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.