FEATURE OPERATIONS

Feature operations are performed on the basic form features to smooth corners, create tapers, and unite or subtract certain solids from other solids. Some of the feature operations are shown below.

Let us see the different types of feature operation commands in NX5 and the function of each command.


TYPES OF FEATURE OPERATIONS
The features operations used in NX include Edge blend, Face blend, Soft blend, Chamfer,Hollow, Instance, Sew, and Patch. Let us see some of the important commands in details. Unlike the NX3 version, some of the feature operations have been removed in NX5. For example, the Taper operation has been removed. In addition, changes have been made to the way a few
operations are performed. For example, the Trim Body operation no longer supports solid bodies as tools for trimming. Some of the feature operations such as Split Body cannot be accessed from the INSERT menu and have to be opened using the Toolbar.


Edge Blend

An Edge Blend is a radius blend that is tangent to the blended faces. This feature modifies a solid body by rounding selected edges. This command can be found under Insert → Design Feature. You can also do a face
blend.

Chamfer
The chamfer function operates very similarly to the blend function by adding or subtracting material relative to whether the edge is an outside chamfer or an inside chamfer. This command can also be found under the Insert → Design Feature menu.
You can preview the result of chamfering and if you are not happy with the result you can undo the operation.

Thread
Threads can only be created on cylindrical faces. The Thread function lets you create symbolic or detailed threads (on solid bodies) that are right or left handed, external or internal, parametric,and associative threads on  cylindrical faces such as holes, bosses, or cylinders. It also lets you select the method of creating the threads such as cut, rolled, milled or ground. You can create different types of threads such as metric, unified, acme and so on. To use this command, go to Insert → Design Feature

 Trim Body
A solid body can be trimmed by a sheet body or a datum plane. You can use the Trim Body function to trim a solid body with a sheet body and at the same
time retain parameters and associativty. To use this command, go to 
Insert → Trim

Split Body
A solid body can be split into two just like trimming it. It can be done by a plane or a sheet body. Click on the icon in the Form Feature Toolbar as shown to open the Split Body dialog box.

Instance
A Design feature or a detail feature can be made into dependent copies in the form of an array. It can be Rectangular or Circular array or just a Mirror. This particularly helpful feature saves plenty of time and modeling when you similar features for example threads of gear or holes on amounting plate, etc. This command can be found by going to Insert → Associative Copy →

Instance Feature.

Boolean Operations

Boolean operations are:
• Unite
• Subtract
• Intersect
These options can be used when two or more solid bodies share the same model space in the part file. 
To use this command, go to Insert → Combine Bodies.
Consider two solids given. The block and the cylinder are next to each other as shown below. 

Unite:
The unite command adds the Tool body with the Target body. For the above example, the output will be as follows if Unite option is used.

Subtract:
When using the subtract option, the Tool body is subtracted from the Target body. The following would be the output if the rectangle is used as the Target and the cylinder as the Tool.

Intersect:
This command leaves the volume that is common to both the Target body and the Tool body.The output is shown below

Editing a Hole Feature

After creating a hole, you may need to edit its parameters. The parameters that can be edited in NX include the diameters, depth, and the positioning values of the hole. To modify the parameters of a simple hole, double-click on it; the Edit Parameters dialog box will be displayed if the hole is created by the Pre-NX5 Hole tool, as shown in Figure 

Also, the parameters of the hole will be displayed on the model, as shown in Figure .

Note
In case, the hole is created by the Hole tool, the Hole dialog box will be redisplayed. In this dialog box, you can redefine the parameters of the hole.

Feature Dialog Button
To modify the parameters of the hole, choose the Feature Dialog button from the Edit Parameters dialog box; the Diameter, Depth, and Tip Angle edit boxes will be displayed. If the hole selected is a counterbore or a countersink hole, the counter related values will also be displayed. Enter the new values in the respective edit boxes and choose the OK button; the original options of the Edit Parameters dialog box will be restored. Choose the OK button from this dialog box; the changes made in the parameter values of the hole will be
reflected in the model. 

Reattach Button
To change the placement face of the hole, choose the Reattach button from the Edit Parameters dialog box; the Reattach dialog box will be displayed, as shown in Figure 

By default, the Specify Target Placement Face button is chosen from the Selection Steps area and you will be prompted to select the target face. Select a new placement face to reattach the hole. On doing so, the Redefine Positioning Dimensions button will be automatically chosen from the Selection Steps area of the Reattach dialog box. To retain the same positional values for the hole on the new placement face and create it, choose the OK button.
To specify new positional values for the hole, select the dimension to be modified; a dialog box will be displayed and it will be named based on the type of dimension used to place the hole. Also, you will be prompted to select the target object. Select an edge or datum to define the new reference for the dimension in the new placement face; you will be prompted to select the reference from the tool (hole). Select the bottom circular edge from the hole; the Select Arc Position dialog box will be displayed. To define the positional value between the selected edge/datum and the center point of the hole, choose the Arc Center button from the Select Arc Position dialog box. To define the positional value between the selected edge/ datum and any of the quadrant points of the hole, choose the End Point button. To define
the positional value between the selected edge/datum and the tangent point on the bottom edge of the hole, choose the Tangent Point button. After specifying the dimension, choosethe OK button from the Select Arc Position dialog box. Also, choose the OK button from the
Reattach dialog box; the changes will be reflected in the model.

Note
You can also delete the hole dimensions using the Reattach dialog box. To do so, choose the Delete Positioning Dimension button from the Reattach dialog box and then select the dimension to be deleted.

Test your self:3

1. The Reordering Features option allows you to change the order in which the features are created. (T/F)
2. Boss can be placed on a nonplanar surface. (T/F)
3. In NX, you can create three types of pockets. (T/F)
4. The pad feature is defined as the process of adding material to the model. (T/F)
5. In the Tangent to Faces draft type, there is no need to select a stationary plane. (T/F)
6. General pockets can be created on both _________ and _________ faces.
7. In NX, you can create _________ types of drafts.
8. In a draft tool, the _________ check box allows you to select whether to taper only the specified instance or all instances in the array features.
9. The Tangent to Faces type is used to create a draft, which is _________ to the selected faces.
10. The length of the rectangular pad will be _________ to the horizontal reference.



key:
1.T, 2. F, 3. T, 4. T, 5. T, 6. planar, nonplanar, 7. four, 8. Draft All Instances, 9. tangent, 10.
parallel.

ROTATING THE VIEW OF A MODEL IN 3D SPACE

NX provides you with an option of rotating the view of a solid model freely in
3-dimensional (3D) space. This enables you to visually maneuver around the solid model and view it from any direction. To do so, choose the Rotate button from the View toolbar; the cursor changes to the rotate view cursor and you will be prompted to drag the cursor to rotate the model. Next, press and hold the left mouse button and drag the cursor; the view of the model will be rotated and you can visually maneuver around it.


You can also rotate the view around the X, Y, or Z-axis of the current view. To rotate the view around the X-axis of the current view, invoke the Rotate tool and move the cursor close to the left or right edge of the drawing window; the cursor changes to the X-rotate cursor. Press and hold the left mouse button and drag the cursor; the view will be rotated around the X-axis of the current view. Move the cursor close to the bottom edge of the drawing window and drag the cursor to rotate the view around the Y-axis of the current view. Similarly, move the cursor close to the top edge of the drawing window and drag the cursor to rotate the view around the Z-axis of the current view. Figure below shows the X, Y, and Z rotate cursors. 

HIDING & SHOWING ENTITIES

Whenever you create a sketch-based feature, the sketch used to create it is retained on the screen, even after the feature is created. NX allows you to hide the sketches or any other entity on the screen using the Hide tool. To invoke this tool, press the CTRL+B keys; the Class Selection dialog box will be displayed. Alternatively, you can invoke the Hide tool from the Utility toolbar. Select the sketch or any other entity from the screen using this dialog box and choose the OK button; the selected entities will be hidden


SHOWING HIDDEN ENTITIES

To restore the display of the hidden entities, press the SHIFT+CTRL+K keys; the Class Selection dialog box and the hidden entities will be displayed. Also, you will be prompted to select the objects to be displayed. Select the entities to be displayed and then choose the OK button.


HIDING ALL ENTITIES USING A SINGLE TOOL

NX allows you to hide all entities (all datum planes, coordinate systems, sketches,faceted bodies, solid bodies, and so on) from the drawing window, using a single tool.To do so, choose the Show and Hide button from the Utility toolbar; the Show and Hide dialog box will be displayed, as shown in Figure 

click on image to enlarge

All entities are divided into three categories, Bodies, Sketches, and Datums. Select the minus sign (-) from the respective rows; the corresponding entities will be hidden. For example, if you need to hide all the sketches in the drawing window, select the minus sign (-) from the Sketches row; all the sketches will be hidden. Similarly, to show hidden entities, select the plus sign (+) from the respective row; all entities under that category will be re-displayed in the drawing window.


Toolbar: Utility > Show
Toolbar: Utility > Show and Hide



TIP:The Show and Hide tool is very useful while working with complicated models and assemblies, where datums planes, coordinate systems, and sketches are in large numbers.You can also invoke this tool by pressing the CTRL+W keys.

Creating a solid model using REVOLVE command

The Revolve tool allows you to create a solid body by revolving a sketch around the revolution axis, which could be a sketched line or an edge of an existing feature. Figure below shows a sketch for the revolved feature and

 Figure shows the Isometric view of the resulting feature revolved through an angle of 270-degree.

To convert a sketch into a revolved body, you need to invoke the Revolve tool. This tool works in the following three steps:
Step 1: Select the sketch to be revolved
Step 2: Select the revolution axis
Step 3: Specify the revolution parameters
To invoke the Revolve tool, choose the revolve button in the Feature dialog box; the Revolve dialog box will be displayed, as shown in Figure 

click on the picture to enlarge

 The options in this dialog box are same as the options in the Extrude dialog box, except the ones that are explained next.


Axis Rollout
The options in this rollout are used to specify the revolution axis. These options are discussed next.
Specify Vector
The options in this area are used to specify the revolution axis using the Vector Constructor button or the Inferred Vector drop-down list.
Vector Constructor
When you choose this button, the Vector dialog box will be displayed. You can specify the revolution axis by using this dialog box.

Inferred Vector
This drop-down list is a shortcut to specify the revolution axis.
Reverse Direction
You can choose this button to flip the direction of revolution.
Specify Point
The options in this area are used only when you use the vector method to specify the revolution axis.
Point Constructor
When you choose this button, the Point dialog box will be displayed. You can specify the point to define the revolution axis using this dialog box.
Inferred Point
This drop-down list contains the snap point options that are used to automatically snap the keypoints of the previously sketched entities or features



Limits Rollout
The options in this rollout are used to specify the start and termination angles of revolution.These options are discussed next.
Start Drop-down List
This drop-down list allows you to specify the start angle of the revolution feature. You can select the Value and Until Selected options from this drop-down list. The Value option allows you to enter the value of the start angle in the Angle edit box. You need to enter a positive value of the angle. This value will be taken as the offset value between the sketch and the start of the revolved feature. The Until Selected option allows you to start the revolve
feature from the selected plane, face, or body. When you select this option, the Face, Body,Datum Plane button will be chosen and you will be prompted to select the face, body, or datum plane to start the revolved feature.
End Drop-down List
This drop-down list allows you to specify the termination angle of the revolution feature. You can select the Value and Until Selected options from this drop-down list. The Value option allows you to enter the value of the end angle in the Angle edit box. You need to enter a positive value of the angle. This value will be taken as the offset value between the sketch and the end of the revolved feature. The Until Selected option allows you to terminate the
revolve feature using the selected plane, face, or body. When you select this option, the Face, Body, Datum Plane button will be chosen and you will be prompted to select the face, body, or datum plane to start the revolved feature.


The default value of the end angle is the value that you have used to create the last revolved feature. Figure below shows a revolved feature with the start angle as 30 degree and the end angle as 180-degree. The sketch used to create this feature is also displayed.

Note that NX uses the right-hand thumb rule to determine the direction of revolution. This rulestates that if the thumb of your right hand points in the direction of the axis of revolution, then the direction of the curled fingers will define the direction of revolution, refer to Figure

Figure below shows the sketch and an arrow pointing in the direction of the axis of revolution

and Figure below shows the resulting feature revolved through an angle of 180 degree.

And the sketch and an arrow pointing in the direction of the axis of revolution

the resulting feature revolved through an angle of 180-degree.

Offset Rollout
NX also allows you to create thin revolved bodies using the open and closed sketches. This process is similar to that of creating solid extruded features. Select the Offset rollout in the Revolve dialog box; the rollout will expand and display the Offset drop-down list. There is only one option, Two-Sided, available in this drop-down list. Select this option; the Start and the End edit boxes will be available. Enter the start and end offset values in the respective
edit boxes. Figure below shows a thin revolved model with the open sketch and the revolution axis used to create it. In this model, the start angle is 30 degree, the end angle is 180-degree, and the start offset value is 2.

Figure below shows a thin revolved model with the closed sketch and the revolution axis used to create it. In this model, the start angle is 45 degree, the end angle is 270-degree, and the start offset value is 2.

SETTING DISPLAY MODES

You can set the display modes for the solid models using the buttons in the View toolbar. Figure shows the partial display of the View toolbar with various buttons and flyout options that you can use to set the display modes of the model

COLOR SCHEME

NX allows you to use various color schemes as the background screen color and also for displaying the solid bodies on the screen. To change the background color scheme, choose Preferences > Background from the menu bar; the Edit Background dialog box will be displayed.
Select the Plane radio button from the Shaded Views and Wireframe Views areas. Next,choose the color swatch available on the right side of the Plain Color option; the Color dialog box will be displayed. Select the White color swatch from the Colors dialog box and choose the OK button twice to apply the new color scheme to the NX environment. 
Note that all the files that you open henceforth will not use this color scheme.

Creating a solid model using EXTRUDE command

Extrude is defined as the process of creating a feature from a sketch by adding the material along the direction normal to the sketch or any other specified direction.

Above Figure shows the isometric view of a closed sketch 

and  above Figure shows the extruded feature created using this sketch.



When you invoke the Extrude tool, the Extrude dialog box will be displayed, as shown in Figure

 You will be prompted to select the planar face to sketch or the section geometry to be extruded. If you select the sketch at this stage, the preview of the extruded feature created using the default values will be displayed on the screen. If you select the sketch plane, the Sketcher environment will be invoked. Draw the sketch and exit the Sketcher environment; the
preview of the extruded feature will be displayed in the Modeling environment.


Extrude Dialog Box Options
The options in this dialog box are discussed next.

Section Rollout
The options in this rollout are used to sketch the section or select the section. By default,both the Sketch Section and Curve buttons will be chosen in this rollout and you will be prompted to select the planar face to sketch or the section geometry to be extruded. These options are discussed next.
Sketch Section
This button is used to draw the sketch for extrusion. When you choose this button, the Create Sketch dialog box will be displayed and you will be prompted to select the object for the sketch plane. You can select a datum plane or the face of a solid body as the sketching plane.
Curve
By default, this button is also chosen from the Section rollout and it is used to select the already drawn section sketch.
Direction Rollout
By default, the direction of extrusion will be normal to the selected section. The buttons in this rollout are used to define the direction of extrusion. These options are discussed next.

Vector Constructor
If you choose this button, the Vector dialog box will be displayed. You can specify the extrude direction using this dialog box.
Inferred Vector Drop-down List
This drop-down list is used to specify the direction of extrusion. The default direction is normal to the selected section.
Reverse Direction
This button is chosen to flip the current extrusion direction.
Limits Rollout
The options in this rollout are used to specify the start and termination of the extrusion.
These options are discussed next.
Start Drop-down List
This drop-down list allows you to specify the start point of the extrusion. You can select the Value and Symmetric Value options from this drop-down list. The Value option allows you to specify the distance from the sketching plane at which the extruded feature will start. You need to enter this value in the Distance edit box. If you enter a positive value, it will be taken as the offset value between the sketch and the start of the extrusion feature. If you enter 0,
the extruded feature will start from the sketch plane. If you enter a negative value, the extruded feature will start from below the sketch plane. The Symmetric Value option allows you to extrude the sketch symmetrically in both the directions of the current sketching plane. When you select this option, the edit boxes on the right of the Start and the End edit boxes will show identical values and the preview will also be modified dynamically.
Figure shows the preview of a sketch being extruded symmetrically in both the directions.

Preview of the symmetric extrusion

End Drop-down List
This drop-down list allows you to specify the extrusion termination in the
direction of extrusion. For the base feature, only the Value and Symmetric Value options will be available in this drop-down list. By default, the Value option will be selected, and the value entered last will be displayed in the Distance edit box. As a result, the sketch will be extruded only in the specified direction. Note that you need to enter a positive value in the Distance edit box.
Figure shows the preview of the extrusion in only one direction 

 Figure shows the preview of the extrusion with different values in both directions. In this figure,the extrusion value in the upward direction is 10 and in the downward direction is -5.

Boolean Rollout
Options in this rollout allow you to select the boolean operation that you need to perform. These options in this rollout are discussed in the next chapter.
Draft Rollout
The options in this rollout are used to specify a draft angle to the extrusion feature. The options in this area will be available only when you select the section to extrude. Various draft options in this rollout are discussed next.
Angle
This edit box allows you to specify the draft angle.
Draft
This drop-down list allows you to specify the type of draft to be applied to the feature.
The options in this area are discussed next.
From Start Limit
This option adds the draft from the start section to the end section of the extruded feature. As a result, the dimension of the feature at the start section is the same as that of the original sketch and it tapers toward the end section. 
Figure shows thepreview of the extruded feature drafted using this option. 

It is evident from this figure that the bottom section of the extruded feature is the same as that of the original sketch and the feature tapers as it goes toward the top section.



From Section
This option is used to taper the extruded surface in such a way that the cross-section of the extruded feature remains the same at the sketching plane, as shown in Figure

From Section - Symmetric Angle

This option is available only when you select the Symmetric Value option from the Limits rollout or specify the values in both the start and the end directions. This option adds a symmetric taper in both directions of the sketch, as shown in Figure.

In this draft type, if the distance value in one of the directions is more than the other, the section in that direction will also be smaller in size.


From Section - Matched Ends
This option is also available only when you select the Symmetric Value option fromthe Limits rollout or specify the values in both the start and the end directions. Thisoption tapers the model such that the end sections in both the directions are of similar size, irrespective of the distance values in both directions, as shown in Figure 

From Section - Asymmetric Angle

This option is also available only when you select the Symmetric Value option fromthe Limits rollout or specify the values in both the start and the end directions. This option adds different tapers in both directions of the sketch, as shown in Figure 

When you select this option, the Front Angle and Back Angle edit boxes will be
available in the Draft rollout. The front and back angle values will be applied at the front and back sides of the sketching planes used to create the extruded feature.



Offset Rollout
NX also allows you to create thin base features by extruding open or closed sketches. For example, refer to the closed sketch shown in Figure 

 A thin feature created using this sketch is shown in Figure

 Similarly, Figure shows an open sketch 

and Figure shows the resulting thin feature.

Two-Sided
This option is used to create a thin feature by offsetting the sketch in two directions.Select this option; the Start and End edit boxes will be displayed. If you enter the positive value in the End edit box, the sketch will offset outward and vice-versa.
Figure shows the preview of a thin feature with an offset only in the end direction

and Figure  shows the preview of the same feature with an offset in both the directions

Single-Sided
This option will be enabled only when you create a thin feature using a closed sketch with no nested closed sketch in it. If you select this option, the inner portion of the sketch will be filled automatically. As a result of this, there will be no cavity inside the model. It will be similar to the solid extrusion from inside. However, you can also add some offset to the outer side of the sketch.


Symmetric
This option is used to offset the material symmetrically on both sides of the sketch to create the thin feature.



Settings Rollout
The options in this rollout are used to specify whether you need the extruded feature to be a sheet body or a solid body. To get a solid body, the section must be a closed profile or an open profile with an offset. If you use a Single-Sided offset, you will not be able to get a sheet body.
You can select the required option from the Body Type drop-down list.
Preview Rollout This rollout is used to preview the model dynamically while modifying the values in the Extrude dialog box. If you select the Preview check box, it will allow you to dynamically preview the changes in the model as you modify the values of the extrusion. The Show Result button is used to view the final model. The Undo Result button is used to go back to the preview mode.
After setting the values in the Extrude dialog box, choose OK to create the extruded feature and exit the dialog box. If you need to extrude more than one sketches, choose the Apply button; the selected sketch will be extruded and the dialog box will be retained. Also, you will be prompted to select the section geometry. Select the other sketch to extrude and choose the OK button.
You can also set and modify the values of extrusion using the drag handles that will be displayed in the preview of the extrusion feature, refer to Figure.

The start drag handlewill be a filled circle and the end drag handle will be an arrow. To modify the start limit, end limit, or draft angle values, click on their respective drag handles, and then press and hold the left mouse button and drag the mouse. You can also enter the new values in the edit boxes that will be displayed after clicking on the respective handles. To modify the type of limits or taper, right-click on their respective drag handles and select the type from the shortcut menu.