Transcript Inventor Lecture #4

EGR 110 – Inventor Lecture #4
Features in Inventor
Inventor includes two types of
geometric features:
• Sketched features (including
extrusions, revolutions, and
sweeps)
• Placed features (including holes,
fillets, chamfers, and shells)
Sketched features required that 1 or
2 sketches be drawn first. Placed
features do not require a sketch.
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Sketched feature
Placed feature
Placed feature
Sketched feature
Sketched feature
So far we have only used sketched
features (extrusions) to create solid
models.
Placed feature
Sketched feature
The Model browser shows a series
of sequential sketched and placed
features (see example to the right).
Placed feature
Placed feature
EGR 110 – Inventor Lecture #4
Holes
We can create holes using extrusions, but an easier way is to use Hole from the 3D
Model menu.
Example:
Create a simple solid block (extrude a rectangle) and switch to an isometric view.
Select Hole from the 3D Model menu (or press H on the keyboard).
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Holes (continued)
On the Hole menu, select Linear under Placement. Then select three items:
1) Face – Pick the face where you want the hole (pick the approximate location)
2) Reference 1 – Pick an edge for a distance measurement to the center of the hole
3) Reference 2 – Pick another edge for a second distance measurement
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Holes (continued)
Experiment by creating various types of holes, including:
• Through holes
• Holes with a specified depth
• Tapped (threaded) holes
• Countersink holes
• Counterbore holes
• Holes that intersect holes
Also try editing various holes to
change their type, size, location, etc.
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Threads
Note that threads placed inside holes are bit-map images added for appearance only (although the
thread sizes used can be referred to when dimensioning). Threads do not appear on isometrics in
drawing files; however, the threads are properly represented in other views.
Dashed lines
represents threads
EGR 110 – Inventor Lecture #4
External threads – Internal threads are typically added with
the Hole command. External threads can be applied to the
3D model using the Thread command.
Example: Try creating the following object. Discuss
the sequence of operations used as shown in the browser.
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Fillets, Rounds, and Chamfers
Sharp edges on objects are often rounded off using curved edges or beveled edges.
• Fillet - rounded inside corner
• Round – rounded outside corner
• Chamfer – beveled edge connecting two surfaces
Notes:
• Both fillets and rounds are created in Inventor using the Fillet command
• Chamfers and fillets can be added to both 2D sketches and to existing solid features.
Original object with sharp corners:
Round
Fillet
Chamfer
EGR 110 – Inventor Lecture #4
Adding a Fillet to a 2D Sketch
Enter radius
Pick two edges
and fillet (round)
will appear
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Adding a Fillet to a 3D Model
Pick edge
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Example with several fillets and chamfers
• Try building this solid in class. Discuss the series of operations that might be used.
• Which fillets and chamfers could be added to 2D sketches?
• Which should be added later to the 3D model?
Chamfer
Fillet
Chamfer
Round
Fillet
Note: If possible, add chamfers and fillets to a 2D sketch before extrusion. If they are added later to a solid
(as a placed feature), they are often added as late as possible in the sequence of operations so that they do not
interfere with other operations. Note that a machinist creating a part would be likely to add chamfers and
fillets after creating other key features. It is often useful to think of creating parts in Inventor using a
sequence of operations that might be logically used in building the part in a machine shop.
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Revolution
Another type of sketched feature in Inventor is a revolution. Revolutions are useful for
features that are symmetrical about an axis. A revolved feature is formed by revolving a
2D sketch about a specified axis.
Example: Creating a wheel using revolution
2D Sketch: Profile and
axis of revolution
(axis of revolution does not
have to be a centerline)
3D Model: Select Revolve and
the window above appears.
Select the Profile and Axis
Revolved feature
EGR 110 – Inventor Lecture #4
Quick Test
The profile shown could be revolved around lines A, B, C, D, E, or F.
Can you determine which line was used for each solid shown below?
Circle the correct letter in each case.
A
B
C
E
D
F
A B C D E F
A B C D E F
A B C D E F
A B C D E F
A B C D E F
A B C D E F
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EGR 110 – Inventor Lecture #4
Additional Revolution Examples
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EGR 110 – Inventor Lecture #4
Symmetrical Features
Symmetrical Features can be added in Inventor using:
• Circular Pattern
• Rectangular Pattern
• Mirror Pattern
The patterns above can be added to the following:
• 2D Sketch
• 3D Model
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Examples of Rectangular Patterns
• Create the solid box using an extrusion
• Add one countersink hole
• Use rectangular pattern on 3D model
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• Draw box and one circle in 2D Sketch
• Use rectangular pattern on 2D sketch
• Extrude
Quick Test
Would you use a rectangular pattern on the 2D
sketch or on the 3D model? Circle the answer.
Would you use a rectangular pattern on the 2D
sketch or on the 3D model? Circle the answer.
EGR 110 – Inventor Lecture #4
Examples of Circular Patterns
• Create circular plate using an extrusion
• Add one stud with a second extrusion
• Use circular pattern on 3D model
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• Draw 2D Sketch with one circle
• Use circular pattern on 2D sketch
• Extrude
Useful note: If you try to perform operations (such as trim or fillet) on
a pattern, you may find that it will not work. To correct this problem:
1) Select Edit Pattern (box appears such as the one below)
2) Select the More button (>>)
3) Remove the check from Associative
More
More complex example
Remove Check
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Example of Mirror Pattern
Mirror
Line
1. Draw half of object. Include mirror
line (construction line may be useful)
3. Extrude to create
solid model
2. Select sketch features to
mirror and the mirror line
EGR 110 – Inventor Lecture #4
Detailed Example: Rectangular Pattern in a 2D Sketch
1) Draw sketch, including one hexagon (use Polygon tool)
2) Select Rectangular pattern, select Geometry, and select the hexagon
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Detailed Example: Rectangular Pattern in a 2D Sketch (continued)
3) Select Direction 1 and pick a line in the direction the pattern should go (a
horizontal line in this case). An arrow appears showing the direction selected. If
the arrow is in the opposite direction, select the Flip button.
4) Enter the number of pattern elements and spacing for Direction 1
Direction arrow and Flip
button
Number of elements
Spacing between elements
Arrow appears in the
direction selected
for Direction 1
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Detailed Example: Rectangular Pattern in a 2D Sketch (continued)
5) Select Direction 2 and pick a line in the second direction the pattern should go
(vertical line). An arrow appears showing the direction selected. If the arrow is in
the opposite direction, select the Flip button.
6) Enter the number of pattern elements and spacing for Direction 2
Arrow appears in the
direction selected
for Direction 1
Final result
after extrusion
EGR 110 – Inventor Lecture #4
Detailed Example: Circular Pattern in a 3D Model
Create a wheel with 6 equally space threaded holes shown below.
1. Create the basic wheel using a revolution
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Detailed Example: Circular Pattern in a 3D Model (continued)
2. Add another sketch plane to the face of the wheel where the holes will be added.
• Add a line and a dimension for the bolt circle – the circular path on which the
holes will lie.
• Finish the sketch.
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Detailed Example: Circular Pattern in a 3D Model (continued)
3. Select Hole from the 3D Model menu. Use the following options:
• Placement: From Sketch
• Pick the center point where the hole is to be placed
• Termination: Through All
• Diameter: 0.75 in (or your choice)
• Select Threaded Hole and then select OK
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Detailed Example: Circular Pattern in a 3D Model (continued)
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4. Select Circular Pattern from the 3D Model menu. Use the following options:
• Features: Select the threaded hole just created
• Rotational Axis: Pick any circle on the wheel that has the correct center
• Placement: Pick 6 holes spread over 360 degrees
• Select OK
Final result
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Centerlines and Linear Diametric Dimensions
For revolved features it is common to use linear diametric dimensions instead of
radial dimensions. An example of the difference is shown below.
f25
f25
f15
f5
f15
f5
Front
Example using
radial dimensions
Right
Front
Example using
linear diametric dimensions
EGR 110 – Inventor Lecture #4
Revolved Features with Linear Diametric Dimensions
An example is shown below to illustrate the procedure for creating a revolved feature
using a centerline and linear diametric dimensions.
1.
Create a new (metric) part and draw the profile to be revolved.
Use a centerline for the axis of revolution (required).
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Revolved Features with Linear Diametric Dimensions (continued)
2.
3.
Add dimensions by selecting:
a) The centerline (not its endpoint)
b) A line on the profile
Finish the sketch and revolve the sketch
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Revolved Features with Diametric Dimensions (continued)
4. Create a metric drawing file using the part (ANSI(mm).idw with A-size, portrait).
• Add front, top, and isometric views. Change the scale if necessary.
• Retrieve dimensions for the front view – note that they are linear diametric dimensions
• Change the number of digits to whole mm using:
Manage – Styles Editor – Dimension – Default: mm (ANSI) – Precision - 0
Linear diametric dimensions