In this chapter, you will learn the following:

In this chapter, you will learn the following:
Chapter 8: Advanced Modeling - II In this chapter, you will learn the following: Creating a Sweep Feature Creating a Sweep Cut Feature Creating a Lofted feature Creating a Lofted Cut Feature Creating a Boundary Feature Creating a Boundary Cut Feature Creating Curves Splitting Faces of a Model Creating 3D Sketches

Creating a Sweep Feature
Chapter 8: Advanced Modeling II Creating a Sweep Feature A sweep feature is created by adding material by sweeping a profile along a path.

Chapter 8: Advanced Modeling II
After creating the path and the profile, click on the Swept Boss/Base tool in the Features CommandManager. The Sweep PropertyManager appears.

Profile and Path The options in the Profile and Path rollout of the PropertyManager are used for selecting a profile and a path. The options are discussed next. Sketch Profile The Sketch Profile radio button of the Profile and Path rollout is selected, by default. As a result, the Profile and the Path fields are available in the PropertyManager.

Circular Profile The Circular Profile radio button of the Profile and Path rollout is used for creating a sweep feature that has a circular cross section such as solid rod or hollow tube by specifying the diameter value.

Options Chapter 8: Advanced Modeling II
By default, the Options rollout of the PropertyManager is collapsed. To expand this rollout, click on the arrow available on its right. Note that some of the options of the Options rollout are not available while creating a base/first feature. Also, the availability of options in this rollout depends upon the selection of Sketch Profile or Circular Profile radio button in the Profile and Path rollout of the PropertyManager. The options of the Options rollout are discussed next.

Profile orientation drop-down list The options in the Profile orientation drop-down list are used for controlling the orientation of the profile along the path. Follow Path By default, the Follow Path option is selected in the drop-down list. As a result, the profile follows the path by maintaining the same angle of orientation from start to end by aligning itself normal to the path.

Keep Normal Constant On selecting the Keep Normal Constant option, the profile follows a path such that it remains parallel throughout the path.

Profile Twist drop-down list The options in the Profile Twist drop-down list are used for controlling the twisting or alignment of the profile along the path. None By default, the None option is selected in the Profile Twist drop-down list. As a result, the profile follows a path such that it maintains normal alignment.

Specify Twist Value By selecting the Specify Twist Value option, you can twist the profile along the path.

NOTE: If the profile is created between the endpoints of the path and you are creating a bi-directional sweep feature, then on selecting the Specify Twist Value option in the Profile Twist drop-down list, the Direction 2 field also becomes available in the rollout along with the Twist control drop-down list and the Direction 1 field. The Direction 2 field is used for specifying the twist angle in the second direction of the sweep feature.

Specify Direction Vector On selecting the Specify Direction Vector option in the Profile Twist drop-down list, the Direction Vector field becomes available. The Direction Vector field is used for selecting a direction vector for aligning the profile.

Minimum Twist On selecting the Minimum Twist option in the Profile Twist drop-down list, the minimum twist is allowed to the profile while following the path in order to avoid self-intersection.

Tangent to Adjacent Faces On selecting the Tangent to Adjacent Faces option, the profile maintains tangency with the adjacent face of the path.

Natural On selecting the Natural option in the Profile Twist drop-down list, the profile follows a path such that it maintains natural twist.

Follow Path and First Guide Curve On selecting the Follow Path and First Guide Curve option, the profile follows the path as well as the 1st guide curve.

Follow First and Second Guide Curve On selecting the Follow First and Second Guide Curve option, the profile follows the path, and the first and second guide curves.

Merge tangent faces On selecting the Merge tangent faces check box in the Options rollout, the tangent faces of the resultant sweep feature get merged and appear as a single face.

Merge result By default, the Merge result check box is selected in the Options rollout. As a result, the resultant sweep feature merges with the existing features of the model and forms a single body.

Align with end faces On selecting the Align with end faces check box, the end section of the sweep feature gets aligned with the face of an existing feature, which is encountered by the path.

Guide Curves The Guide Curves rollout of the Sweep PropertyManager is used for selecting guide curves for creating the sweep feature. Guide Curves field The Guide Curves field is used for selecting guide curves in the graphics area. Move Up and Move Down The Move Up and Move Down buttons are used for changing the order or sequence of guide curves in the Guide Curves field.

Merge smooth faces By default, the Merge smooth faces check box is selected. As a result, the smooth or tangent segments of the sweep feature get merged together.

Show Sections The Show Sections button of the rollout is used for viewing the intermediate sections of the sweep feature being created by using guide curves.

Start and End Tangency The options in the Start and End Tangency rollout of the PropertyManager are used for specifying the start and end tangency of the sweep feature. Start tangency type The options in the Start tangency type drop-down list are used for specifying the start tangency for a sweep feature.

End tangency type The options in the End tangency type drop-down list are used for specifying the end tangency type for a sweep feature. Thin Feature The Thin Feature rollout of the PropertyManager is used for creating a thin sweep feature.

Creating a Sweep Cut Feature
Chapter 8: Advanced Modeling II Creating a Sweep Cut Feature The method of creating a sweep cut feature is the same as creating a sweep feature with the only difference that a sweep cut feature is created by removing material from the model.

To create a sweep cut feature, click on the Swept Cut tool in the Features CommandManager. The Cut-Sweep PropertyManager appears.

On selecting the Solid Profile radio button, the Tool body and Path fields get enabled in the PropertyManager. The Tool body field is activated, by default and is used for selecting a tool body that follows the path in order to create a sweep cut feature.

Creating a Lofted feature
Chapter 8: Advanced Modeling II Creating a Lofted feature A lofted feature is created by lofting two or more than two profiles (sections) such that the cross-sectional shape of the lofted feature transits from one profile to another.

To create a lofted feature, click on the Lofted Boss/Base tool in the Features CommandManager. The Loft PropertyManager appears.

Profiles The Profiles rollout of the PropertyManager is used for selecting profiles of the lofted feature. You can select two or more than two similar or dissimilar closed profiles for creating a lofted feature. After selecting the profiles, the preview of the lofted feature appears in the graphics area with connectors, that connect the profiles. NOTE: You can drag the connectors that appear in the preview of a lofted feature to create a twist in the feature. By default, in the preview of a loftrd feature, only one handle appears with its connectors.

Start/End Constraints The options in the Start/End Constraint rollout are used for defining normal, tangent, or curvature continuity as the start and end constraints of a lofted feature. Start constraint The options in the Start constraint drop-down list are used for defining the start constraint for a lofted feature.

None By default, the None option is selected in the Start constraint drop-down list. As a result, no constraint is applied and the cross-sectional shape transits from one profile to another, linearly.

Direction Vector On selecting the Direction Vector option, the Direction Vector, Draft angle, and Start Tangent Length fields become available in the rollout.

The Direction Vector field is used for selecting a direction vector that defines the start constraint for a lofted feature. You can select a plane, a linear edge, a linear sketch entity, or an axis as direction vector. Figure shows the preview of the lofted feature after selecting the Top plane as the direction vector.

The Draft angle field is used for defining the draft angle for start constraint. By default, the draft angle is set to 0 degree.

The Start Tangent Length field is used for defining the start tangent length for start constraint. By default, the start tangent length is specified as 1. Figure shows the preview of the lofted feature with the draft angle set to 0-degree and the start tangent length is set to 2.

Normal To Profile On selecting the Normal To Profile option in the Start constraint drop-down list, the tangency constraint is applied normal to the start section of the lofted feature. Tangency To Face On selecting the Tangency To Face option in the Start constraint drop-down list, the start section of the lofted feature maintains tangency with the adjacent face of existing geometry

Curvature To Face On selecting the Curvature To Face option, the start profile of a lofted feature maintains curvature continuity with the adjacent faces of existing geometry. NOTE: If the loft feature being created is the base/first feature, then the Curvature To Face option will not be available in the drop-down list.

Reverse Direction and Reverse Tangent Direction The Reverse Direction and Reverse Tangent Direction buttons of the Start/End Constraint rollout are used for reversing the direction of the applied constraints.

Apply to all The Apply to all check box is selected in the rollout, by default. As a result, only one handle appears in the preview of a lofted feature.

End constraint The End constraint drop-down list is used for defining the end constraint of a lofted feature.

Guide Curves Guide curves are used for guiding the cross-sectional shape of a lofted feature. You can create multiple guide curves for controlling the cross-sectional shape of a lofted feature.

To select guide curves, click on the Guide Curves field in the Guide Curves rollout and then select the guide curves.

To Next Guide The To Next Guide option in the Guide curves influence type drop-down list is used for extending the influence of the guide curve to the next guide curve only

To Next Sharp The To Next Sharp option is used for extending the influence of the guide curve to the next sharp. To Next Edge The To Next Edge option is used for extending the influence of the guide curve to the next edge.

Global The Global option is used for extending the influence of the guide curve to the entire lofted feature.

Centerline Parameters The Centerline Parameters rollout of the PropertyManager is used for selecting a centerline for creating a lofted feature. Centerline is used for maintaining the neutral axis of the lofted feature.

Sketch Tools The Sketch Tools rollout is used for editing the 3D sketch sections/profiles of a lofted feature. Options

Merge tangent faces On selecting the Merge tangent faces check box, the tangent faces of the feature merge with each other.

Close Loft The Close loft check box is used for creating a lofted feature such that the start and end profiles of the lofted feature join automatically with each other and create a closed lofted feature.

Show preview The Show preview check box is used to show the preview of the lofted feature in the graphics area. Thin Feature The Thin Feature rollout is used for creating a thin lofted feature.

Creating a Lofted Cut Feature
Chapter 8: Advanced Modeling II Creating a Lofted Cut Feature The method of creating a lofted cut feature is the same as of creating a lofted feature with the only difference that the a lofted cut feature is created by removing material from the model.

Creating a Boundary Feature
Chapter 8: Advanced Modeling II Creating a Boundary Feature Boundary features are high quality, complex shaped, and accurate features. Boundary features are used for maintaining high curvature continuity as well as for creating complex shape features. You can create boundary features by using the Boundary Boss/Base tool.

Figure given below shows one section as direction 1 guide and three curves as direction 2 guides. Figure shows the resultant boundary feature.

To create a boundary feature, create all sections and curves as direction 1 and direction 2 guides of the boundary feature, respectively, and then click on the Boundary Boss/Base tool in the Features CommandManager. The Boundary PropertyManager appears.

Direction 1 The Curves field in the Direction 1 rollout is used for selecting the sections as direction 1 guides. By default, this field is activated. As a result, you are prompted to select sections. Select the sections as direction 1 guides in the graphics area one by one.

Direction 2 The Curves field in the Direction 2 rollout is used for selecting the curves as direction 2 guides. Click on this field and then select curves in the graphics area.

Options and Preview The options in the Options and Preview rollout are the same as those discussed earlier, while creating the lofted feature except the Trim by direction 1 check box, which is discussed next. Trim by direction 1 The Trim by direction 1 check box is used for trimming the extended portion of the feature, which is beyond the direction 1 guides.

Thin Feature The Thin Feature rollout is used for creating a thin boundary feature.

Curvature Display The options in the Curvature Display rollout are used for controlling the display style of the preview that appears in the graphics area . Mesh preview The Mesh preview check box is used for displaying the mesh preview in the graphics area .

Zebra stripes The Zebra stripes check box is used for turning on the appearance of zebra stripes in the preview of the boundary feature

Curvature combs The Curvature combs check box is used for turning on the appearance of curvature combs in the preview of the boundary feature.

Creating a Boundary Cut Feature
Chapter 8: Advanced Modeling II Creating a Boundary Cut Feature The method for creating a boundary cut feature is the same as creating a boundary feature with the only difference that the boundary cut feature is created by removing material from the model.

Creating Curves Chapter 8: Advanced Modeling II
In SOLIDWORKS, you can create different types of curves. Curves are mainly used as the path, guide curves, and so on for creating features such as sweep, lofted, and boundary. The tools for creating different types of curves are grouped together in the Curve flyout.

Creating Projected Curves In SOLIDWORKS, you can create projected curves by using the Project Curve tool. The Project Curve tool is used for creating projected curves by using two methods: Sketch on Faces and Sketch on Sketch

To create a projected curve, invoke the Curve flyout by clicking on the arrow at the bottom of the Curves tool in the Features CommandManager. Next, click on the Project Curve tool in the flyout. The Projected Curve PropertyManager appears. The options in this PropertyManager are discussed next.

Sketch on faces The Sketch on faces radio button is used for creating projected curves by projecting a sketch on to an existing face of a model. On selecting this radio button, the Sketch to Project and the Projection Faces fields are enabled in the rollout.

Sketch on sketch The Sketch on sketch radio button is used for projecting one sketch onto another sketch such that the resultant projected curve represents the intersection of sketches.

Creating Helical and Spiral Curves You can create helical and spiral curves by using the Helix and Spiral tool of the Curves flyout. You can use helical and spiral curves as paths, guide curves, and so on for creating features like sweep and lofted.

To create a helical or a spiral curve, create a circle and then invoke the Curves flyout. Next, click on the Helix and Spiral tool. The Helix/Spiral PropertyManager appears.

The options in the Helix/Spiral PropertyManager are used for creating constant pitch helical curves, variable pitch helical curves, and spiral curves. The options are discussed next. Defined By The Defined By rollout is used for defining the type of curve (helical or spiral) to be created and the method to be adopted for creating it. Pitch and Revolution Height and Revolution Height and Pitch

Spiral The Spiral option is used for creating a spiral curve by defining its pitch and number of revolutions. On selecting this option, the options for creating a spiral curve by defining its pitch and revolutions are enabled in the Parameters rollout.

Parameters The Parameters rollout of the PropertyManager is used for specifying the parameters for creating a curve. Constant pitch Pitch, Revolutions, Height, and Start angle Reverse direction Clockwise and Counterclockwise

Variable pitch The Variable pitch radio button is used for creating a helical curve with variable pitch and variable diameter .

Taper Helix The Taper Helix rollout of the PropertyManager is used for creating a tapered helical curve.

Creating Curves by Specifying XYZ Points You can create a curve by specifying coordinates (X, Y, Z), which define the shape of the curve. For doing so, invoke the Curves flyout and then click on the Curve Through XYZ Points tool. The Curve File dialog box appears.

In the Curve File dialog box, you can specify the coordinates (X, Y, Z) of multiple points with respect to the origin (0, 0, 0) for creating a curve. Besides specifying coordinates of points, you can import .sldcrv or .txt (notepad) files containing the coordinates of a curve.

Creating Curves by Selecting Reference Points
Chapter 8: Advanced Modeling II Creating Curves by Selecting Reference Points In SOLIDWORKS, you can create 3D curves by selecting reference points in the graphics area. The reference points can be located in the same or different planes. You can also select vertices of the model or sketch points as reference points for creating a curve. To create a curve by selecting reference points, invoke the Curves flyout and then click on the Curve Through Reference Points tool. The Curve Through Reference Points PropertyManager appears.

Creating a Composite Curve
Chapter 8: Advanced Modeling II Creating a Composite Curve A composite curve is created by joining two or more than two curves together. You can join multiple curves or sketches together and create a single composite curve by using the Composite curve tool of the Curves flyout.

Splitting Faces of a Model
Chapter 8: Advanced Modeling II Splitting Faces of a Model You can split faces of a model by creating split lines. In SOLIDWORKS, you can create split lines by using the Split Line tool. For doing so, click on the Split Line tool in the Curves flyout. The Split Line PropertyManager appears. The options in this PropertyManager are discussed next.

Type of Split The options in the Type of Split rollout are used for selecting the type of split method to be used for splitting the faces of a model. The options are discussed next. Projection

On selecting the Projection radio button, the Sketch to Project and Faces to Split fields are enabled in the Selections rollout of the PropertyManager.

Intersection

Silhouette

Creating 3D Sketches Chapter 8: Advanced Modeling II
In SOLIDWORKS, in addition to creating 2D sketches and 3D curves, you can also create 3D sketches in the 3D Sketching environment. Most of the time, 3D sketches are used as 3D path and the guide curve for creating features like sweep, lofted, and boundary. To create 3D sketches, you need to invoke the 3D Sketching environment of SOLIDWORKS.

For doing so, click on the arrow at the bottom of the Sketch tool in the Sketch CommandManager. The Sketch flyout appears. In this flyout, click on the 3D Sketch tool. The 3D Sketching environment is invoked.

Using the Line Tool in the 3D Sketching Environment

Using the Spline Tool in the 3D Sketching Environment

Tutorial 1 Chapter 8: Advanced Modeling II
Create the model given Below. The different views and dimensions are given in the same figure. All dimensions are in mm. To create this tutorial, follow the steps given in the textbook.

Create the model shown in the figure given below. The different views and dimensions are given in the same figure. All dimensions are in mm. To create this tutorial, follow the steps given in the textbook.

Create the model shown in the figure given below. All dimensions are in mm. To create this tutorial, follow the steps given in the textbook.

Hands-on Test Drive 1 Chapter 8: Advanced Modeling II
Create the model, as shown in figure given below. After creating the model, apply the Cast Alloy Steel material and then calculate its mass properties. All dimensions are in mm.

Hands-on Test Drive 2 Chapter 8: Advanced Modeling II
Create the model, as shown in figure given below and then apply the Alloy Steel material. Also, calculate the mass properties of the model. All dimensions are in mm.

Summary Chapter 8: Advanced Modeling II
In this chapter, you have learned how to create sweep features, sweep cut features, lofted features, lofted cut features, boundary features, boundary cut features, curves, split face, and 3D Sketches. A sweep feature is created by sweeping a profile along a path. The profile of the sweep feature can be a closed sketch, whereas a path can be an open or a closed sketch. You can also use guide curves to guide the profile (section) of the sweep feature. Additionally, you can twist the profile along the path. You can also create thin sweep feature. You have also learned that while creating the sweep cut feature, you can use a closed sketch and a solid body as the profile to sweep along the path.

A lofted feature is created by lofting two or more than two profiles (sections) such that its cross-sectional shape transits from one profile to another. You can also use guide curves to control the cross-sectional shape of the lofted feature. You can also create closed lofted feature. Similar to creating lofted features, you can also create boundary features, which are high quality and complex shaped features. You have also learned about creating projected curves, helical and spiral curves, curves by specifying XYZ points, curves by selecting reference points, and composite curves. In addition, you have learned how to split the faces of a model and create 3D sketches.

Questions Chapter 8: Advanced Modeling II
The ________ tool is used for creating sweep features. While creating a sweep feature, the ________ option is selected by default. As a result, the profile follows the path. Selecting the ________ option creates a sweep feature such that the profile twists along a path. By selecting the ________ option, you can select a tool body following the path to create a sweep cut feature. You can create projected curves by using two methods: ________ and ________. The ________ radio button is used for creating helical curve with a variable pitch.

By selecting the ________ option, you can create a helical curve by defining its pitch and number of revolutions. The ________ tool is used for creating curve by specifying coordinate points. The profiles/sections of a lofted feature must be closed. (True/False) In SOLIDWORKS, you cannot create tapered helical curves. (True/False) For creating sweep feature, the start point of the path must lie on the plane of the profile created. (True/False)

In this chapter, you will learn the following:

Similar presentations

Presentation on theme: "In this chapter, you will learn the following:"— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

In this chapter, you will learn the following:

Similar presentations

Presentation on theme: "In this chapter, you will learn the following:"— Presentation transcript:

Similar presentations

About project

Feedback