Feature-Based Modeling and Optional Advanced Modeling. ENGR 1182 SolidWorks 05

Transcription

1 Feature-Based Modeling and Optional Advanced Modeling ENGR 1182 SolidWorks 05

2 Today s Objectives Feature-Based Modeling (comprised of 2 sections as shown below) 1. Breaking it down into features Creating Construction Centerlines Construction Centerlines to Create Holes Constraining Circular Patterned Holes 2. Edge Features(3D Fillets & Chamfers) and Model Tree SW05 Activity SW05 Application Optional Advanced Modeling Methods to Save Time ( Planes, Axes, Mirroring & Patterning, Holes, Shells, Sweep, & Loft) with HYPERLINK navigation

3 Feature-Based Modeling Break down into Features Series of Steps 1 st Step: Base Feature Adding / Subtracting Material Edge Features Model Tree

4 Breaking it Down into Features ENGR 1182 SolidWorks 05

5 Breaking it Down into Features Objects can be thought of in terms of features Shapes Holes Rounds Etc. Feature Modeling Example Determines design strategy

6 Series of Steps Base Feature First Extrusion or Revolve Reduce Steps of Construction Features Additions or subtractions from original base feature

7 How many different ways could we make this?

8 Example Construction 1 We can think of the block in terms of 2 L shapes and then cut out the hole

9 Example Construction 2 We can think of the block in terms of a C shape and then add the plank with a hole

10 Example Construction 3 Finally, we could draw the overall shape from the top view and remove unwanted material

11 An Important Concept Most sketches can be greatly simplified by establishing horizontal and vertical "Centerlines" and then applying constraints employing those construction centerlines. When the object exhibits symmetry, those construction centerlines are often drawn though the origin. Many sketches will be much easier to constrain if one uses horizontal and vertical construction centerlines. Typically used constraints include dimensioning, symmetry and equal. So even if you don t initially recognize a need for vertical and horizontal construction centerlines, it is a very good practice to include them in your sketches!

12 Using Construction Center Lines to Position Multiple Holes In the sketch mode insert a horizontal construction line of infinite length and 2 angled infinite length construction lines through the origin using the As sketched option. DIMENSION the angle to be 45 O. Sketch a circle on each of the the angled construction lines setting all the circles EQUAL. Locate and Size all of the EQUAL circles which requires 5 dimensions. Exit sketch and perform an Extruded Cut using the Through All direction on the FULLY DEFINED sketch. Note that any additional circles require corresponding angled construction lines and located and sized circles.

13 A Short Cut Method to Produce Multiple Holes Any NUMBER In the sketch mode insert a horizontal construction line of infinite length and an angled line as shown. DIMENSION the angle to be 45 degrees. Select the drawn circle and set the pattern number to 4 Sketch a single circle on the angled construction line, locate and size the circle Offset the pattern center by x=y= 0.1 Select Linear Sketch Pattern/Circular Sketch Pattern As illustrated earlier, exit the now FULLY DEFINED SKETCH and perform an Extruded Cut using the Through All direction. Select Display/Delete Relations/Add Relations, click on the Offset pattern center and the part center, select Coincident and then OK.

14 Breaking it Down Wrap Up Breaking it down Base Feature Start with an extrusion (or revolve) that contains the basic shape of the object Minimize steps by choosing an appropriate shape for the base step (what shape can be used to build off of) Do not try to take into account every detail, add later with additional features Series of Logical Steps Application SW05: Problem 6.4 (ss) from the text.

15 In-Class Activity The object to the right can be created many different ways. Can you determine at least 2 different methods (starting on different planes) and create the same object?

16 Edge Features and Model Tree ENGR 1182 SolidWorks 05

17 Edge Features 3D Fillets create rounded edges 3D Chamfers create slanted edges

18 2D Fillets vs. 3D Fillets 2D Fillets are only to be used in Sketches 3D Fillets are used on edges of the part (3D Fillets are extremely powerful in making realistic designs)

19 SolidWorks Example: Piston Head How would you break this down into features? Where would you start? Where would you use the edge tools? At what point in the process?

20 SolidWorks: Base Feature There are a couple ways to effectively model this piston head but for these slides we will start with a simple extrusion of a circle to create a cylinder

21 SolidWorks: Extruded Cut The volume will be removed using an extruded cut offset from the bottom surface

22 SolidWorks: Revolved Cut The piston rings will be cut out using a revolved cut

23 SolidWorks: Review Design Is there any other way that we could have reached this point and how many steps would it have involved? Would it be easier?

24 SolidWorks: Extruded Cut The pin hole and groove will be removed using an extruded cut

25 SolidWorks: Chamfer The top slanted edge will be added using a chamfer

26 SolidWorks: Fillet And finally the bottom edge of the head will be smoothed out using a Fillet (under the features menu)

27 SolidWorks: Finished Part This finished product can now be used in an assembly with other components shown here

28 SolidWorks: Design Tree The design tree on the left of the screen catalogs all the steps of creating this part and records the steps from top to bottom Sketches are absorbed into features but can be accessed by clicking the plus sign next to each feature

29 SolidWorks: Part Editing The design tree can be rolled back by clicking and dragging the blue bar at the bottom up and the features are no longer shown New features can be added to this model in the middle of the design tree while other items are still rolled back

30 SolidWorks: Altered Final Part These changes will also carry over to the assembly that contains the part When the design tree is restored then all the features return as long as changes do not interfere with previous features

31 Feature Based Modeling Wrap Up Recognize Features of Object Start with Base Feature Carefully consider the use of construction centerlines in most sketches Add or Remove Material in a series of steps TOP VIEW Application SW05: Problem 6.4 (nn) Features to add last: 3D Fillets: Rounded edges 3D Chamfers: Slanted edges Editing Features with Model Tree R3

32 Activity (SW05) Problem 6.4 (u) Create the following shape according to the features and dimensions. First break this object down into features (you should be able to create this in 2 sketches) Then use 3D Fillets for the 4 rounded edges

33 Important Takeaways Feature-based modeling is used to break down the features of a part to create the part in an efficient way. Edge features, like chamfers and fillets, are used to create different edge designs efficiently. R3

34 What s Next? Due Next Class SW05 Application Before next class, you will read about assembly modeling. Assemblies are collections of 3D parts that are constrained to form one engineering system. Take SolidWorks 6 Quiz on readings

35 Optional Advanced Modeling Methods to Save Time Methods to Create Shapes Convert Entities Reference Geometry Planes & Axes Mirroring Patterning Linear & Circular Hole Wizard Shells Sweeps Lofts Advance Modeling Wrap Up In the SLIDE SHOW MODE this page supports HYPERLINK navigation

36 Optional Advanced Modeling Techniques ENGR 1182 SolidWorks 05

37 Convert Entities (adds all lines to the sketch plane and makes them available for future operations with is very useful when more than one feature appears within a sketch) Desired Object WITHOUT Convert Entities Starting Object (1) Draw Perimeter Circle, (2) Dimensioned Center Circle and (3) Carefully Create Closed Sections for Cut (must precisely connect circle midpoints with corners as shown above) (4) Must Trim Perimeter Circle (5) Select Areas to Extrude Cut and accept Cut WITH Convert Entities Starting Object (1) Draw Perimeter Circle, (2) Dimensioned Center Circle (3) Click on Convert Entities to automatically generate shown RED Lines No Trimming of Perimeter Circle required! (4) Select Areas to Extrude Cut and accept Cut

38 Reference Geometry: Planes SolidWorks starts off with the 3 original planes: front, right, top To add a new plane we can reference previous planes and create offset new planes or other options RETURN TO START

39 Reference Geometry: Axes Axes can also be created without the creation of a 2D sketch RETURN TO START

40 Mirror Mirroring creates an reverse copy of features on the opposite side of a mirroring plane First the Mirror Plane must be chosen

41 Mirror Once the plane has been chosen then the features to mirror are selected The new features are joined to the original model RETURN TO START

42 Linear Patterns Once edges are selected for direction, number of instances and distance are specified in the dialog box Features can also be duplicated in linear patterns in either one or two directions. RETURN TO START

43 Circular Patterns Once features and axes are chosen the angle and number of instances are specified Features can also be duplicated in circular patterns around an axis Also see slide 12 - Using Construction Center Lines to Position Multiple Holes RETURN TO START

44 Holes Mating Parts Hole Specifications Built-in Hole Tools Location and Size Selected

45 Holes using the Hole Wizard 1) Under Feature select Hole Wizard 2) Specify the type of Hole 3) Specify Hole Position 4) Add threads RETURN TO START

46 Shells Removes Volume Thin Wall Created RETURN TO START

47 Sweep Pathways can be combined with a 2D profile, such as a circle, to create what is known as a sweep Mirror complex features to save time RETURN TO START

48 Loft Lofting is taking two profiles on separated planes and filling the space between with material that blends the original profiles The same shape but different sizes can be used

49 Loft Different shapes can be blended into one solid such as the hexagon is connected to the circles of different sizes Circular patterns, fillets, and appearances can also be added RETURN TO START

50 Advanced Concepts Wrap Up Time Saving Methods Reference Geometry Planes/Axes/Points Mirroring Linear Patterns One or two directions Circular Patterns Advanced Shapes Sweep Loft OPTIONAL: SolidWorks tutorials Lofts Pattern Features Revolves and Sweeps Found under the Building Models tab of the SolidWorks tutorials RETURN TO START