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In This Chapter
23
Creating Shafts
The shaft generator in Autodesk
®
Mechanical Desktop
®
6
is an automated feature that eliminates the need for
many of the manual steps previously required to create
shafts.
In this tutorial, you learn how to design shafts using the
shaft generator. You create a shaft with segments of
different shapes, and add threads and a profile. Then
you edit the shaft and add standard parts to it. Finally,
you check your design in front and isometric views with
wireframe and shaded displays.
Run Mechanical Desktop with the power pack to
perform this tutorial.
■
New in this tutorial
■
Using the Shaft Generator
■
Creating shaft geometry
■
Adding thread and profile
information to a shaft
■
Editing a shaft
■
Adding standard parts to a shaft
■
Shading and displaying 3D views
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Key Terms
Term
Definition
bearing calculation
Calculates limiting value, dynamic and static load rating, dynamic and static
equivalent load, and fatigue life of bearing in revolutions and hours.
centerline
Line in the center of a symmetrical object. When you create centerlines, you
specify the start and end points.
chamfer
A beveled surface between two faces or surfaces.
dynamic calculation
Calculation required for a revolving bearing. The result is the Adjusted Rating Life.
This is the life of the bearing associated with 90% reliability with contemporary,
commonly used material, and under conventional operating conditions. With the
number of revolutions you get the life in working hours.
dynamic dragging
The act of determining the size of a standard part with the cursor while inserting
it into a side view. The standard part is displayed dynamically on the screen and
can be dragged to the next possible size and length. The values (sizes) are taken
from the Standard parts database.
shaft generator
Tool to draw rotationally symmetric parts.
UCS
User coordinate system. Designated by arrows that signify the XY coordinates.
Establishes a construction plane and simplifies location of 3D points. Provides
visual reference for positioning a surface.
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Tutorial at a Glance
It is no longer necessary to create a cylinder manually and define new sketch
planes and work planes in order to create a shaft. Instead, you make selec-
tions in the 3D Shaft Generator dialog box, and enter values to further define
your selections.
In this tutorial you use this automated feature to
■
Create a shaft with cylindrical and conical sections.
■
Add threads and a profile to the shaft.
■
Edit the shaft.
■
Add standard parts to the shaft.
■
Shade and display 3D views of the shaft.
Basic Concepts of the Shaft Generator
The shaft generator is an automated feature for creating shafts of many con-
figurations, including outer and inner shaft contours for hollow shafts, You
define the different segments of a shaft using the options in the 3D Shaft
Generator dialog box.
As you select and define each segment, it is generated automatically and
added to the shaft. Usually, you work from left to right as you add different
types of segments, such as cylinders, cones, thread, profiles, and grooves.
Shaft segments can be inserted, deleted, or edited.
Each element of a shaft is generated from the segment preceding it. When
you delete a shaft element, you also delete the shaft elements that follow.
As you create shaft segments, corresponding icons for the work features and
shaft contours are displayed in the Desktop Browser.
While you are creating the shaft, it is helpful to display front and isometric
views using two viewports. Toggling between wireframe and shaded displays
also makes it easier to visualize your design.
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Using the Shaft Generator
You use the 3D Shaft Generator dialog box to select a type of shaft segment,
such as a cylinder or a cone, and then you define that segment. The shaft
generator creates the segment automatically and adds it to the previous
segment.
Getting Started
In order to work through this tutorial chapter, the ISO standard system has
to be installed at your system.
Moreover, you need to set your measurement units to metric. This can easily
be done by selecting an appropriate drawing template. Open the drawing
template acadiso.dwt.
To open a drawing template
1
Open a new template.
Menu
File ➤ New
Command
NEW
The AutoCAD Mechanical Today window is displayed.
2
In the AutoCAD Mechanical Today window, in the section My Drawings,
change to the tab Create Drawings, and select the template acadiso.dwt.
Now, you are working with the selected template.
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Creating Shaft Geometry
You start creating the shaft by defining the segments that govern its shape.
In the 3D Shaft Generator dialog box, you select the first segment type and
then you define that segment. You continue adding segments until the con-
tour of the shaft is complete.
To create a shaft using the shaft generator
1
Use
AMSHAFT3D
to define the shaft.
Menu
Content 3D ➤ Shaft Generator
Respond to the prompts as follows:
Specify start point or [Existing shaft]:
Select a point in the drawing
Specify centerline endpoint:
Drag a line to the right, and select a point
Specify point for new plane <parallel to UCS>:
Press
ENTER
The 3D Shaft Generator dialog box is displayed.
Define the shaft contour, starting with the segment at the left, and working
to the right.
2
Verify the Outer Contour tab is selected, then choose the lower Cylinder icon.
Respond to the prompts as follows:
Specify length or [Associate to/Equation assistant] <50>:
Enter 10
Specify diameter or [Associate to/Equation assistant] <40>:
Enter 74
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3
Choose the Slope icon, and respond to the prompts as follows:
Specify length or [Dialog/Associate to/Equation assistant] <10>:
Enter 7
Specify diameter at start point or [Associate to/Equation assistant] <74>:
Press
ENTER
Specify diameter at end point or [Slope/aNgle/Associate to/Equation assistant]
<72>:
Enter 48
NOTE
If the 3D Shaft Generator dialog box hides your shaft, move the dialog
box to another position on the screen.
4
Choose the lower Cylinder icon again, and respond to the prompts as follows:
Specify length or [Associate to/Equation assistant] <7>:
Enter 20
Specify diameter or [Associate to/Equation assistant] <48>:
Enter 40
5
Choose the Slope icon again, and respond to the prompts as follows:
Specify length or [Dialog box/Associate to/Equation assistant] <20>:
Enter 10
Specify diameter at start point or [Associate to/Equation assistant] <40>:
Press
ENTER
Specify diameter at end point or [Slope/aNgle/Associate to/Equation assistant]
<36>:
Enter 32
6
Choose the lower Cylinder icon once more, and respond to the prompts as
follows:
Specify length or [Associate to/Equation assistant] <10>:
Enter 28
Specify diameter or [Associate to/Equation assistant] <32>:
Press
ENTER
You have created a shaft consisting of three cylindrical and two conical seg-
ments. Your drawing should look like this.
Next, you add thread information to the shaft.
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Adding Threads to Shafts
The 3D Shaft Generator dialog box provides the option to add threads to a
shaft. You define the thread information in the Thread dialog box, and the
thread is added to the shaft automatically.
To add threads to a shaft
1
In the 3D Shaft Generator dialog box, select the Outer Contour tab and
choose the Thread icon.
2
The Thread dialog box is displayed. Select ISO 261 from the available thread
types.
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3
The Thread ISO 261 dialog box is displayed. Specify:
Nominal Diameter d [mm]:
M 32 x 1.5
Length
l=:
Enter 12
4
Choose OK.
NOTE
If you have previously chosen a thread standard, the Thread dialog box
opens directly to the Nominal Diameter selection screen (illustrated above).
There is no need to choose the same standard again. To return to the standard
selection list in the Thread dialog box, choose Standard.
Mechanical Desktop Power Pack calculates the thread and adds it to the
shaft, then returns you to the 3D Shaft Generator dialog box.
Following the thread segment, you need to add another cylindrical segment
with a diameter smaller than the threaded section.
5
Choose the lower Cylinder icon, and respond to the prompts as follows:
Specify length or [Associate to/Equation assistant] <28>:
Enter 2
Specify diameter or [Associate to/Equation assistant] <32>:
Enter 25
The new segment is added, and you are ready to add a profile to your shaft.
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Adding Profile Information to Shafts
The 3D Shaft Generator dialog box provides the option to add a profile to a
shaft. You further define the profile information in the Shaft dialog box.
Add a profile segment to connect a drive to the shaft.
To add a profile to a shaft
1
In the 3D Shaft Generator dialog box, choose the Profile icon.
2
In the Profile dialog box, select ISO 14.
3
In the Splined Shaft dialog box, specify:
Nominal Size n x d x D [mm]:
6 x 26 x 30
Length
l=:
Enter 30
Choose OK.
The profile is added to the shaft.
Add another small cylindrical segment to the end of the shaft.
4
In the 3D Shaft Generator dialog box, choose the lower Cylinder icon again,
and respond to the prompts as follows:
Specify length or [Associate to/Equation assistant] <30>:
Enter 5
Specify diameter or [Associate to/Equation assistant] <30>:
Enter 25
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5
Close the 3D Shaft Generator dialog box.
The shaft contour is complete. Your drawing should look like this.
Save your drawing as shaft.dwg.
Next, you edit the shaft.
Editing Shafts
You can make changes to simple shaft segments such as cylinders and cones.
It is recommended that you delete a more complex segment, such as a gear,
and create a new one. In this exercise, you add a chamfer to a segment and
you add a groove to another segment.
First, add a chamfer to the end segment of your shaft.
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To add a chamfer to a shaft segment
1
Activate the shaft generator.
Menu
Content 3D ➤ Shaft Generator
Command
AMSHAFT3D
2
On the command line, respond to the prompts as follows:
Specify start point or [Existing shaft]:
Enter E
Select shaft:
Select the shaft
3
In the 3D Shaft Generator dialog box, select the Outer Contour tab. Choose
the chamfer icon, and respond to the prompts as follows:
Select edge for chamfer:
Select the edge (1)
Specify length (max. 5) or [Associate to/Equation assistant] <2.5>:
Enter 2.5
Specify angle (min 0.0001, max 78.69) [Distance/Associate to/Equation
assistant] <45>:
Enter 45
Enter an option [Revolve/Chamfer] <Revolve>:
Press
ENTER
The chamfer is created on the shaft end.
In the next step, you use the 3D Shaft Generator dialog box to insert a groove
for a retaining ring on a section of the shaft. This groove will be used for posi-
tioning a bearing.
1
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To insert a groove on a shaft segment
1
Choose the Groove icon, and respond to the prompts as follows:
Select cylinder or cone:
Select the third cylindrical section (1)
Select position on cylinder or cone [Line/Plane]:
Specify the point (2)
Specify direction or [Flip/Accept] <Accept>:
Press
ENTER
Enter distance from base plane [Associate to/Equation assistant] <11.4>:
Enter 25
Specify length or [Associate to/Equation assistant] <5>:
Enter 1.5
Specify diameter <50>:
Enter 29
The groove is inserted and displayed on the shaft.
The edits to the shaft are complete.
2
Close the 3D Shaft Generator dialog box.
Save your file.
Now that you have finished the shaft, you add standard parts to it.
1
2
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Adding Standard Parts to Shafts
In Mechanical Desktop Power Pack, standard parts such as bearings, seals,
circlips, keys, adjusting rings, and undercuts are available. You can select and
insert these standard parts using the shaft generator.
When you insert a standard part on a shaft, the standard part is not con-
sumed by the shaft. You are actually building an assembly. An icon for each
new part is displayed in the Browser under the assembly icon.
To add a bearing to a shaft
1
Use
AMSHAFT3D
TO
add a standard part to the shaft.
Menu
Content 3D ➤ Shaft Generator
Command
AMSHAFT3D
2
On the command line, respond to the prompts as follows:
Specify start point or [Existing shaft]:
Enter E
Select shaft:
Select the shaft
3
The 3D Shaft Generator dialog box is displayed. Choose Std. Parts.
4
In the Select a Part dialog box, choose Roller Bearings ➤ Radial ➤ ISO 355.
Respond to the prompts as follows:
Select cylindrical face:
Select a point on the third shaft segment (1)
Specify location on cylindrical face [Line/Plane]:
Select the left plane of the third shaft segment (2)
Enter distance from base plane [Associate to/Equation assistant] <0>:
Press
ENTER
Choose insertion direction [Flip/Accept] <Accept>:
Press
ENTER
1
2
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5
In the ISO 355 dialog box, verify Geometry is selected and specify:
Inner Diameter:
40
Choose Next to continue.
You use the ISO 355 dialog box for the bearing calculation.
6
In the ISO 355 dialog box, verify Calculation is selected and specify the val-
ues as shown below.
By choosing dynamic calculation, Mechanical Desktop is calculating the
adjusted rating life of the bearing.
Choose Next.
The possible bearings are calculated and the results are displayed in the ISO
355 dialog box in Result. Two tabs are provided so you can check both your
input and results.
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7
In the ISO 355 dialog box, select the Result tab, and then select 2BC - 40 x 62
x 15.
Choose Finish.
Use dynamic dragging to size the bearing on the screen.
8
Respond to the prompt as follows:
Drag size [Dialog] <10>:
Drag the bearing, and click when 2BC - 40 x 62 x 15 is displayed in the status bar
The bearing is inserted and your drawing should look like this.
Insert a second bearing, starting from the groove at the left of the fifth
segment of the shaft.
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To add the second bearing
1
In the 3D Shaft Generator dialog box, choose Std. Parts.
2
In the Select a Part dialog box, choose Roller Bearings ➤ Radial ➤ ISO 355.
3
Respond to the prompts as follows:
Select cylindrical face:
Select a point on the fifth shaft segment (1)
Specify location on cylindrical face [Line/Plane]:
Select the right plane of the fifth shaft segment (2)
Enter distance from base plane [Associate to/Equation assistant] <25>:
Press
ENTER
Choose insertion direction [Flip/Accept]:
Enter f
4
Use the default values for the calculation, and select the bearing ISO 355 2BD
- 32 x 52 x 14.
5
Place the bearing by responding to the prompt as follows:
Drag size [Dialog] <10>:
Drag the bearing, and click when 2BC - 32 x 52 x 14 is displayed in the status bar
Close the 3D Shaft Generator dialog box. Your drawing should look like this.
Save your file.
1
2
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Displaying and Shading 3D Views
You can split your screen to display the front and isometric views of the shaft
in separate viewports. You can activate a viewport by clicking inside its
border.
To display front and isometric views in a split screen
1
On the command line, enter 2, and press
ENTER
.
Your drawing area is split to display front and isometric views in separate
viewports.
2
Click a viewport to activate it.
3
Use
AMDT_TOGGLE_SHADWIREF
to add shading to the shaft.
Menu
View ➤ Shade ➤ Gouraud Shaded
4
Activate the second viewport and toggle to shading.
For better visualization, you can change the color properties of a single part,
such as the bearing.
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To change the color of a single part on a shaft
1
In the Desktop Browser, right-click a bearing and choose Properties ➤ Color.
2
Select a different color.
The bearing is displayed in a different color on the shaft. Try changing the
colors of the other parts on the shaft.
Save your file.