersection between the selected faces or when there are more than two sharp edges between the faces. 1 Use the following steps to create a face-face fillet: 1. Click the Face-Face icon. 2. Select the two faces. The fillet is created between these faces. The selected faces must belong to the same surface. 3. Enter a radius value. 4. Click OK to create the fillet

64 Creating a Tritangent Fillet A Tritangent fillet creates a transitional surface by removing one of three selected surface. The fillet surface is created tangent to the three selected faces. 1 Use the following steps to create a Tritangent fillet: 2 1. Click the Tritangent Fillet icon. 2. Select the two faces to keep. 3. Select the face to remove. 4. Click OK to complete the feature

65 Boundary Curves Use the Boundary tool to create boundary curves of internal or external surface edges. While defining the boundary, only one element needs to be selected. Using the correct propagation type, the remaining boundary is automatically determined. The propagation of a selected edge can be defined by: A A. Using the Complete boundary option, the selected edge is continued about the entire surface boundary. B B. Using the Point continuity option, the selected edge is continued about the surface boundary until a point discontinuity is met. C. Using the Tangent continuity option, the selected edge is propagated about the surface boundary until a tangent discontinuity is met. D. Using the No propagation option only the selected edge is used to create the boundary curve. C D 8-65

66 Creating Boundary Curves Use the Boundary tool to create boundary curves of internal or external surface edges. Use the following steps to create a boundary curve: 1 1. Click the Boundary icon. 2. Specify the propagation type. 3. Select the surface edge. 4. If necessary, limit the boundary curve using points or vertices. a. Select in the Limt1 field b. Select the first limiting element c. Select in the limit2 field d. Select the second limiting element 5. Click OK to generate the boundary curve a 2 4c 4b 4d 8-66

67 Extracting an Edge from a Surface The Extract tool is used to extract subelements from a surface. Edges and surface faces can be extracted from the original surface. 1 To extract an edge from a surface use the following steps: 2 1. Click the Extract icon. 2. Select a surface edge. 3. Specify the propagation type. In this example, Tangent continuity is selected. 4. Click OK to complete the extraction

68 Extracting a Face from a Surface You can also use the Extract tool to extract one or several faces of a surface with or without propagation. The same operations can be performed on solids using the extract tool. 1 Use the following steps to extract a face from a surface. 1. Click the Extract icon. 2. Select the face. 3. Specify the propagation type. In this example Point continuity is selected. 4. Click OK to complete the extraction

69 CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces To Sum Up In the following slides you will find a summary of the topics covered in this lesson. 8-69

70 Creating the Complex Surface Geometry Sweep is a surface generated by sweeping a profile along a guide curve with respect to a spine. The profile can be a user-defined or pre-defined profile. A Spine can control the orientation of the profile as it sweeps along the guide curve's. By default the first guide is used as the spine for the Swept feature. Complex surfaces can be created by following commands: Creating an Offset Surface: The new instances will be created in a new open body. Creating a Fill Surface: Surface can be filled inside closed boundary. Creating a Blend Surface: A blend surface is used to create a surface between two wireframe elements. Creating a Multi-Section Surface: A surface is computed by passing through two or more consecutive sections along a spine is called Multi-Section surface. 8-70

71 Perform Fillet Operations After the basic surface geometry is created, it may be composed of construction elements that do not describe the finished shape. Operations such as trim, join, extrapolate, and transform are then performed to produce the required finished geometry. Join operation is used when you want to concatenate or logically group the adjacent surfaces/wireframes together into a single element that can be used for future operations. Fillets are used to remove sharp edges on the parts. The Edge Fillet tool is used to provide a transitional surface along a sharp edge of a surface. 8-71

72 Main Tools Operations Join: logically fills the gap between two surfaces. Boundary: creates boundary curves of internal or external surface edges. Extract: creates an extract sub elements from a surface Surfaces 4 Offset: creates a surface offset from an existing surface. 5 Sweep: creates a surface by sweeping a profile along a spine. 4 6 Fill: creates a surface inside a close boundary Multi-section surface: creates a surface passing through two or more consecutive sections along spine. Blend: creates a surface between two wireframe elements

73 Exercise: Surfaces Operations Recap Exercise 20 min In this exercise, you will create a stamp feature on the thermal insulation cover using the surface tools. During the creation, you will practice the tools learnt in the previous steps. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a Revolve surface Create a surface Boundary Create a Fill surface Create a Join between surfaces Create a surface Trim Create a Fillet between surfaces Create a pre-defined Cylinder surface Create an Intersection curve Create a Split surface 8-73

74 Do it Yourself (1/10) 1. Load Ex8D.CATPart Load Ex8D.CATPart. This part already has some curves and surface created in the previous exercise. a. Observe that the sketches required to create the surface data are provided in the model. b. You will be creating the surface in the respective geometrical sets while performing the steps. c. Study the model along with the specification tree to understand the sequence of the model construction. 8-74

75 Do it Yourself (2/10) 2. Create the Stamp Define in work object the Stamp Geometrical set. Show the Geometrical Set Stamp Balance. Create a Revolve surface from the sketch and stamp axis. a. Click the Revolve icon b. Select Stamp_Sketch as profile c. Select Stamp Axis as axis. d. Click OK to create a revolve surface. Hide all the sketches and the Geometrical Set Stamp balance. 2a 2d 2b 2c 8-75

76 Do it Yourself (3/10) 3. Create the upper boundary of Stamp Create the upper boundary of stamp surface. a. Click the Boundary icon b. Select upper edge of the surface as shown c. Click OK to create a boundary. 3a 3c 3b 4. Create the upper surface of Stamp Create the upper surface of stamp by filling the boundary created in the previous step. a. Click the Fill icon b. Select the upper boundary of the surface as shown c. Click OK to create a fill surface. d. Hide the upper boundary of the stamp surface. 4a 4b 4c 8-76

77 Do it Yourself (4/10) 5. Assemble the surfaces Join the Revolve and Fill surfaces. a. Click the Join icon b. Select the revolve surface c. Select the fill surface d. Click OK to join the surfaces 5a 5b 5c 5d 8-77

78 Do it Yourself (5/10) 6. Merge the stamp surface with Screen surface Trim the Stamp and Screen surface. a. Click the Trim icon. b. Select the Stamp surface. c. Select the Screen surface. d. Select the Other side option to keep the required surface. e. Click OK to trim the surface. 6a 6b 6c 6d 6e 8-78

79 Do it Yourself (6/10) 7. Blend the sharp edges. Create an edge fillet on the intersecting edge. Specify the parameters as follows a. Click the Fillet icon b. Select the intersecting edge. c. Specify the fillet radius as 10mm d. Click OK to create a fillet. e. Click the Fillet icon. f. Select the intersecting edge. g. Specify the fillet radius as 5mm h. Click OK to create a fillet. 7a 7d 7c 7b 7e 7g 7f 7h 8-79

80 Do it Yourself (7/10) 8. Rename the surface as Stamp Screen Rename the surface as Stamp Screen a. Right-click the last filleted surface. b. Select Properties c. In the Feature Properties tab, specify the name as Stamp Screen. d. Click OK to rename the surface. 8a 8b 8c 8d 8-80

81 Do it Yourself (8/10) 9. Create a pass cut for a flexible device Show the Geometrical Set stamp Balance. Create a Cylinder. a. Click the Cylinder icon b. Select the axis extremity as point input. c. Select the axis as direction d. Specify the radius equal to 6.5mm e. Specify the length equal to 100mm at both the sides f. Click OK to create a cylinder. 9a 9c 9e 9b 9d 9f 8-81

82 Do it Yourself (9/10) 10. Creating an intersecting curve Create an intersection curve between the Cylinder and Stamp Screen surface a. Click the Intersection icon. b. Select the Cylinder surface. c. Select the Stamp Screen surface. d. Click OK to create an intersecting curve. 10a 10b 10c 10b 10c 10d 8-82

83 Do it Yourself (10/10) 11. Create a passing hole on the Stamp Screen surface Create a split on the Stamp Screen surface using the intersection curve. a. Click the Split icon. b. Select the Stamp Screen surface. c. Select the intersection curve. d. Click OK to split a hole on the surface. 11a 11b 11c 12. Prepare the final data. Hide the Intersection curve. Rename the Split surface as Screen Finished. Close the part without saving it. 11d 8-83

84 Exercise Recap: Surfaces Operations Create a Revolve surface Create a surface Boundary Create a Fill surface Create a Join between surfaces Create a surface Trim Create a Fillet between surfaces Create a pre-defined Cylinder surface Create an Intersection curve Create Split surface 8-84

85 Exercise: Surface Delimitation Recap Exercise 40 min In this exercise, you will open an existing model and use the tools learned in this lesson to create a shape of a door using a surface. To save time, simple wireframe and surface elements have already been created for you. Detailed instructions for this exercise are provided for all new topics. By the end of this exercise you will be able to: Assemble the surface Define the upper/lower shape of the door Finalize the door 8-85

86 Do it Yourself (1/17) 1. Load Ex8E.CATPart. Load Ex8E.CATPart. This part already has some curves and surfaces created for you. Study and organize the specification tree. a. Observe that all the wireframe and surface elements have been created in a separate geometrical set. b. Create a new geometrical set called UPPER_DOOR_SHAPE c. Inside this Geometrical Set, create two geometrical sets called Surface and Wires. 2. Assemble the surfaces Define in work object the Surface Geometrical Set. Join the five surface in the geometrical set UPPER_INPUT_SURFACE. a. Click the Join icon. b. Select the surfaces to be joined (Corner, Front blend, Rear blend, Upper and side). c. Click OK to create a join. d. Rename the Join surface as Surf

87 Do it Yourself (2/17) 3. Create an offset curves Define in work object the Wires Geometrical Set. Hide the LOWER_INPUT_SURFACES for better visualization Create a parallel curves and Corner. a. Click the Parallel icon. b. Select the CURVE_UPPER_TRIM. c. Select surf1 as the Support. d. Specify the offset value equal to 50mm. e. Select the Reverse Direction if required. f. Click OK to create Parallel curve. g. Rename Parallel curve as CURVE UPPER OFFSET. 3a 3e 3c 3d 3f 8-87

88 Do it Yourself (3/17) 3. Create an Side offset curve (continued) Create a parallel curve. h. Click the Parallel icon. i. Select the CURVE SIDE TRIM. j. Select Surf1 as the Support. k. Specify the offset value equal to 50mm. l. Select the Reverse Direction if required. m. Click OK to create a Parallel curve. n. Rename the Parallel curve as CURVE SIDE OFFSET. 3h 3j 3k 3l 3m 8-88

89 Do it Yourself (4/17) 4. Create a Corner on support Create a Corner curve. a. Click the Corner icon. b. Select the first offset curve 4a c. Select the second offset curve d. Select the Surf1 as Support e. Specify the Radius value equal to 50mm. f. Select Next Solution to choose the required solution. g. Click OK to create Corner curve. h. Rename Corner curve as SIDE CORNER. 4g 4d 4e 4c 4b 8-89

90 Do it Yourself (5/17) 5. Create curves Create an intersection between Plane.1 and SIDE CORNER. Create a spline on support to connect SIDE_CORNER and CURVE_FRONT. Create a Join. a. Click the Intersection icon. b. Select the SIDE CORNER curve. c. Select Plane.1. d. Click OK to create an intersection. e. Rename the point as INTERSECTION 1. 5a 5b 5c 5d 8-90

91 Do it Yourself (6/17) 5. Create Curves (continued) f. Show CURVE FRONT. g. Click the Spline icon. h. Select the end point of CURVE_FRONT as the first input point i. Select INTERSECTION 1 j. Ensure that the arrow is pointing in the correct direction. If it is not, then click on the arrow to change its direction. k. Select Surf1 as support surface l. Click OK to create the spline. 5h 5i 5g 5k 5l 8-91

92 Do it Yourself (7/17) 5. Create Curves (continued) 5m m. Click the Trim icon. n. Select the Spline curve. o. Select the SIDE CORNER. p. Select Other side option if required. q. Click OK. 5p 5n 5o 5q 8-92

93 Do it Yourself (8/17) 5. Create Curves (continued) 5r r. Click the Join icon. s. Select the trimmed curve. t. Select the CURVE FRONT surface. u. Click OK to join the surfaces. v. Rename the Join as INTERNAL CURVE. 5s 5u 5t 8-93

94 Do it Yourself (9/17) 6. Create Corner on support Create a Corner curve between CURVE UPPER TRIM and CURVE SIDE TRIM. a. Click the Corner icon. b. Select the CURVE UPPER TRIM. c. Select the CURVE SIDE TRIM. d. Select the Surf1 as support surface. e. Specify the Radius value equal to 50mm. f. Click OK to create Corner curve. 6a 6d 6c 6e 6b 6f 8-94

95 Do it Yourself (10/17) 6. Create Corner on support (continued) g. Click the Boundary icon. h. Select the edge of the surface as shown. i. Click OK to create a boundary. j. Click the Corner icon. k. Select the previously created corner and boundary. l. Select the Surf1 as support surface. m. Specify the Radius value equal to 50mm. n. Click OK to create Corner curve. o. Rename the corner curve as EXTERNAL CURVE. p. Define in work object the Surfaces Geometrical Set. 6g 6i 6j 6h 6k 6n 6l 6m 8-95

96 Do it Yourself (11/17) 7. Create a surface split Split the surface surf1 using curves EXTERNAL CURVE and INTERNAL CURVE. a. Click the Split icon. b. Select the Surf1 surface. c. Select the EXTERNAL CURVE. d. Select the INTERNAL CURVE. e. Specify the side to be kept by selecting Other side option, if required. f. Click OK to split the surface. g. Rename the split as UPPER SHAPE. 7a 7b 7e 7c 7d 7f 8-96

97 Do it Yourself (12/17) Create the Lower Door Shape: 8. Create the Geometrical Set Create three geometrical sets as shown. a. Create a new geometrical set called LOWER_DOOR_SHAPE b. Inside this geometrical set, create two other geometrical sets called Surface and Wires. c. Show the surface Lower. 9. Create wireframe elements 8a Create the four boundary elements at the shown edges of Surf1 surface in Wires Geometric Set. a. Double-click the Boundary icon. b. Select the edge of the surface Lower. c. Click OK to create a first boundary. 8b 9a 8c CB4 d. The boundary dialog box reappears, repeat the steps and create the other three boundaries as shown. e. Rename the boundaries as CB1, CB2, CB3 and CB4. 9c CB3 CB2 CB1 8-97

98 Do it Yourself (13/17) 9. Create wireframe elements (continued) f. Double-click on the Point icon. g. Select the Curve as EXTERNAL CURVE h. Select the Point type as On curve option. i. Specify the Ratio value as 0 9f 9h 9g j. Click OK to create a point. k. Repeat the steps to create a point on the other end. 9i 9j 8-98

99 Do it Yourself (14/17) 9. Create wireframe elements (continued) 9l l. Double-click on the Parallel icon. m. Select the Curve as CB1. n. Select Lower as the Support. o. Select Point.1 as the Point. p. Click OK to create a Parallel curve. q. Repeat the steps to create a second parallel curve from CB3 passing through the second point created in the previous step. r. Rename both the Parallel curves as CB1_OFFSET and CB3_OFFSET respectively. 9m 9o 9n 9p 8-99

100 Do it Yourself (15/17) 9. Create wireframe elements (continued) s. Create a parallel curve at a distance of 50mm from CB2 curve on the Lower surface. t. Rename the Parallel curve as CB2_OFFSET. 10. Create a Corner on support Create a Corner curve between CB1_OFFSET, CB2_OFFSET and CB3_OFFSET curves. a. Double-click on the Corner icon. b. Select the Element 1 as CB1_OFFSET. c. Select the Element 2 as CB2_OFFSET d. Select the Lower surface as Support e. Specify the Radius value equal to 50mm. f. Click OK to create Corner curve. g. Repeat the steps to create a corner curve of 50mm radius between the resultant curve andcb3_offset. h. Rename the resultant curve as DOOR_LOWER_SHAPE_BOUNDARY 10h 10f 10b 10c 10d 10e 8-100

101 Do it Yourself (16/17) 11. Create a surface split Define in work object the Surfaces Geometrical Set which is inside LOWER_DOOR_SHAPE. Split the surface LOWER using the curve DOOR_LOWER_SHAPE_BOUNDARY. a. Click the Split icon. b. Select LOWER as the Element to cut. c. Select DOOR_LOWER_SHAPE_BOUNDARY as Cutting elements. d. Specify the side to be kept by selecting Other side option, if required. e. Click OK to split the surface. f. Rename the split as LOWER SHAPE. 11a 11b 11d 11c 11e 8-101

102 Do it Yourself (17/17) 12. Create the final door surface Create a new Geometrical Set called Door Assemble the UPPER_SHAPE and LOWER_SHAPE of the door. a. Click the Join icon. b. Select UPPER_SHAPE surface as Elements to Join c. Select LOWER_SHAPE surface as Elements to Join d. Click OK to join the surfaces to form a single door surface. e. Rename the result as DOOR. 12a 12b 12c 12d 8-102

103 Exercise Recap: Surface Delimitation Assemble the surface Define the upper/lower shape of the door Finalize the door 8-103

104 Exercise: Boss and Flange Creation Recap Exercise 30 min In this exercise, you will create a flange surface of the wheel arch and add the boss. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create the flange surface Create the boss surface Relimit the surfaces using the main surface 8-104

105 Do it Yourself (1/6) 1. Load Ex8F.CATPart. Load Ex8F.CATPart. This part already has some curves and surfaces created for you. 2. Create construction elements for a flange surface Define in work object the Reference Elements Geometrical Set. Join all the surfaces available in the WING_SURFACE Geometrical Set. Specify the Merging distance as 0.04mm Join the surface 8,9 and 10 available in the WHEEL_ARCH_STUDY_AREA Geometrical Set. Specify Merging distance as 0.04mm Join 1 Join

106 Do it Yourself (2/6) 3. Create a flange surface Create a Geometrical Set called Flange_Surface under the father node of the WHEEL_ARCH. Create the intersection of the two join surfaces created in the previous step. Rename the intersection as C1 Create a parallel curve from C1 at a distance of 15mm using the first join surface as the support element. Rename the parallel curve as C2 Split C2 between two planes Plane X=-310 and Plane 2. Rename the Split as C3 Create a vertical line of length 20mm from one extremity of C3. C1 C2 Vertical Line 8-106

107 Do it Yourself (3/6) 3. Create a flange surface (continued) Create a line normal to surface Join.2 from the other extremity of C3 (of default length, later used for reference only) Create an angle line from the same point with reference to the previous line at 30deg angle on the XZ plane Project the vertical line and the angle line on the Join.1 surface Rename these projection curves L1 and L2 respectively Create a Corner curve of radius 4mm between L1 and C2 Create a Corner curve of 4mm radius between the resulting curve and L2 L2 CORNER L1 Rename the resulting curve as CORNER. Project the curve CONTOUR on Join.1 Project 8-107

108 Do it Yourself (4/6) 3. Create a flange surface (continued) Create a Corner of radius 4mm between this projection and the offset curve C2. Do not trim the C2 curve while creating this corner. Repeat the corner operation twice to get the corner on both the sides of the projected curve. Hide the C2 curve. Trim the previous corner with CORNER curve. Split Join.1 using the last trim and C3. Last trim Projected Curve Projected curve is cornered at both end C3 Cornered curve trimmed with CORNER curve

109 Do it Yourself (5/6) 4. Relimit the surfaces Trim Join.2 and the last created split Split the resultant surface between PLANE2 and Surface.7 Trim the previous corner with CORNER curve. Split Join.1 using the last trim and C3. 5. Create a Blend cut Intersect PLANE X=-314 and PLANE.3. With intersection as an axis, create a cylinder (default length) and a radius of 4mm. Split the main surface with this cylinder Join this split with the remaining surfaces of WHEEL_ARCH_STUDY_AREA. Specify the Merging distance as 0.04mm Relimited surface after split operation Intersect Joint surface Cylinder split with main surface Cylinder 8-109

110 Do it Yourself (6/6) 6. Create a revolved shape of the boss Create a Geometrical Set called Bosses under the father node of the WHEEL_ARCH. Create revolution surfaces using L3 stamp axis as axis and the 2 lines L1 40 top and L2 40 down around a full circle. Create a 5 mm shape fillet using the two revolution surfaces and the blue surface called Boss surface. Revolved surface filleted with BOSS SURFACE Create a trim between the upper fillet surface and the main join. Create a fillet of 10mm on the upper edge of the surface. Similarly, create a trim between lower filleted surface and the main surface. Create a fillet of 4mm on the edge that is formed (shown). Apply 4mm fillet on this edge Upper revolve surface trimmed with main surface Fillet the upper edge of the trimmed cutout 8-110

111 Exercise Recap: Boss and Flange Creation Create the flange surface Create the boss surface Relimit the surfaces using the main surface 8-111

112 Case Study: Create Complex Surfaces Recap Exercise 30 min In this exercise, you will create a case study model. Let us recall the design intent of this model: The main junction surface (A) must pass through four section curves. The length of the base junction surface (B) must be 700mm. Sharp edges must not be present between the main junction surface and base junction surface. The front pillar surface (C) and the back pillar surface (D) must pass through the respective guide curves. The result must be a single surface Using the techniques you have learned so far, create the model without detailed instructions. C D A B 8-112

113 Do It Yourself: Create the Simplified B Pillar Load Start_CaseStudy8.CATPart and modify the model using the information below

114 Case Study Recap: Simplified B Pillar Create a Multi-Section surface. Fill the surface and create a join. Create an extruded surface. Apply fillets to sharp edges. Create a sweep. Join the surfaces to get a single result