Inventor 101

DO NOT REPLY TO THIS THREAD.

If you feel the desire to respond or need further instruction - start a new thread and paste the reference url in your new thread.

http://www.cadtutor.net/forum/showthread.php?85808-Inventor-101

This thread will present a beginner tutorial for using Autodesk Inventor.

Start a new Standard(mm).ipt part file.

the *.ipt file extension stands for Inventor Part.

If you somehow get inch units rather than mm - don't worry about it for now.

Expand the Origin folder in the feature browser and right click on Center Point and select Visibility.

Right click on the XY Plane in the browser and select New Sketch.

Start the Line command and sketch a line from the Center Point to the right and dimension the length as 60mm. (be sure to enter the mm units)

Click on the line and change it to Centerline as shown in image below.

If you correctly started using the mm template - you do not need to enter the mm units.

If you incorrectly started using the inch template - Inventor will automatically convert mm to inch value, but you must enter the mm units for every dimension.

More on this later.

Notice in the lower right hand corner of the screen that Inventor reports that our sketch (the line) is Fully Constrained.

No other information is needed to define the position or size of the line.

If at any step Inventor does not report your sketch as Fully Constrained, then stop, Stop, STOP - you have done something wrong or missed an important step.

Ask questions.

Sketch a vertical line from the Origin Center Point (the left end of the line) as shown.

Try dragging the free end of the line.

You should be able to stretch the line but not change the angle - it should remain vertical.

You should not be able to drag the other end away from the Origin Center Point.

In the lower right corner Inventor should report 1 Dimension needed.

Next we will add that dimension in a special way.

Start the dimension command and

1. Click on the centerline (on the line, not on an endpoint or midpoint - the line).

2. Click on the free endpoint of the vertical line.

3. Click in space to place the diametrial dimension and enter the value.

Inventor should now report that the sketch is fully constrained.

Save the file with the name Punch Bushing. (Inventor will prompt you that you need to exit the sketch in order to save the file.)

Close the file. (and any other Inventor files you might have open).

Go to Windows Explorer and create a New Folder named Punch Press at some convenient location. (on your hard drive or USB thumb drive)

Move your Punch Bushing.ipt file into this new Punch Bushing folder.

(Normally it is bad practice to use Windows Explorer to move Inventor files around like this - we will see why when we get to assemblies.)

If you do not know how to do this STOP, you are not ready to learn a professional program like Autodesk Inventor.

If you do not know how to create a folder to store your files, then sign up for a beginner computer literacy class at a school near you and come back to continue this tutorial when you have completed the class.

We are going to create all of the parts and then assembly the parts together of a Punch Press.

All of these files will be hyper-linked together parts/assemblies/drawings.

So that the hyper-links do not become "broken" we should create an Inventor Project (*.ipj) file that will keep track of our files. This is not a requirement, but will help with file management.

Find the Project icon somewhere on the Inventor ribbon interface (cannot have any active Inventor files open while doing the next few steps). Click on the icon.

Note the checkmark next to the Active Project (there can be only one project active at a time).

(your project list might look different than mine)

Click on New at bottom of dialog box to create a new project.

Select Single User Project and then Next.

Type Punch Press as the project name and then Browse to the Punch Press folder path that you created.

Select Finish at bottom of dialog box. (there should be a checkmark next to your project in the list as it is now active) Then click Done.

If you do not know how to do this STOP, you are not ready to learn a professional program like Autodesk Inventor.

Return to the school where you completed the Computer Literacy class and demand a refund of your tuition.

Find a new school, complete the class and return here when finished.

Open the Punch Bushing part file.

Right click on Sketch1 and select Edit Sketch.

Double click on the 60mm dimension and change to 65mm.

Click the green checkmark to Finish Sketch.

Oops, we are not finished with editing Sketch1.

Right click on Sketch1 in the browser and select Edit Sketch.

Add the remaining 4 lines and two dimensions to close the loop as shown.

Note that Inventor should report that the sketch is Fully Constrained.

Notice also that when you added the dimensions to fully define the sketch - that it also changed to a darker color.

Click the green Finish Sketch checkmark and Save the file.

Every time we do something right - save the file.

Click the Revolve tool and then OK.

You should now have our first feature.

Did something right? Save the file.

We can edit the dimensions of our part at any time.

I made a mistake.

Click on the + symbol next to the Revolution1 feature in the browser to expand.

Right click on Sketch1 and select Edit Sketch.

Change the 65mm dimension back to 60mm.

Click the green Finish Sketch icon and our part updates to the correct length.

Let's assign a material to our part.

Click the down arrow in the location shown in red circle in image.

Set to Brass, soft yellow.

This does more than apply a color - it applies actual material properties that will allow Inventor to calculate weight, Finite Element Analysis (FEA) and other physical properties.

Rotate the part around as shown.

Right click on the YZ Plane in the browser and select New Sketch.

(If Inventor rotates your part back around - rotate it back to the orientation I show - we will take care of that annoying behavior later (if it is occurring to you).)

Sketch a circle as shown - be sure to pick the Origin Center Point as the center location. After you dimension the circle - Inventor should report that it is Fully Constrained.

The next step is a little confusing as there are two different interfaces you could use -

the new heads up menus or the older dialog box.

Use either one to set the Extrude to Cut (watch the pop-up tooltips) and through All.

Tip - a red preview is Cut, green preview is Add, and blue preview is Intersection.

Select the Chamfer tool from the Ribbon Modify tab.

Again, there are two different interfaces - the new one and the older dialog box.

Either way - set the chamfer distance to 1mm and select the two edges shown.

Congratulations - we just finished our first (of 23) parts for the assembly.

Save the file.

Part #2.

Start a new Standard(mm).ipt file.

Start a New Sketch on the XY plane as shown.

Save the file as Index Bushing.

Extrude the circle by distance 15mm and click OK. Do it!

Oops, we made a mistake, no problem.

Right click on Extrusion1 in the browser and select Edit Feature.

Change the extrusion distance to 12mm.