Tool bars

Toolbars contain icons, which serve as shortcuts for many NX functions. The following figure shows the main Toolbar items normally displayed. However, you can find many more icons for different feature commands, based on the module selected and how the module is customized.


􀂾 Right-Click anywhere on the existing toolbars gives a list of
other Toolbars. You can add any of the toolbars by checking

them. 
The list of toolbars you can see in the default option is Standard, View, Visualization, Selection, Object Display, etc. Normally, the default setting should be sufficient for most operations but during certain operations, you might need additional toolbars. If you want to add buttons pertaining to the commands and toolbars, 


􀂾 Click on the pull-down arrow on any of the Toolbars and choose
ADD OR REMOVE BUTTONS.
􀂾 Choose CUSTOMIZE



This will pop up a Customize dialog window with all the Toolbars under ‘Toolbar’ Tab and commands pertaining to each Toolbar under ‘Commands’ tab. You can check all the toolbars that you wish to be displayed.

You can customize the settings of your NX interface by clicking on the Roles tab on the Resource Bar

The Roles tab has different settings of the toolbar menus that are displayed on the NX interface.

• It allows you to customize the toolbars you desire to be displayed in the Interface.
• Selecting Advanced shows all the Application Toolbars necessary for drafting and modeling.
• You can also select the Application Toolbars to be displayed in the Interface by clicking on the Industry Specific settings. This provides a list of industry
specific toolbar applications as shown below.

Model a Hexagonal Nut

􀂾 Create a new file and save it as Impeller_hexa-nut
􀂾 Click the polygon icon from the toolbar

􀂾 Create a hexagon with each side measuring 0.28685 inches and constructed at the origin
􀂾 Extrude the hexagon by 0.125 inches
The figure of the model is shown below.

􀂾 Choose INSERT → DESIGN FEATURE → SPHERE
􀂾 Choose CENTER, DIAMETER

􀂾 Enter the diameter value 0.57 inches
􀂾 Enter the Point Constructor values as follows

Axes            XC      YC           ZC
Dimension   0.0      0.0       0.125

􀂾 In the Boolean operations dialog box select INTERSECT
The model will look like the following.

We will now use a Mirror command.
􀂾 Choose EDIT → TRANSFORM
􀂾 Select the model and click OK
􀂾 Click MIRROR THROUGH A PLANE
􀂾 Click on the flat side of the model as shown. Be careful not to select any edges
Click on OK

􀂾 Click on COPY
􀂾 Click CANCEL

You will get the following model.
􀂾 Choose INSERT → COMBINE BODIES → UNITE

􀂾 Select the two halves and Unite them
􀂾 Insert a cylinder with the vector pointing in the Z-direction
and with the following dimensions.
Diameter = 0.25 inches
Height = 1 inch
􀂾 Center the cylinder on the origin and subtract this cylinder
from the hexagon nut

Now, we will chamfer the inside edges of the nut.
􀂾 Choose INSERT → DETAIL FEATURE → CHAMFER

􀂾 Select the two inner edges as shown and click OK

􀂾 Enter the Chamfer Offset Diameter as 0.0436 inches and click OK
You will see the chamfer on the nut. Save the model.

Introduction to manufacturing

The models and drawings created by the designer have to undergo other processes to get to the finished product. This being the essence of CAD/CAM integration, the most widely and commonly used technique is to generate program codes for CNC machines to mill the part. This technological development reduces the amount of human intervention in creating CNC codes. This also facilitates the designers to create complex systems. The manufacturing module allows you to program and do some post-processing on drilling, milling, turning and wire-cut edm tool paths.



A few preparatory steps need to be performed on every CAD model before moving it into the CAM environment.Before getting started, it would be helpful if you can get into a CAM Express Role. To do this, go to the Roles menu on the Resource Bar and click on the INDUSTRY SPECIFIC tab. A dropdown
menu will pop up in which the CAM Express role can be seen as shown in the figure

Threading of a hexagonal bolt

Open the model with Hexagonal nut from my previous post:


http://unigraphicsbasicsnmaterial.blogspot.com/2011/12/model-hexagonal-screw.html

• Choose INSERT → DESIGN FEATURE →THREAD

Here you will see the threading dialog box as shown below.


There are two main options in Threading: 
1)Symbolic and 2) Detailed.

• Click on the DETAILED radio button
• Keep the thread as RIGHT HANDED
• Click on the bolt shaft, the long cylinder below

the hexagon head Once the shaft is selected, all the values will be displayed in the Thread dialog box. Keep all these default values.

• Click OK

The hexagon bolt should now look like the following. Save the model.

Model a Hexagonal Screw

Create a new file and save it as Impeller_hexa-bolt

• Choose INSERT → DESIGN FEATURE → CYLINDER
• The cylinder should be pointing in the Z-direction with the center set at the origin and with the following dimensions:

Diameter = 0.25 inches
Height = 1.5 inches

Now create a small step cylinder on top of the existing cylinder.

• The dimensions of this cylinder are,

Diameter = 0.387 inches

Height = 0.0156 inches 

• On the Point Constructor window,click the Center icon at the top
• Click on the top face of the existing

cylinder as shown in the following figure



Under the Boolean drop-down menu,
choose UNITE

The two cylinders should look like the figure shown below.

Save the model.
Next, we will create a hexagon for the head of the bolt.

• Choose the icon from the Curves Toolbar as shown

• On the Polygon window, type 6 for the number of sides

• Click OK

There are three ways to draw the polygon.
• Inscribed Radius
• Side of Polygon
• Circumscribed Radius

• Choose SIDE OF POLYGON

On the next window, enter the following dimensions.
Side = 0.246 inches
Orientation Angle = 0.00 degree

• Click OK
• On the Point Constructor window, again choose the Center icon
• Click on the top face of the last cylinder drawn 

The polygon will be seen as shown below. 

If the model is not in wireframe, click on the Wireframe icon in the View Toolbar


Now we will extrude this polygon.

• Choose INSERT → DESIGN FEATURE → EXTRUDE
• Click on all six lines of the hexagon to choose the surface that is required to be extruded
• Enter the End Distance as 0.1876 inches

The model looks like the following after extrusion

On top of the cylinder that has a diameter of 0.387 inches, insert another cylinder with the following dimensions.


Diameter = 0.387 inches
Height = 0.1875 inches


You will only be able to see this cylinder when the model is in wireframe since the cylinder is inside the hexagon head. The model will look like the following.

We will now use the feature operation Intersect.

• Choose INSERT → DESIGN FEATURE → SPHERE
• Choose DIAMETER, CENTER

• Enter the value of the diameter as 0.55 inches and click OK
• On the Point Constructor window, choose the Center icon
• Select the bottom of the last cylinder drawn, which is inside the hexagon head and has a diameter of 0.387 inches and a height of 0.1875 inches as shown below

Click OK



This will give take you the next Dialog box which will ask you to choose the Boolean operation to be performed.

• Choose INTERSECT

It will ask you to select the target solid

• Choose the hexagonal head as shown 

• Click CANCEL

This will give you the hexagonal bolt as shown below.

Check here how to add threading to the above bolt in the next post:


http://unigraphicsbasicsnmaterial.blogspot.com/2011/12/threading-of-hexagonal-bolt.html

Test yourself:4

1. In NX, Surfaces are termed as sheets. (T/F)
2. The Trim and Extend tool is used to trim or extend an open or closed surface. (T/F)
3. You can use the Until Selected and Until Next options from the End drop-down list of the Extrude dialog box to create a sheet. (T/F)
4. The default tolerance value for the creation of sheet by is 0.0254. (T/F)
5. The maximum number of sections that can be used to create a sheet using the Ruled tool from the Surface toolbar is ____________.
6. The ____________ tool is used to create a sheet from n number of guide curves and n number of section curves.
7. The ____________ tool is used to stitch individual surfaces into a single surface.
8. The ____________ tool is used to trim and extend a surface.
9. The ____________ tool is used to create a planar surface.
10. The ____________ tool is used to create a surface offset.


Answers :
1. T, 2. T, 3. F, 4. T, 5. Two, 6. Studio Surface, 7. Sew, 8. Trim and Extend, 9. Bounded Plane,
10. Offset Surface