Mechanical Desktop 4 Training

Wheels

Aims and Objectives

The aim of this tutorial is to let you practice solid modeling by sketching, revolving, and modifying solid features. After studying this tutorial, you should be able to:

 

Overview

The front and rear wheels of the model car are similar in shape but different in some of the dimensions. You will make one of them, save the drawing in two drawing file, and modify one of the files.

FIG1.gif (6122 bytes)

Figure 1 Front and rear wheels

Analysis

The models are solids of revolution with a central hole. You will construct a sketch, resolve it, and revolve it. Then you will place a hole to complete the model. To make the second solid model, you will save the model in two drawing files and then modify one of them. Figure 2 shows the solid models.

FIG2.gif (7895 bytes)

Figure 2 Solid models

Modeling

Start a new single part drawing.

<File> <New Part>

Use the LAYER command to construct two additional layers, Solid and Wire. Then set layer Wire as the current layer.

<Assist> <Format> <Layer...>

New layers: Solid and Wire
Current layer: Wire
[OK]

Use the LIMITS command to set the drawing limits. Then use the ZOOM command to zoom to extents.

<Assist> <Format> <Drawing Limits>

Command: LIMITS
ON/OFF/<Lower left corner>: 0,0
Upper right corner: 30,20

<View> <Zoom> <All>

<File> <New Part>

Use the PLINE command to construct a polyline. Then use the AMPROFILE command to resolve it to a profile. See Figure 3.

<Design> <Polyline>

<Part> <Sketch Solving> <Profile>

Command: AMPROFILE
Select objects for sketch:
Select objects: ALL
Select objects: [Enter]

fig3.gif (3026 bytes)

Figure 3 Polyline constructed and resolved

Use the AMADDCON command to add geometric constraint. Then use the AMPARDIM command to add four vertical parametric dimensions. See Figure 4.

<Part> <2D Constraints> <Collinear>
Select object to be reoriented: [Select A (Figure 3).]
Select object to be made colinear to: [Select B (Figure 3).]
Select object to be reoriented: [Enter]

<Part> <Dimension> <New Dimension>

Command: AMPARDIM

Select first object: [Select E (Figure 3).]
Select second object or place dimension: [Select C(Figure 3).]
Specify dimension placement: [Select D (Figure 3).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 10
Select first object: [Select F (Figure 3).]
Select second object or place dimension: [Select C (Figure 3).]
Specify dimension placement: [Select D (Figure 3).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 3.5
Select first object: [Select A (Figure 3).]
Select second object or place dimension: [Select C (Figure 3).]
Specify dimension placement: [Select D (Figure 3).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 8.5
Select first object: [Select G (Figure 3).]
Select second object or place dimension: [Select C (Figure 3).]
Specify dimension placement: [Select H (Figure 3).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 5
Select first object: [Enter]

FIG4.gif (3759 bytes)

Figure 4 Vertical dimensions added

Repeat the AMPARDIM command to add five horizontal dimensions. See Figure 5.

<Part> < Dimension> <New Dimension>

Command: AMPARDIM

Select first object: [Select C (Figure 4).]
Select second object or place dimension: [Select B (Figure 4).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 13
Select first object: [Select G (Figure 4).]
Select second object or place dimension: [Select F (Figure 4).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 6
Select first object: [Select D (Figure 4).]
Select second object or place dimension: [Select B (Figure 4).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 3
Select first object: [Select A (Figure 4).]
Select second object or place dimension: [Select B (Figure 4).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 8.5
Select first object: [Select E (Figure 4).]
Select second object or place dimension: [Select F (Figure 4).]
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 14
Select first object: [Enter]

FIG5.gif (3986 bytes)

Figure 5 Profile fully dimensioned

Use the AMREVOLVE command to revolve the profile. Then set the display to an isometric view. See Figure 6.

<Mechanical Main.>
Current : Solid

<Part> <Sketched Features> <Revolve...>

Command: AMREVOLVE
 Select revolution axis: [Select A (Figure 5).]
[Revolution 
Operation: Base
Termination: By Angle
Angle : 360
OK ]

Command: 8

FIG6.gif (3867 bytes)

 

Figure 6 Profile revolved and display set

Use the AMHOLE command to place a hole. See Figure 7.

<Part> <Placed Features> <Hole...>

Command: AMHOLE
[Hole 
Operation: Drilled
Termination: Through
Placement: Concentric
Dia: 3
OK ]
Select work plane or plane face [worldXy/worldYz/worldZx/Ucs]: [Select A (Figure 6).]
Select concentric edge: [Select A (Figure 6).]
Select work plane or plane face [worldXy/worldYz/worldZx/Ucs]: [Enter]

FIG7.gif (3984 bytes)

Figure 7 Hole placed

The rear wheel is complete. Save your drawing.

<File> <Save>
File name: 24Whr.dwg

Use the SAVEAS command to save to a new file.

<File> <Save As...>
File name: 24Whf.dwg

Use the AMEDITFEAT command to edit a sketch. See Figure 8.

<Part> <Edit Feature>

Command: AMEDITFEAT
Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select Feature]: S
Select sketched feature: [Select A (Figure 7).]

FIG8.gif (4165 bytes)

Figure 8 Sketch displayed

Use the ERASE command to delete a dimension. Then use the AMMODDIM command to modify two dimensions. After that, use the AMADDCON command to add a collinear constraint. See Figure 9.

<Modify> <Erase>

Command: ERASE
Select objects: [Select A (Figure 8).]
Select objects: [Enter]

<Part> <Dimensioning> <Edit Dimension >

Command: AMMODDIM
Select dimension to change:  [Select B (Figure 8).]
New value for dimension<6>: 5
Select dimension to change:  [Select C (Figure 8).]
New value for dimension <14>: 8
Select dimension to change: [Select D (Figure 8).]
New value for dimension <3.5>: 4.5
Select dimension to change: [Enter]

<Part> <2D Constraints> <Collinear>

Select object to be reoriented: [Select F (Figure 8).]
Select object to be made colinear to: [Select E (Figure 8).]
Select object to be reoriented: [Enter]
Enter an option [Hor/Ver/Perp/PAr/Tan/CL/CN/Proj/Join/Xvalue/Yvalue/Radius/Length/Mir/Fix/eXit]: [Enter]

FIG9.gif (3294 bytes)

Figure 9 Sketch modified

Use the AMUPDATE command to update the change. See Figure 10.

<Part> <Update Part>

FIG10.gif (3918 bytes)

Figure 10 Solid updated

Use the AMEDITFEAT command to change the size of the hole. Then update the change. See Figure 11.

<Part> <Edit Feature>

Command: AMEDITFEAT
Independent array instance/Sketch/surfCut/Toolbody/<select Feature>: [Select A (Figure 10).]
[Hole 
Dia: 6
OK ]
Select object: [Enter]

<Part> <Update>

FIG11.gif (3694 bytes)

Figure 11 Hole diameter changed, and solid updated

The model is complete. Save your drawing.

<File> <Save>

Key Points

In this tutorial, you constructed a solid of revolution and placed a hole. Then you save the solid in two drawing files. After that, you modified one of the solids.

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