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:
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. To add a hole, you specify the size and location. Figure 1 shows the rendered image of the front axle of a 24th scale model car.
Analysis
Figure 2 shows the solid model of the front axle of a 24th car model car. This model has two features, a revolve solid and a threaded hole. To make the revolve solid, you make a sketch, resolve it to a profile, fully constrain it, and revolve the profile. To make the threaded hole, you specify the parameters and location.
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> <Zoomt> <All>
Use the PLINE command to construct a polyline. See Figure 3.
<Design> <Polyline>
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: [Select A (Figure 3).]
Select objects: [Enter]
<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> <Dimensioning> <New Dimension>
Command: AMPARDIM
Select first object:[Select D (Figure 3).]
Select second object or place dimension: [Select F (Figure 3).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 16
Select first object: [Select B (Figure 3).]
Select second object or place dimension:[Select E (Figure 3).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 9
Select first object: [Select A (Figure 3).]
Select second object or place dimension: [Select E (Figure 3).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 6
Select first object: [Select B (Figure 3).]
Select second object or place dimension: [Select D (Figure 3).]
Specify dimension placement: [Select G (Figure 3).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 1.5
Select first object: [Select C(Figure 3).]
Select second object or place dimension:[Select D (Figure 3).]
Specify dimension placement:[Select H (Figure 3).]
Enter dimension value [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]: 2
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> <Revolve...>
Command: AMREVOLVE
Select revolution axis: [Select A (Figure 4).]
[Revolution
Operation: Base
Termination: By Angle
Angle: 360
OK ]
Use the AMHOLE command to place a tapped hole. See Figure 6. Note that the thread only displays in drawing mode but not model mode.
<Part> <Placed Features> <Hole...>
Command: AMHOLE
[Hole
Operation: Drilled
Termination: Blind
Placement: Concentric
Tapped Ö
Major Dia: 2
Full Depth : off
Depth: 4
OK ]
Drill Size:
Dia: 1.7
Depth: 6
PT Angle: 118
OK ]
Select work plane or planar face [worldXy/worldYz/worldZx/Ucs] : [Select A (Figure 5).]
Select concentric edge: [Select A (Figure 5).]
Select work plane or planar face [worldXy/worldYz/worldZx/Ucs] : [Enter]
The model is complete. Save your drawing.
<File> <Save>
File name: 24axf.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.