Inventor Tutorial for the iDoor – 01

Inventor Tutorial for the iDoor – 01 – 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 my own home, 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…


Inventor Tutorial iDoor Page One Image 01

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.

Inventor Tutorial for the iDoor Navigation




iDoor Tutorial One

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