Aims and Objectives

The aim of this tutorial is to let you practice solid modeling by sketching, resolving a sketch, constraining a profile, revolving a profile to a solid, and place tapped hole. After studying this tutorial, you should be able to:

• construct a sketch,
• resolve a sketch,
• apply geometric constraints to a profile,
• add parametric dimensions to a profile,
• revolve a profile to a solid, and
• place tapped hole feature.

Basically, a solid is derived from a rough sketch. Prior using the sketch for making a solid, you have to fully constrain it by adding geometric constraints and parametric dimensions. To make a revolve solid, you can revolve a fully constrained profile. 

Modeling

Start a new single part drawing.

<File> <New Part File>
[ Enter]

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

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: 20,10

<View> <Zoom> <All>

Use the PLINE command to construct a polyline. See Figure 3.

<Design> <Polyline> 

Figure 3 Polyline constructed

<Modify> <Mirror>
Command: MIRROR
Select objects: ALL
Select objects: [Enter]
Specify first point of mirror line: [Select A (Figure 3)]
Specify second point of mirror line: @1,0
Delete source objects ? [Yes/No]: [Enter]

Use the AMPROFILE command to resolve the sketch to a profile. Then use the AMADDCON command to add geometric constraints. After that, use the AMPARDIM command to place parametric dimensions. See Figure 4.

<Part> <Sketch Solving> <Profile>

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

<Part> <2D Constraints> <Collinear>

Select object to be reoriented: [Select A (Figure 4).]
Select object to be made colinear to: [Select E (Figure 4).]
Select object to be reoriented: [Select C (Figure 4)]
Select object to be made colinear to: [Select G (Figure 4).]
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]

<Part> <2D Constraints> <Equal Length>

Select object to be resized: [Select A (Figure 4).]
Select object to based sized on: [Select E (Figure 4).]
Select object to be resized: [Select C (Figure 4).]
Select object to based sized on: [Select G (Figure 4).]
Select object to be resized: [Select B (Figure 4).]
Select object to based sized on: [Select F (Figure 4).]
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]

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select C (Figure 4).]
Select second object or place dimension: [Select K (Figure 4).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 8.4
Select first object: [Select A (Figure 4).]
Select second object or place dimension:[Select I (Figure 4).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 11.5
Select first object: [Select B (Figure 4).]
Select second object or place dimension: [Select L (Figure 4).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 16.8
Select first object: [Select D (Figure 4).]
Select second object or place dimension: [Select J (Figure 4).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 18
Select first object: [Select A(Figure 4).]
Select second object or place dimension:[Select E (Figure 4).]
Specify dimension placement:[Select M (Figure 4).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 24.4
Select first object: [Enter] 

Set the display to an isometric view. Then use the AMREVOLVE command to revolve the profile to a solid. See Figure 5.

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

Current layer: Solid

Command: 8

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Base
Termination: Blind
Distance: 5
Draft Angle: 0
OK ]
Direction Flip/<Accept>: [Enter]

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select A (Figure 6)]
Enter an option [Next /Accept] <Accept>  : [Enter] [If face AB is highlighted]
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

Command: 9

<Design> <Polyline> 

<Part> <Sketch Solving> <Profile>

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

<Part> <2D Constraints> <Collinear>

Select object to be reoriented: [Select B (Figure 7.]
Select object to be made colinear to: [Select A (Figure 7).]
Select object to be reoriented: [Select C (Figure 7)]
Select object to be made colinear to: [Select D (Figure 7).]
Select object to be reoriented: [Select E (Figure 7)]
Select object to be made colinear to: [Select F (Figure 7).]
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]

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select E (Figure 7).]
Select second object or place dimension: [Select G (Figure 7).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 2
Select first object: [Select I (Figure 7).]
Select second object or place dimension:[Select G (Figure 7).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 2
Select first object: [Select I (Figure 7).]
Select second object or place dimension: [Select J (Figure 7).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 1.5
Select first object: [Select H (Figure 7).]
Select second object or place dimension: [Select K (Figure 7).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 1
Select first object: [Select B(Figure 7).]
Select second object or place dimension:[Select H (Figure 7).]
Specify dimension placement:[Select G (Figure 7).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: N
Enter dimension value : 100
Select first object: [Enter] 

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Intersection
Termination: Through
Draft Angle: 0
OK ]

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select A (Figure 6)]
Enter an option [Next /Accept] <Accept>  : [Enter] [If face AB is highlighted]
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

Command: 5

<Design> <Polyline> 

<Part> <2D Constraints> <Collinear>

Select object to be reoriented: [Select A (Figure 9).]
Select object to be made colinear to: [Select B (Figure 9).]
Select object to be reoriented: [Select H (Figure 9)]
Select object to be made colinear to: [Select F (Figure 9).]
Select object to be reoriented: [Select H (Figure 9)]
Select object to be made colinear to: [Select I (Figure 9).]
Select object to be reoriented: [Select L (Figure 9)]
Select object to be made colinear to: [Select E (Figure 9).]
Select object to be reoriented: [Select N (Figure 9)]
Select object to be made colinear to: [Select O (Figure 9).]
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]

<Part> <2D Constraints> <Equal Length>

Select object to be resized: [Select H (Figure 9).]
Select object to based sized on: [Select F (Figure 9).]
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]

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select A (Figure 9).]
Select second object or place dimension: [Select G (Figure 9).]
Select place dimension: [Select M (Figure 9).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 13.6
Select first object:[Select J (Figure 9).]
Select second object or place dimension: [Select K (Figure 9).]
Select place dimension: [Select P (Figure 9).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 2
Select first object: [Enter] 

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Join
Distance: 1.8
Draft Angle: 0
Termination: Blind
OK ]

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select A (Figure 6)]
Enter an option [Next /Accept] <Accept>  : [Enter] [If face AB is highlighted]
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

<Design> <Circle> <Center, Radius>

<Part> <Sketch Solving> <Profile>
Command: AMPROFILE
Select objects for sketch:
Select objects: ALL
Select objects: [Enter]

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select A (Figure 11).]
Select second object or place dimension: [Select B (Figure 11).]
Select place dimension: [Select C (Figure 11).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 4.2
Select first object:[Select A (Figure 11).]
Select second object or place dimension: [Select B (Figure 11).]
Select place dimension: [Select D (Figure 11).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 0.01
Select first object:[Select A (Figure 11).]
Select second object or place dimension: [Select C (Figure 11).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 8
Select first object: [Enter] 

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Join
Distance: 10
[Flip (if arrow is point 
Draft Angle: 0
Termination: Blind
OK ]

<View> <3D Views> <Back Left Isometric>

Figure 12 

Command: 9

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select A (Figure 12)]
Enter an option [Next /Accept] <Accept>  : [Enter] [If face AB is highlighted]
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

<Design> <Circle> <Center, Radius>

<Part> <Sketch Solving> <Profile>
Command: AMPROFILE
Select objects for sketch:
Select objects: ALL
Select objects: [Enter]

Figure 13 

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select A (Figure 13).]
Select second object or place dimension: [Select B (Figure 13).]
Select place dimension: [Select C (Figure 13).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 1
Select first object:[Select A (Figure 13).]
Select second object or place dimension: [Select B (Figure 13).]
Select place dimension: [Select D (Figure 13).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 8
Select first object:[Select A (Figure 13).]
Select second object or place dimension: [Select C (Figure 13).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 8
Select first object: [Enter] 

Figure 13A 

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Join
Distance: 3
[Flip, if Arrow is point toward -X axis]
Draft Angle: 0
Termination: Blind
OK ]

Figure 14 

<View> <3D Views> <Front Left Isometric>

Figure 15 

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select A (Figure 11)]
Enter an option [Next /Accept] <Accept>  : [Enter] [If face AB is highlighted]
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

<Design> <Circle> <Center, Radius>

<Part> <Sketch Solving> <Profile>
Command: AMPROFILE
Select objects for sketch:
Select objects: ALL
Select objects: [Enter]

Figure 16 

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select B (Figure 16).]
Select second object or place dimension: [Select A (Figure 16).]
Select place dimension: [Select C (Figure 16).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 8
Select first object:[Select B (Figure 16).]
Select second object or place dimension: [Select A (Figure 16).]
Select place dimension: [Select D (Figure 16).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 2.8
Select first object:[Select B (Figure 16).]
Select second object or place dimension: [Select C (Figure 16).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 14.4
Select first object: [Enter] 

Figure 16A

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Join
Distance: 10.4
[Flip, if Arrow is point toward +z axis]
Draft Angle: 0
Termination: Blind
OK ]

Figure 17

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select A (Figure 17)]
Enter an option [Next /Accept] <Accept>  : [Enter] [If face AB is highlighted]
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

<Design> <Rectangle>

Specify first corner point : END of [Select A (Figure 17)]
Specify other corner point : END of [Select B (Figure 17)]

<Part> <Sketch Solving> <Profile>
Command: AMPROFILE
Select objects for sketch:
Select objects: ALL
Select objects: [Enter]

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Cut
Draft Angle: 0
Termination: Through
OK ]

Figure 18 

<Part> <Placed Features> <Fillet...>

Command: AMFILLET
[Constant]
Radius: 2
[OK]

Select edges or faces to fillet: [Select A (Figure 18)]

<Part> <Placed Features> <Shell...>

Command: AMSHELL
Default Thickness
[Inside]
Radius: 1

Excluded Faces
[Add]
Select faces to exclude : [Select B (Figure 18)] 
Enter an option [Next/Accept] :  [Enter , if Face BC is highlight]
Select faces to exclude : [Enter]
[OK]

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select A (Figure 18)]
Enter an option [Next /Accept] <Accept>  : [Enter] [If face AB is highlighted]
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

Command: 6

<Design> <Polyline>

Figure 19 

<Part> <Sketch Solving> <Profile>
Command: AMPROFILE
Select objects for sketch:
Select objects: ALL
Select objects: [Enter]

<Part> <2D Constraints> <Collinear>

Select object to be reoriented: [Select D (Figure 19).]
Select object to be made colinear to: [Select B (Figure 19).]
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]

<Part> <2D Constraints> <Equal Length>

Select object to be resized: [Select D (Figure 19).]
Select object to based sized on: [Select B (Figure 19).]
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]

<Part> <2D Constraints> <Concentric>

Select object to be reoriented:  [Select A (Figure 19).]
Select object to be made concentric to: [Select C (Figure 19).]
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]

<Part> <2D Constraints> <Vertical>

Select object to be resized: [Select A (Figure 19).]
Select object to based sized on: [Select C (Figure 19).]
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]

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select A (Figure 19).]
Select second object or place dimension: [Select E (Figure 19).]
Enter dimension value [Undo/Diameter/Orinate/Placement point] : 4.5
Select first object:[Select C (Figure 19).]
Select second object or place dimension: [Select E (Figure 19).]
Enter dimension value [Undo/Diameter/Orinate/Placement point] : 3
Select first object:[Select A (Figure 19).]
Select second object or place dimension: [Select F (Figure 19).]
Select place dimension: [Select G (Figure 19).]
Enter dimension value [Undo/Diameter/Orinate/Placement point] : 8
Select first object:[Select A (Figure 19).]
Select second object or place dimension: [Select F (Figure 19).]
Select place dimension: [Select G (Figure 19).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] : V
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] : 1
Select first object: [Enter] 

Command: 8

Figure 19A 

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Join
Distance: 1.5
Draft Angle: 0
Termination: Through
OK ]

Figure 20 

<Part> <New Sketch Plane>
Select work plane, planar face or [worldXy/ worldYz/ worldZx/Ucs] : [Select B (Figure 20)]
Enter an option [Next /Accept] <Accept>  : [Enter] 
Select edge to align X axis or [Z-flip/Rotate] : [Enter]

<Part> <Copy Feature>

Command: AMCOPYFEAT
Select feature to be copied (from any part):  [Select A (Figure 20)]
Specify location on the active part or [Parameters]: [Select B (Figure 20)]
Specify location on the active part or [Parameters/Rotate/Flip]]: F
Specify location on the active part or [Parameters/Rotate/Flip]]: [Enter]

Command: 8

[Select copied feature in Desktop Browser>
[Right button of your mouse]
[Edit Sketch]

Figure 21 

<Part> <2D Constraints> <Concentric>

Select object to be reoriented:  [Select A (Figure 21).]
Select object to be made concentric to: [Select B (Figure 21).]
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]

<Part> <Update Part>

Command: 8

<Part> <Work Feature> <Work Plane>
1 st  Modifier 
[Plane Parallel]
2 nd Modifier
[Offset]
Offset : 7.5
[Create Sketch Plane]

Select work plane, planar face or [WorldXy/WorldYz/worldZx/Ucs]:  X
Enter an option [ Flip/Accept] :  F
Enter an option [ Flip/Accept] :  [Enter]
Select edge to align X axis or [Z-flip/Rotate] :  [Enter]

Command: 9

<Design> <Circle> <Center, Radius>

 
Figure 22 

<Part> <Sketch Solving> <Profile>
Command: AMPROFILE
Select objects for sketch:
Select objects: ALL
Select objects: [Enter]

<Part> <2D Constraints> <Radius>

Select object to be resized:  [Select A (Figure 22).]
Select object radius is based on: [Select C (Figure 22).]
Select object to be resized:[Enter]
Enter an option [Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix/eXit] : [Enter]

<Part> <Dimensioning> <New Dimension>

Command: AMPARDIM
Select first object:[Select A (Figure 22).]
Select second object or place dimension: [Select C (Figure 22).]
Select place dimension: [Select E (Figure 22).]
Enter dimension value [Undo/Diameter/Orinate/Placement point] : 2.8
Select first object:[Select A (Figure 22).]
Select second object or place dimension: [Select C (Figure 22).]
Select place dimension: [Select D (Figure 22).]
Enter dimension value [Undo/Diameter/Orinate/Placement point] : 2.2
Select first object:[Select A (Figure 22).]
Select second object or place dimension: [Select E (Figure 22).]
Select place dimension: 2
Select first object:[Select A (Figure 22).]
Select second object or place dimension: [Select B (Figure 22).]
Select place dimension: [Select E (Figure 22).]
Enter dimension value [Undo/Diameter/Orinate/Placement point] : 31.6
Select first object:[Select A (Figure 22.]
Select second object or place dimension: [Select B (Figure 22).]
Select place dimension: [Select D (Figure 22).]
Enter dimension value [Undo/Diameter/Orinate/Placement point] : 13.6
Select first object: [Enter] 

Figure 23 

<Part> <Sketched Features> <Extrude...>

Command: AMEXTRUDE
[Extrusion Feature
Operation: Join
Termination: Blind
Distance: 8.9
Draft Angle: 0

OK ]

Figure 24 

The model is complete. Save your drawing.

<File> <Save>

File name: fcover.dwg

Key Points

In this tutorial, you constructed a sketch, resolved it to a profile, revolved the profile to a solid, and placed a tapped hole.