3D Modelling Workshop By Keith Phelan!

Welcome ! In this workshop, you will get familiar with the basic tools used to create 3D objects in Autodesk Inventor with a step by step tutorial! In this workshop, we’ll be making 2 objects.

Here’s the first object we’ll be making To make this object we’ll use: The circle and rectangle tools Extruding and cutting Fillets and chamfers Project Geometry Offsets And constraints

Let’s get started First we need to open up Autodesk Inventor. If you are using your own computer, use your university email and download Autodesk Inventor here: https://www.autodesk.com/education/free- software/inventor-professional Or type in ‘Autodesk inventor student’ into google. If you are a student (or have a school email), you can download Inventor free here: https://www.autodesk.com/education/free-software/inventor-professional (Only for windows computers)

Opening a new part project Welcome to the home screen. To start a new part: Click ‘New’ in the top corner Make sure you are in the ‘English’ folder Click on ‘Standard(in).ipt’ Click Create.

Starting a sketch Click the ‘Start 2D Sketch’ button Select the XZ Plane (The horizontal one) Find the rectangle tool Click the dropdown menu and select Two Point Center Rectangle

Making a shape Time to make our rectangle. Start by clicking on the origin point in your sketch Drag out the rectangle, type in ‘4’ to set the dimension of one side. Now press enter to make the shape. We will set the dimension of the other side in a second. Note that you can set both the dimensions now, but to demonstrate we will set the second after making the shape.

Setting dimensions Time to set the other dimension of the rectangle. To get out of the Rectangle tool press escape on your keyboard. To do so we use the ‘Dimension’ tool. Select both of the green lines, and set the dimension to 4 and press enter. Press escape to get out of the tool.

Great! Now what? We now have a 4x4 inch square sketch, we are now ready to ‘extrude’ the shape. Before we extrude our shape, we need to Finish the sketch. To extrude, we will be using a shortcut. Just press ‘e’ on your keyboard to start the extrusion. For now, just set the distance to 6 inches and click OK. Usually you have to exit the sketch to extrude. Note: because we only have one shape on this sketch, our shape extrudes automatically, but usually we have to manually select what we want to extrude.

Making a new sketch & The View cube Now that we have an object, we can start to modify it. To do so we have to step into another sketch. Click on start 2D Sketch, and select the ‘Front’ face of the object. How do you find the front face? Use the view cube! This is the view cube. Click and drag to rotate the object, or click on a face/corner/edge to center the camera where you clicked. You can use Shift + middle mouse to more your object also. Middle mouse click will pan the camera.

The Circle Tool Now we’ll be making new shapes on our new sketch. Place two circles on inside the object, set the diameter of each to 1 inch. Now we are going to center them. Click on the ‘Vertical Constraint’ tool and select the Center point of each circle, and the middle point at the bottom of the object.

Constraining the holes Now we will set the vertical dimensions of the circles. Set the center point of the bottom circle 1.5 inches from the bottom, and the center point of the top circle 3 inches from the bottom circle, and start an extrude with ‘e’, selecting both of the circles. We’ll change the extrude settings in the next slide. Finish the sketch.

Cutting the holes Welcome back to the extrude menu. This time, instead of extruding, we’ll be cutting into the object. Set the operation to cut (this button) Set the direction to back ( ) And set the distance to 3 inches. Press OK.

Fillets Fillets and chamfers are usually reserved to finish up a part, but for today we’ll be using them a bit early. To start a fillet, click the ‘Fillet’ button. Let’s set the radius to .5 inches and select the four top edges of the piece. Click OK.

Chamfers Next we will use the chamfer tool, which is very similar to the fillet tool. Select ‘Chamfer’ and select the four vertical edges of our shape, remember to rotate the part with the view cube. Set the distance to .25 inches.

Project Geometry Project Geometry is a very useful tool in Inventor. You can project edges, vertices, shapes, and curves with this tool. To start, make a new sketch on the top face of our object. Our goal is to project the inner shape that was made with the fillets and chamfers. Click somewhere inside the shape when all of the edges are highlighted at once. Make sure you click escape before moving on!

Offset Offsets use the outline of a shape to make either a bigger or smaller version of that shape. Select the ‘Offset’ tool. Select the shape we projected, and set the distance between the two to .25 inches. Press escape to leave the tool.

Final extrude For the final extrusion for this part, we are going to need to Finish our Sketch. We are going to extrude the inner shape. Set it to extrude back Make sure the operation is ‘cut’ Set the extent to ‘all’. Click OK. You can modify anything by double clicking the feature in the model menu.

Changing the appearance / material The last thing we’ll do to finish up this beautiful part is change it’s appearance. Click on the blank space next to the object, and then find the material menu near the top of the program. Set the appearance to Glossy – Gold, or whatever you prefer.

And there we have it Congratulations, you have officially finished your first part. Now onto the second one.

Starting our new part To start the new part, click on ‘My Home’ near the bottom of the window. Back on the home screen click ‘New’ again, and create a new Standard(in).ipt part.

Here’s what we’ll be making To make this screw, we’ll be using tools and techniques we just learned, as well as new ones, including: Line Arc Revolve Offset from plane Point constraint And Angular dimensions

Let’s go Create a new 2D sketch Start a sketch on the XY Plane.

The line tool Select the ‘Line tool’. Make a vertical line extending up from the Origin point 5 inches. This will the center of the screw, which we will revolve around Press escape to exit the tool.

Making the body of the screw To continue the body of our screw, we will make a new line extending from the origin at an angle. After that line is created, make a vertical line connecting to the angled line. If you need to, use the ‘Vertical Constraint’ tool on the second line.

Constraining the lines We’ll start with the angle constraint. Select the ‘Dimension’ tool, select the constrained (purple) line first, then the angled line second. Where you click when you make the constraint is important: Make sure you make the angle acute. Set the angle to 30 degrees.

The remaining constraints Set the unconstrained line to be 3.5 inches long. Set the distance between the top point of the angled line and the Origin point to .75 inches. A point should appear when you hover over the endpoint of the line.

Starting The head of the screw Now that we’ve made the body, we can start work on the head of the screw. To start, make a horizontal line extending right from our 3.5 inch line. Set this new line to 1 inch.

The arc tool Let’s use a new tool to complete the head of the screw. To achieve a curved line, we use the ‘Arc tool’ Select the tool, and click on the top point of the 5 inch line, and the rightmost point of the horizontal line to start the arc. When moving your mouse you should notice you are changing the radius of the arc. For now just click to create the arc. Note: Make sure to make your arc domed (pictured) instead of concave, or our next step will not work.

Constraining the arc To constrain this arc, we will be using the Coincident Constraint Tool. Select the tool, then select the center point of the arc, after, click anywhere on the 5 inch line. Our sketch should now be fully constrained.

Starting a revolve So why did we only make half the screw? We actually only need half of the profile of our object to revolve our part. For any revolve we need our profile (what we are revolving) and an axis (the axis we revolve around). To start our revolve, finish the sketch and press ‘r’.

Revolving the part The profile of our part has already been determined since we only have one closed shape, so we only have to select the axis of rotation. For our screw, the axis is the 5 inch center line. Select axis, and then select the line. Click OK.

That is a thumb tack “You said we would get a screw, what gives?” Let’s add a crosshead design to our screw. To do so we need to make a new sketch, however there's no flat plane to make a sketch on. This is where we use the ‘Offset from plane’ tool. Click on the dropdown menu below the ‘Plane’ tool, and select ‘Offset from plane’ What plane are we offsetting from? The XZ Plane. To get to this plane, go into the ‘Origin’ folder in the model menu. Select the XZ Plane, now set the offset to 5 inches, which is the length of our part. Press enter.

Now we have a plane We can make a sketch on this new plane. Click on one of the corners of the new plane, highlighting it, and then click Start 2D Sketch. Once the sketch is made, you can right click on corner of the plane and uncheck ‘Visibility’ to make the plane invisible.

Making the cross head Now that we are in a sketch, we will make 2 ‘Two Point Center’ rectangles, use the point in the middle for the center of the rectangles. Make one rectangle 1 inch long by .25 inches wide. Make the other .25 inches long by 1 inch wide.

Cutting the cross head Finish the sketch. Start an extrude and set the operation to cut. Set the direction to back. Set the distance to .5 inches. Click OK.

Making the “Thread” We are going to give the screw a thread now. The “thread” we are using is just an image giving an idea of what the thread should look like. Select the shaft of the screw, it should be highlighted. Click the ‘Thread’ button, and click OK.

Setting the Material For the last part, we set the appearance, and for this one we will set a material. The material is the first dropdown menu at the top of the program. I set mine to Steel – Alloy. The program automatically set the appearance to Semi - Polished.

Thank you! Congratulations on making these two parts in Autodesk Inventor. Hopefully, you have learned an assortment of valuable tools and techniques to model objects in this program. Thank you for participating in this workshop!