Autodesk Inventor® Part Modeling: The First Step (Part 1)

11/28/2006 - 10:30 am - 12:00 pm Room:Marcello - 4503 (MSD Campus)
Autodesk Inventor® Part Modeling: The First Step [Part 1]

Anthony Dudek - BP
and Thomas Short
MA11-5 Lofts, tangents and bores! Oh my! No need to fear Inventor Part Modeling. We’ll show you everything
you need to know to be the hero back in the office. This class will demonstrate most of the sketch tools
and part features in Autodesk Inventor® and show logical techniques and guiding principles that can
help you create accurate and healthy parametric parts that will behave themselves in your assemblies.
Proper sketch and part modeling is the foundation for Inventor assemblies and capturing the proper
design intent.
About the Speaker:

One of Tony's main ideas overarching his 20-year-long career in engineering is that designing in 3D is
a smarter and faster way to work. His philosophy is "Whatever it takes, do it right the first time." Tools
like Autodesk Inventor can help achieve that goal. He believes that the engineering landscape in
America has changed from an internal, ownership environment to an overextended and outsourced
managed environment. Within this context, we are challenged to continue to deliver more quality in
less time. This is the challenge of our generation of technology workers. The future is very promising
with new technologies and methods being implemented every day. This will be Tony's 12th year at
Autodesk University.
dudea1@bp.com
Stay Connect to AU all year at www.autodesk.com/AUOnline

MA11-5 Autodesk Inventor® Part Modeling: The First Step [Part 1]
Objectives
Take a good look at the powerful tools available to assist you in designing incredible parts in
Autodesk Inventor.
Gain more Inventor power from these techniques to make you famous!
Acquire a better understanding of parametric design methodology inside the latest release of
Autodesk Inventor.
Outline
10:30 – 10:45 15 min. Introductions – Class Objectives
10:45 – 11:15 30 min. Sketching and Control
11:00 – 11:50 50 min. Effective Part Modeling
11:50 – 12:00 10 min. Summary - Question & Answer
On Sketches, Geometric Constraints, Dimensional Constraints, etc.
Try to use geometric constraints wherever possible. They are tough little guys doing ten times
work for their body size. Not very noticeable, doing their work behind the scenes, but they bring
an unruly profile into line (no pun intended).
Sketch your profile to roughly the final size. Drawing a rectangle 12 X 6 when you really want to
end up with a 2 X 1 final size doesn’t make sense and you’re asking for trouble. The rectangle
example is an oversimplification, but you get the idea. Later on, as your skills improve you can use
Shared Sketches and what I call “Controlling” Sketches.
Use “smart” equations for your dimensional values, not just dumb numeric values. Equations help
to tie dimensions together so that if one changes perhaps they all do! The ideal is to have all your
part’s features tied to one or two key dimensions. Change one of those key dimensions and the
part significantly changes. Most part designs evolve around a few key dimensions – the bore ID of
a cylinder, the mounting holes on a bracket, etc.
Any sketch profile must survive the acid test first before it can be turned into a 3D feature. Any
dimension on your profile should be able stand a reasonable dimension value change without the
entire sketch profile distorting out of shape. A dimension change should produce the change you
expected, if not then the sketch profile is not considered “logically” constrained; even though
Inventor may have reported it as “fully” constrained.
What happens if you, like the rest of us, lose track of how many dimensions/constraints are still
needed to fully constrain the profile? Use the Auto-dimension tool and it will report how many more
dimensions and/or constraints left to go.
Use construction geometry! Use construction geometry! Please! This very powerful, yet under
utilized, technique is often you’re only chance to fully constrain a profile. Use construction
geometry. Although invisible when the profile is extruded, construction geometry is behind the
scenes doing its job. Construction geometry not only has its uses in sketch profiles, but also in
assemblies.
The Sketch Doctor isn’t always right! Many of you have probably ran into the infuriating Catch-22
type situation wherein the Sketch Doctor says that a sketch is missing coincident constraints at
some vertices. However, at the same time he is also reporting that those same vertices have
redundant coincident constraints! My best advice – ignore him in this situation.
2
Inventor Features Tutorial

We’re going to do a tutorial to demonstrate some
of Inventor’s Part Modeling capabilities. No
dataset parts are required – this will start from a
new Part.
Start a new Part. There should be a Sketch
already created and opened for edit.
On the Sketch Project the X axis and the Y axis

from the Origin folder. This is an industry-
accepted practice, although some only Project
the Center Point.
Draw a rectangle and dimension it so that it is

centered using the projected axis lines. Make the
dimensions parametrically defined so as to center the rectangle on the Origin. Example: D0/2
F6 to change the display to Isometric
Add .50 fillets to the sketch at each corner.
Hit E on the keyboard – Extrude. Specify an

extrusion height of .50”
Expand the Origin folder in the Browser and in
turn left-click on each of the Origin Workplanes.
Notice how they bisect the Base feature evenly in
all three dimensions.
Start a secondary sketch on top of the Base feature.
Project the Center Point from the Origin folder.
Draw a Circle centered on the projected Center

Point.
Dimension its diameter - tie it parametrically to the

vertical half-dimension using Show Dimensions. It is
not necessary to locate it dimensionally. Do you
understand why?
Type E on the keyboard for Extrude. There is the

possibility of two Sketches and so Inventor needs
you to specify which - the area inside the circle or
outside of it.
3
At this point it may be beneficial to the student to understand the three possible Boolean
operations that are available. They weren’t available before with the first Sketch because there was
no solid geometry to interact with. They are Join, Cut & Intersect – graphically shown down the
center of the dialog box. We will be adding material in the shape of a cylindrical Boss feature so we
will use Join. Cut would be used if you were to extrude the circle down into the Base to produce a
void or a hole. Intersect would create a solid based on the common volume of the two features –
the Base and the extruded cylinder. Try to imagine
what that would look like.
To continue, choose Join and specify a height of 2.00”
for the
cylindrical Boss.
Create another Sketch on top of the cylindrical Boss

feature merely to create a Hole Center Point. At times
this is not necessary – Inventor let’s you drill holes at
any point in a Sketch. We don’t have that situation
here though.
Using the Hole tool drill a tapped Hole using ¾-12 UN

for the Pitch, Major for the Diameter, 2B for the Class
of fit.
The Hole tool requires that you position “Point, Hole Center”
points on a sketch plane on the part or a work plane and
then use the “Hole” tool on the Feature menu to specify the
size and type. All the holes in one sequence have the same
sizes and characteristics. The advantages of using holes over
extruded circles are:
The holes can be drilled, counterbored or countersunk.
Thread sizes and specifications can be easily applied.
Threads will be displayed in the shaded image.
Threaded holes will display correctly in the part drawings.
“Hole Notes” can be automatically applied to the part
drawings.
“Hole Tables” can be created in the part drawings.
There is a Thread tool also. This is meant for internal / external
threads on extruded cylinders that were not created with the Hole
tool.
Using the Chamfer tool put a .06” Chamfer on the opening edge of
the tapped Hole.
Using the Color Style droplist on the right-hand side of the Standard
toolbar change to Metal Brass or Beige Light.
4
Select the YZ Plane of the Origin folder

in the Browser and key ‘S’ on the
keyboard. The F7 function key will slice
the part visually with the Sketch Plane.
Successive use of the F7 key simply
toggles the effect on and off. F4 Rotate
the screen to look at the other side of
the Part and use F7 again. Notice that
the visual slice is viewpoint dependent.
Select the Sketch in the Browser and hit
Page Up on the keyboard to get a plan
display of the Sketch. Project the top
edge of the Base (left side). Draw a line
from touching the projected geometry
and up and to the right. Dimension it from the edge
(.01875”) and at a 60 deg. angle. Not necessary to
fully constrain it. (refer to Figure)
Use the Rib tool to create a Rib feature. Use the

midplane option and make it (.125”) thick. Use the
Direction button to specify that the Rib should extrude
down towards the body of the Part. A visual cue will
help you. It should not be necessary to Extend the Rib
feature so that it meets the solid geometry of the Part
– Inventor will assume that.
Select the Rib feature in the Browser by left-clicking on
it. Choose the Circular Pattern tool from the
Tool Panel and specify the cylindrical Boss
feature as the axis for the Pattern. Choose a
count of 4 for the Ribs and an angle of 360 to
fill with the Pattern. Expand the << button
and examine the Methods. The Creation
Method dictates whether the members of the
Pattern will all be alike or will adjust to
conform to the Part’s perhaps changing
geometry. The Positioning Method determines
whether the angle value (360 in our example)
is used to Fit all the members in it (yes in our
example) or whether the value will be used to
specify angular spacing between members.
Locate the Base feature in the Browser and
Edit the sketch so that the Base feature is 3”
square. Notice the changes.
Create a sketch on the top face of the Boss.

Notice that the edges and the hole centers are automagically projected. This is a setting and is
controlled by the Tools -> Application Options -> Sketch dialog box settings. Use the Hole tool to
create four counterbored holes at the hole center points. Take note that this creates (4) holes, but
only one Feature in the Browser – maybe this is good, maybe not. It all depends on your design
intent.
5
Take a moment and
examine what’s been
done. Now’s a good time
to rename the Features in
the Browser.
Now it’s time for the coup

de grace. Usually the last
operation is the
application of Fillets. Refer
to the figure as you do
this. You need only use
the Fillet tool once and
create one Fillet Feature in
the Browser.
The best way to do this is

to use the Loop selection
to pick the bottom of the
cylindrical Boss and the
top face’s edge of the
Base, then use the
Feature selection to pick
the Rib Feature as a whole
and then the Pattern Feature. Choose OK and you should have it done. Oila!
We are now going to Engrave some text on our part as if we were stamping a part number on it.
On the left-front side of the Base feature left-click on the face. Press ‘S’ on the keyboard and you
will be in Edit Sketch mode. Draw a construction line from the midpoint (green dot) of the left
vertical line to the midpoint of the right vertical line. Draw another construction line from the
midpoint of the top horizontal line to the midpoint of the bottom horizontal line. These will be used
to center the Engraving text in the center of the face. Pick the Create Text tool from the 2D Sketch
Panel and pick a point anywhere in the face. In the dialog box type in “PART NO. AU2004” and
choose horizontal and vertical justification from the buttons along the top of the dialog box. Pick
OK to exit the dialog box. You’ll notice a frame around the text. You’ll dimension to this frame to
control the size of the text string.
Use a value of 1.50 for the length
and .125 for the text height. The
location of the text string will be
geometrically constrained by using
Coincident constraints between the
horizontal and vertical midpoints of
the text frame and the horizontal
and vertical construction lines
created earlier. Select the Auto
Dimension tool to ensure that
you’ve eliminated all of the
constraints needed. Pick Return to
exit out of Edit Sketch mode. Select
the Emboss tool from the Tool
Panel. The same tool is used for
Engraving (sunken letters) and Embossing (raised letters). The Profile will need to be specified
carefully. You do not want to select the large face – only the text letters themselves. Refer to the
6
Figure using a value of .05 for the depth of the letters and the other selections necessary –
Engrave and direction.
The Emboss Feature should be in the Browser – right-click on it and choose Properties from the
context menu. Change the Feature Color Style to Metal-Silver as shown in the Figure to the right.
In Closing
I hope that everyone agrees that effective Part Modeling is something that can be learned and
applied to make your part designs smarter and more efficient. It has been shown that Autodesk
Inventor is packed with the tools and features that are required to produce today’s complex parts
in today’s complex world. I hope that you now have the knowledge you need to go back to the
office and design it better, faster and cheaper.
I sincerely thank you for your time and attention,

Anthony Dudek
Anthony.Dudek@bp.com
Thomas Short, P.E.
notietom@cs.com
Portions reprinted from “Learning Inventor 10” published by Goodheart-Willcox publishers.

Autodesk Inventor® Part Modeling: The First Step (Part 1)

Uploaded by

Copyright:

Available Formats

Autodesk Inventor® Part Modeling: The First Step (Part 1)

Uploaded by

Document Information

Original Title

Copyright

Available Formats

Share this document

Share or Embed Document

Sharing Options

Did you find this document useful?

Is this content inappropriate?

Copyright:

Available Formats

Autodesk Inventor® Part Modeling: The First Step (Part 1)

Uploaded by

Copyright:

Available Formats

11/28/2006 - 10:30 am - 12:00 pm Room:Marcello - 4503 (MSD Campus)

Autodesk Inventor® Part Modeling: The First Step [Part 1]

About the Speaker:

Stay Connect to AU all year at www.autodesk.com/AUOnline

Inventor Features Tutorial

On the Sketch Project the X axis and the Y axis

Draw a rectangle and dimension it so that it is

F6 to change the display to Isometric

Add .50 fillets to the sketch at each corner.

Hit E on the keyboard – Extrude. Specify an

Start a secondary sketch on top of the Base feature.

Project the Center Point from the Origin folder.

Draw a Circle centered on the projected Center

Dimension its diameter - tie it parametrically to the

Type E on the keyboard for Extrude. There is the

Create another Sketch on top of the cylindrical Boss

Using the Hole tool drill a tapped Hole using ¾-12 UN

Select the YZ Plane of the Origin folder

Use the Rib tool to create a Rib feature. Use the

Create a sketch on the top face of the Boss.

Now it’s time for the coup

The best way to do this is

I sincerely thank you for your time and attention,

You might also like