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)
Breaking it down into features
Creating Construction Centerlines
Construction Centerlines to Create Holes
Constraining Circular Patterned Holes
Edge Features(3D Fillets & Chamfers) and Model Tree
SW05 In-Class Activity
SW05 Out-of-Class Homework Assignment
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
1st Step: Base Feature
Adding / Subtracting Material
Edge Features
Model Tree
Final parts are created using a series of steps
The first step to creating a part is to create the “Base” feature
This base feature takes into account the overall shape of the object and tries to account for as many features as possible in one extrusion
Once a base feature is created the shape can be modified by adding or subtracting material to create form features
Special features that would be too complex to add by extrusion or revolving are built-in to 3D parametric programs

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.
Determines design strategy
Feature Modeling Example

6. Series of Steps Base Feature Features First Extrusion or Revolve
Reduce Steps of Construction
Features
Additions or subtractions from original base feature
When trying to construct a 3D model by viewing the final product first determine the base feature
This feature probably cannot take care of every feature of the final part but will be the main starting point for construction
Base features normally involve an extrusion or revolve and the goal is to take care of as many features as possible in one step

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 construction line of infinite length at a 45O angle through the origin
Repeat procedure at a -45O angle through the origin
Exit sketch and perform an Extruded Cut through all
Draw 4 center point circles on construction lines and make them equal
Establish Symmetry for each pair of circles
Dimension

13. A Short Cut Method to Produce Multiple Holes
In the sketch mode insert a construction line of infinite length at a 45O angle through the origin
Sketch a single circle on the construction line, locate and dimension the circle
Note that the number 4 could have been set to any number … 2, 3, 8,etc
Select Linear Sketch Pattern/ Circular Sketch Pattern
Select the drawn circle
Set the number of circles to 4, accept and Extrude Cut as before

14. Breaking it Down Wrap Up
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
Homework Assignment SW05-OUT:
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?
Revolve a shape that has the profile and the grooves already. This would only take one step but it is debatable if this would be easier. Depends on the designer and the design intent of the object.

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

25. The top slanted edge will be added using a chamfer
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
Features to add last:
3D Fillets: Rounded edges
3D Chamfers: Slanted edges
Editing Features with Model Tree
Homework Assignment SW05-OUT:
Problem 6.4 (nn) R3

32. In-Class Activity 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 Out-of-Class HW
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
Reference Geometry – Planes & Axes
Mirroring
Patterning – Linear & Circular
Hole Wizard
Shells
Sweeps
Lofts
Advance Modeling Wrap Up
Methods to Save Time
Methods to Create Shapes
In the SLIDE SHOW MODE this page supports HYPERLINK navigation

36. Optional Advanced Modeling Techniques
ENGR 1182
SolidWorks 05

37. 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
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38. Reference Geometry: Axes
Axes can also be created without the creation of a 2D sketch
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39. First the Mirror Plane must be chosen
Mirroring creates an reverse copy of features on the opposite side of a mirroring plane
First the Mirror Plane must be chosen

40. The new features are joined to the original model
Mirror
Once the plane has been chosen then the features to mirror are selected
The new features are joined to the original model
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41. 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.
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42. Features can also be duplicated in circular patterns around an axis
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
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43. Holes Mating Parts Hole Specifications Built-in Hole Tools
Location and Size Selected
Mating parts are usually attached using bolts or screws
This requires special holes that will have the right dimensions and shape depending upon the fastener
3D Parametric design programs have built-in hole tools that quickly and accurately create these holes
The type of hole can be selected from drop down lists and the location of the hole can be specified

44. Holes using the Hole Wizard
1) Under Feature select Hole Wizard 2) Specify the type of Hole 3) Specify Hole Position 4) Add threads 1 2 3 4
Mating parts are usually attached using bolts or screws
This requires special holes that will have the right dimensions and shape depending upon the fastener
3D Parametric design programs have built-in hole tools that quickly and accurately create these holes
The type of hole can be selected from drop down lists and the location of the hole can be specified
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45. Shells Removes Volume Thin Wall Created
Shelling removes the interior volume of a solid model
One surface removed and thin wall of constant thickness left
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46. Mirror complex features to save time
Sweep
Mirror complex features to save time
Pathways can be combined with a 2D profile, such as a circle, to create what is known as a sweep
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47. The same shape but different sizes can be used
Loft
The same shape but different sizes can be used
Lofting is taking two profiles on separated planes and filling the space between with material that blends the original profiles

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