Autodesk Inventor iDoor Tutorial
Page 1 - Starting the Sketch and adding parameters
The following tutorial is for Inventor 2010 and later versions of
Autodesk Inventor. The tutorial will lead you thru the steps needed to
create a skeletally controlled, multi-solid door; use the Create iPart
and Component Authoring
commands to
create and upload the part to Content Center
, then insert that single
part into an entire kitchen full of door opening sizes. From there, you will
learn to Make Components
from all of the inserted, multi-body parts.
If you are very new to Inventor, the tutorials that ship with inventor are pretty good, and you should take advantage of them, but anyone that is fairly good with the ribbon interface and is not incredibly stupid can master this tutorial with a bit of work.
Starting the Sketch and Adding Parameters
The skeletal model is the first, and most important step in the
creation of any model in my opinion; but in this case, the skeleton is not
derived
into anything as it generally is in old-school skeletal modeling. In
this, and many of the workflows you will see on this website, the skeletal
part is developed further using the multi-solid part functionality that is
now included (finally) in Autodesk Inventor 2010.
With the new multi-solid functionality, you can go far beyond the old skeletal modeling schema by developing skeletal layouts that are various combinations of solid bodies and sketches, which can be derived into other skeletal layout parts to create a skeletal system contained in a master skeleton file. This schema is how I created the model for the Free Small House Plans, and I will put up a page on how the schema works if there is any interest.
Back to the iDoor. The first thing to do is create a new part, and create a new
Sketch
on the XZ Plane
. If your part started with a sketch on the
XY Plane
, click the green Finish Sketch
icon
up on the right side of the sketch ribbon to get out of sketch mode, then right click
on Sketch1 in the browser and choose 'Delete' from the context menu. Now
click on Create 2D Sketch
in the browser and click on the XZ Plane
in the
browser's Origin folder ( the reason for doing this is so the part comes in
in the correct orientation when placing from Content Center
) .
Click the Finish Sketch
to exit out of the sketch environment again and save the file as iDoor.ipt
Rename the new sketch 'Layout', and open the Parameters
editing
window. Create the following parameters (note; due to a flaw in Inventor,
you cannot copy and paste in the parameter editor Update -- it has been
brought to my attention that you can copy & paste in the parameter editor,
but you must use the keyboard shortcuts, there is no context menu as you
would expect. Thanks Peter);
| User Parameters | Unit | Equation | Export? |
| Opening_Width | in | 12 in | No |
| Opening_Height | in | 24 in | No |
| Left_Stile_Width | in | 2 in | No |
| Right_Stile_Width | in | 2 in | No |
| Top_Rail_Width | in | 2 in | No |
| Bottom_Rail_Width | in | 2.5 in | No |
The comment field should generally always be filled out, even if you are
working in a single user environment. I say that because the model I am
re-creating to produce this tutorial was made by myself nearly a year
ago, and its a real pain in the ass trying to figure out what parameters
do what by the time the model is done and there are 59 (or many
hundreds) of them to sort
through.
Your parameters editor dialog should now look like this...
Now that the starting parameters are completed, its
time to start adding some geometry. Double click on the 'Layout' sketch in
the browser to activate it. Click the Two Point Rectangle
on the Draw Panel
of the ribbon
(the fourth icon in from the left in Inventor 2010),
and draw a box around the center point as shown in the next image.