Inventor Tutorial #2: Assemblies and Labeling Parts
This week, we will review how to use individual parts to create an assembly. The process itself is
not very difficult, but if it is not done properly, it can cause quite a headache. This quarter, since
we may be using the animation option within Inventor itself, it is especially important that
students are comfortable with assemblies.
Here are the main points you should probably note and go through with students:
• To open an assembly, open a “Standard.iam” file
• You can insert parts into your assembly in two ways:
o In the “Assembly Panel”, choose “Place Component” and find your part click to
place one – right click and choose done when you have placed enough (Insert the
base plate from Assignment 1)
o In the “ “ menu, create your the component within the assembly file – it will save
this part as a new “.ipt” file for you by default
• The first part you insert will be by default “Grounded”
o If you look at the part on the “Model Toolbar”, you will see a pushpin next to this
object
o A “Grounded” object will not move –constrained objects will move with respect
to this one
o You can remove the “Grounded” property by right clicking on the part and
unselecting the grounded option (you should have one object grounded at any
given time)
• It is recommended to place components and constrain them one at a time (Insert bearing)
• There are three general categories of constraints – we are only really concerned with:
o Assembly – basic constraint used to constrain objects to proper orientation with
respect to one another by using surfaces, edges, planes, points and axes.
o Motion – used for components such as meshing gears or rack and pinions
• Within the Assembly constraints tab, there are 4 types of constraints
o Mate
Used to orient chosen FLAT faces of objects in desired way
Explain (maybe show) the difference between mate, flush and angle
Mate the bottom of the bearing to the top of the base plate and look at the
side of the base plate to show what constraint did
o Tangent
Used to orient ROUND face with FLAT or ROUND face
Suppress previous constraint and show how rounded face of bearing can
be constrained to be tangent to flat surface of base plate
Undo previous step
o Insert
Used to insert a ROUND object into another ROUND object
We’ll come back to this one
o Concentric
Used to make the center axis of two circular parts the same
Make the center axis of one of the side holes of the bearing the same as the
ones of the side holes of the base plate Show that you can rotate the objects using the “Rotate component”
command even if it is constrained – it will automatically snap back when
you are done
Do the same with the hole on the other side
• Place the collar in the assembly and use the insert constraint to put the collar into the
bearing
• Emphasize the option of offsets
• Check for problematic constraints by going to modeling toolbar and changing from
“Assembly view” to “Modeling view” and look for next to constraints
o It is easiest to just check the constraints and you can generally see what the issue
is
o If not, right click and use Inventor help
• The motion constraints are slightly more complicated – there are two options:
o Two round objects – gears and pulley systems
Different approach with circles and gears:
• With circles, you select the contact surface of the objects and the
ratio is automatically calculated using the diameters
• With gears, you select the hole of the gear and then enter the ratio
of teeth
o A round and a flat object – rack and pinion systems
Select the edge of the round object to highlight the rotational axis
Select the REAR EDGE of the flat object
Enter the distance that the linear object moves for each round object
revolution (circumference!)
• Excellent resource to explain this:
http://usa.autodesk.com/adsk/servlet/item?siteID=123112&id=3028036
• Point out that multiple assemblies can be combined to form a more complete assembly
(and they will be doing this later!) so it is important to use proper constraints even now!
• Once an assembly is complete, it can then be inserted onto a drawing file as we did
before
o Use “Drawing Annotation Panel” to add balloons and parts list – line up balloons!
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CAD Resources >
Inventor Assembly Tutorial
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