In this chapter, you will learn the following:

In this chapter, you will learn the following:
Advanced Modeling - III In this chapter, you will learn the following: Working with Hole Wizard Creating Advanced Holes Adding Cosmetic Threads Creating Threads Creating Fillets Creating Chamfers Creating Rib Features Creating Shell Features Creating Wrap Features

Working with Hole Wizard
Advanced Modeling - III Working with Hole Wizard The Hole Wizard tool is used to create standard holes such as counterbore, countersink, and straight tap as per the standard specifications. To create standard holes by using the Hole Wizard tool, click on the Hole Wizard tool in the Features CommandManager. The Hole Specification PropertyManager appears.

Advanced Modeling - III
Type Tab The Hole Specification PropertyManager has two tabs: Type and Positions. By default, the Type tab is activated. As a result, the options to specify the type of hole and hole specifications are displayed in different rollouts of the PropertyManager. The options are as follows: Hole Type The Hole Type rollout of the PropertyManager is used to select the type of hole such as counterbore, countersink, or straight tap. Depending upon the type of hole to be created, you can click on the Counterbore, Countersink, Hole, Straight Tap, Tapered Tap, or Legacy button in this rollout.

Standard The Standard drop-down list is used to select the type of standard such as ANSI Metric, ANSI Inch, BSI, IS, JIS, and ISO for creating hole. Type The Type drop-down list is used to specify the type of fastener to be inserted into the hole.

Hole Specifications The Hole Specifications rollout of the PropertyManager is used to define specifications for the fastener to be inserted into the hole. Size The Size drop-down list is used to select the size of the fastener to be inserted. Fit The Fit drop-down list is used to select the type of fit between the fastener and hole. Show custom sizing The Show custom sizing check box is used to display and customize the standard size of the hole.

End Condition The options in the End Condition rollout are used to define the end condition or termination method for a hole. Options The availability of the options in the Options rollout depends upon the type of hole selected.

Head clearance The Head Clearance field is used to define the clearance between the top face of the fastener head and the hole. Near side countersink

Far side countersink Under head countersink

In case of Straight tap hole type, the options in the Options rollout appear as shown in Figure. These options are as follows:

Tap drill diameter, Cosmetic thread, and Remove thread

Thread class On selecting the Thread class check box, the Thread class drop-down list becomes available in front of it. By using this drop-down list, you can select a class for the threaded or tapped holes. After specifying all specifications in the Type tab, you need to define the placement point for the hole by using the Position tab. Positions Tab The Positions tab of the PropertyManager is used to define the position of the hole.

You can select a planar face, a plane, or a curved face as the placement face for the hole. You can use the dimension tools to position the placement points of the hole.

Creating Advanced Holes
In SOLIDWORKS 2017, you can create advanced holes such as manifolds and multi-stepped by using the Advanced Hole tool. You can also define customized hole types with the combinations of different standard holes such as counterbore, countersink, straight tap, and tapered by using this tool.

Near And Far Side Faces The Near And Far Side Faces rollout of the PropertyManager is used to select near and far side faces of a hole.

Once you have defined the first near side hole element by using the Near Side flyout, you need to define the hole element specifications such as type of hole, standard, and size by using the options of the Element Specification rollout of the PropertyManager.

To define the far side face of the hole, select the Far Side check box in the Near And Far Side Faces rollout of the PropertyManager. The Far Side Face field and the Far Side flyout appears.

Select a face of the model as the far side face of the hole
Select a face of the model as the far side face of the hole. The preview of the hole is modified in the graphics area such that the default far side hole element is added. You can select a required far side hole element by using the Far Side flyout. To select a far side hole element, invoke the Far Side flyout.

After selecting the required first far side hole element, you need to define its specifications by using the options of the Element Specification rollout in the PropertyManager. You can also add multiple far side elements by using the Insert Element Below Active Element and Insert Element Above Active Element buttons of the Far Side flyout.

Adding Cosmetic Threads
Advanced Modeling - III Adding Cosmetic Threads A Cosmetic thread represents the real thread of a feature. It is recommended to add cosmetic threads to holes, fasteners, or cylindrical features of a model.

To add a cosmetic thread, click on the Insert > Annotations > Cosmetic Thread in the SOLIDWORKS menus. The Cosmetic Thread PropertyManager appears.

Thread Settings The Circular Edges field of the Thread Settings rollout is activated by default. As a result, you can select a circular edge of a feature for adding the cosmetic thread. Click on a circular edge of a feature for adding cosmetic thread.

Standard The Standard drop-down list is used to select the type of standard such as ANSI Inch or ANSI Metric . Type The Type drop-down list is used to select the type of thread to be added. Size The Size drop-down list is used to select the standard size of the thread. Minor Diameter / Major Diameter The Minor Diameter / Major Diameter field is used to specify the minor/major diameter of the thread, respectively. End Condition The End Condition drop-down list is used to specify the end condition or termination for the cosmetic thread.

Thread Callout The Thread Callout field is used to enter text or comment for a thread, which appears in the thread callout of the drawing view. After specifying all parameters for adding cosmetic thread in the PropertyManager, click on the green tick mark in the PropertyManager. The respective cosmetic thread is added and appears in the graphics area.

The shaded display style of cosmetic thread is turned off. As a result, only the dotted circle representing the thread diameter appears in the graphics area.

Creating Threads Advanced Modeling - III
In SOLIDWORKS, in addition to adding cosmetic threads, you can create real threads on cylindrical or circular cut features by removing material from the model.

You can create a real helical thread on a cylindrical or a circular cut/hole features by using the Thread tool.

Thread Location By default, the Edge of Cylinder field in the Thread Location rollout is activated. As a result, you can select the circular edge of a cylindrical feature or a hole feature for creating a thread. The Offset check box is used to create the thread at an offset distance from the start location.

End Condition The End Condition rollout of the PropertyManager is used to specify the end condition or termination for the thread. Specification The Specification rollout is used to define specifications for the thread such as type and size.

By default, the Cut Thread radio button is selected as the thread method in the Specification rollout. As a result, the thread is created by removing the material from the model. On selecting the Extrude Thread radio button, you can create a thread by adding the material in the features.

Thread Options The Thread Options rollout is used to select the thread direction (clockwise or counter-clockwise) and align the thread to the start and end faces of the feature.

Creating Fillets Advanced Modeling - III Preview Options
The options in the Preview Options rollout is used to specify the type of preview to be appeared in the graphics area. Creating Fillets fillet is a curved face of a constant or variable radii and is used to remove sharp edges of a model that may cause injury while handling the model.

In SOLIDWORKS, you can create fillets by using two methods: Manual FilletXpert

Creating a Constant Radius Fillet A constant radius fillet is a fillet that has a constant radius throughout the selected edge.

Items To Fillet The options in the Items To Fillet rollout are used to select entities such as edges, faces, and features to create fillet. The options are as follows: Edges, Faces, Features and Loops NOTE: If you select a face to create a fillet, all the edges of the selected face are filleted and if you select a feature, all the edges of the selected feature are filleted.

Tangent propagation The Tangent propagation check box is used to apply fillet to all the edges that are tangent to the selected edge.

Show selection toolbar
The Show selection toolbar check box of the Items To Fillet rollout is selected by default. As a result, the Selection toolbar appears on selecting an entity for creating a fillet.

Full preview, Partial preview, and No preview The Full preview radio button is used to display full preview of the fillet, which includes the preview of all fillet edges. On selecting the Partial preview radio button, the partial view of the fillet appears. On selecting the No preview radio button, the display of preview is turned off. Fillet Parameters The options in the Fillet Parameters rollout are used to specify fillet parameters. The options are as follows:

Fillet Method The Fillet Method drop-down list is used to select the type of method to be used for creating fillet.

Multiple radius fillet By selecting the Multiple radius fillet check box, you can assign different radius values for the selected edges Profile The Profile drop-down list is used to select the type of fillet profile.

TIP: If the Rho value is less than 0.5 then the fillet profile is of elliptical shape. If the Rho value is 0.5 then the fillet profile is of parabola shape. If the Rho value is greater than 0.5 then the fillet profile is of hyperbola shape.

Setback Parameters A setback fillet is a fillet that has a smooth transition from fillet edges to a common intersecting vertex. Setback Vertices Distance Setback Distances Set All

Fillet Options Select through faces

Keep features

Creating a Variable Radius Fillet A variable radius fillet is a fillet that has variable radii. You can create a variable radius fillet by using the Variable Size Fillet button of the Fillet Type rollout.

Items To Fillet The Edges, Faces, Features and Loops field of the Items To Fillet rollout is activated by default. As a result, you can select edges, faces, features, or loops for creating variable radius fillet. Variable Radius Parameters The options in the Variable Radius Parameters rollout are used to define variable radius fillet.

Attached Radii The Attached Radii field displays a list of all vertices and control points of the selected edge or edges for defining a variable radii. Number of Instances The Number of Instances field is used to specify the number of control points on the selected edge for defining variable radii

Set All The Set All button is used to assign the radius value specified in the Radius field to all the control points and vertices of the edge. Set Unassigned The Set Unassigned button is used to assign the specified radius value to all control points and vertices whose radius value is not assigned. Smooth transition Straight transition

Creating a Face Fillets A face fillet is created between two non-adjacent or non-continuous faces of a model.

To create a face fillet, invoke the Fillet PropertyManager. Next, click on the Face Fillet button in the Fillet Type rollout of the PropertyManager.

Items To Fillet Face Set 1 The Face Set 1 field is used to select the first set of non-continuous faces. Face Set 2 The Face Set 2 field is used to select the second set of non-continuous faces of a model.

Creating a Full Round Fillet A full round fillet is created tangent to three adjacent faces of a model.

To create a full round fillet, invoke the Fillet PropertyManager and then click on the Full Round Fillet button in the Fillet Type rollout of the PropertyManager.

Items To Fillet Side Face Set 1 Center Face Set Side Face Set 2

Creating Chamfers Advanced Modeling - III
A chamfer is a bevel face that is non perpendicular to its adjacent faces.

To create a chamfer, click on the down arrow below the Fillet tool in the CommandManager. A flyout appears. Next, click on the Chamfer tool of the flyout. The Chamfer PropertyManager appears.

Chamfer Type The Chamfer Type rollout of the PropertyManager is used to select the type of chamfer to be created by clicking on the respective button in this rollout. Angle Distance Chamfer The Angle Distance button of the Chamfer Type rollout is used to create an Angle Distance chamfer by specifying its angle and distance values.

Distance Distance Chamfer The Distance Distance button is used to create a Distance Distance chamfer by specifying symmetric or asymmetric distance values on both sides of the chamfer edge.

Vertex Chamfer The Vertex button of the Chamfer Type rollout is used to create a Vertex chamfer on a vertex of a model.

Offset Face Chamfer The Offset Face button of the Chamfer Type rollout is used to create multiple chamfers of different sizes.

Face Face Chamfer The Face Face button of the Chamfer Type rollout is used to create a Face Face chamfer between non-adjacent or non-continuous faces of a model.

Creating Rib Features Advanced Modeling - III
Rib features act as supporting features and are generally used to increase the strength of a model. You can create a rib feature from an open or closed sketch by adding thickness in a specified direction.

To create a rib feature, create an open sketch on a plane that intersects with the model. Note that the projection of both the ends of the sketch should lie on the geometry of the model. After creating the sketch of the rib feature, click on the Rib tool in the Features CommandManager. The Rib PropertyManager appears.

Parameters The options in the Parameters rollout of the PropertyManager are used to specify parameters of the rib feature. Thickness The Thickness area of the Parameters rollout has three buttons: First Side, Both Sides, and Second Side. Rib Thickness The Rib Thickness field is used to specify the thickness value of the rib feature.

Extrusion direction The Extrusion direction area has two buttons: Parallel to Sketch and Normal to Sketch.

Flip material side The Flip material side check box is used to flip the direction of extrusion of the rib feature. Draft On/Off The Draft On/Off button is used to add draft to the rib feature. Selected Contours The Selected Contours rollout is used to select the required contour of the sketch for creating the rib feature.

Creating Shell Features
Advanced Modeling - III Creating Shell Features A shell feature is a thin walled feature, which is created by making a model hollow from inside.

To create a shell feature, click on the Shell tool in the Features CommandManager. The Shell PropertyManager appears.

Thickness The Thickness field is used to specify wall thickness for the shell feature. Faces to Remove The Faces to Remove field is used to select the faces of the model to be removed.

Shell outward On selecting the Shell outward check box, thickness is added outward to the model. Show preview On selecting the Show preview check box, the preview of the shell feature appears in the graphics area. Multi-thickness Settings The options in this rollout are used to create multi-thickness shell feature. Multi-thickness Faces

Creating Wrap Features
A Wrap feature is created by wrapping a sketch onto a face or faces of a model. Wrap Type The options in the Wrap Type rollout of the PropertyManager are used to select the type of wrap.The options are as follows: Emboss Deboss Scribe

Wrap Method Analytical Spline Surface Wrap Parameters
The options in the Wrap Method rollout of the PropertyManager are used to select a method for creating the wrap feature. Analytical Spline Surface Wrap Parameters The options in the Wrap Parameters rollout are used to specify parameters for creating the wrap feature.

Source Sketch Face for Wrap Sketch Thickness Depth
The Source Sketch field of the PropertyManager is used to select a sketch to be wrapped. Face for Wrap Sketch The Face for Wrap Sketch field is used to select a face or faces of a model for wrapping the sketch. Thickness The Thickness field is used to specify thickness of the wrap feature. Depth The Depth field is used to specify the depth of the wrap feature.

Reverse Direction The Reverse Direction check box is used to reverse the direction of projection.

Tutorial 1 Advanced Modeling - III
Create the model shown in the figure given below. All dimension are in mm. To create this tutorial, follow the steps given in the textbook.

Tutorial 2 Advanced Modeling - III
Create the model shown in the figure given below. All dimension are in mm. To create this tutorial, follow the steps given in the textbook.

Hands-on Test Drive 1 Advanced Modeling - III
Create the model shown in the figure given below. All dimension are in mm.

Hands-on Test Drive 2 Advanced Modeling - III
Create the model shown in the figure given below. All dimension are in mm.

Summary Advanced Modeling - III
In this chapter, you have learned how to create standard or customized holes such as counterbore, countersink, straight tap, tapered tap, and multi-stepped holes as per standard specifications. Also, you have learned that cosmetic threads can be used to represent real threads on the holes, fasteners, and cylindrical features to reducing the complexity of a model and improve the overall performance of the system. In addition to the cosmetic threads, you have also learned how to create the realistic threads on a cylindrical feature or cut/hole feature of a model. You can add constant and variable radius fillets to remove the sharp edges of a model. In addition, you have learned about various methods of adding chamfer on the edges of a model. You can create a rib feature by using the open or closed sketch. At last, you have learned about creating the shell and wrap features.

Questions Advanced Modeling - III
The ________ tool is used to create standard holes such as counterbore and countersink. The ________ tool is used to add cosmetic threads to holes, fasteners, and cylindrical features. Using the Fillet tool, you can create ________ , ________ , ________ , and ________ fillets. If the Rho value is less than ________ then the resultant fillet profile becomes elliptical in shape. The ________ fillet is created tangent to three adjacent faces of a model. The ________ fillet is created between the two non-continuous faces of a model.

You can create a rib feature by using the open or closed sketch. (True/False). You cannot create a rib feature with a draft angle. (True/False). While creating a hole by using the Hole Wizard tool, you cannot customize the size of hole. (True/False). Using the Hole Wizard tool, you can create counterbore slot, countersink slot, or slot holes. (True/False).

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