# 2809 CAD TRAINING: Part 1 Sketching and Making 3D Parts. Contents

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1 Contents Getting Started... 2 Lesson 1:... 3 Lesson 2: Lesson 3: Lesson 4: Lesson 5: Final Project:... 28

3 Lesson 1: Open Autodesk Inventor and from the drop down menu select New In the pop up menu select the Metric tab and scroll down to find Standard (mm).ipt Every CAD program has different file extensions, for Inventor parts are.ipt assemblies are.iam and 2D drawings are.dwg. For now only worry about.ipt. We are going to do these tutorials in metric but the units can easily be changed to imperial. Now we have created a new part and Inventor has automatically created a new Sketch for us. Sketches are 2D drawings; the basic work flow of CAD is like this -> create a 2D sketch then create a 3D feature from that sketch. Select the top left corner Create a 2D Sketch then click on a plane to start your sketch.

4 Take a moment to look at the ribbon interface across the top of the screen; we are in the sketch tab. If you are ever confused and can t find a tool make sure you are in the right tab. Now it s time to begin modelling our part. Select the rectangle tool and draw a rectangle, don t worry about its position or size etc. we ll take care of that later. Select the Line tool and draw the following lines in your rectangle, again don t worry about exactly how they look for now. Make sure that your lines are connected to the rectangle at the end, your cursor should snap to the rectangle when you are close by. Also watch the symbols that Inventor is showing you as you draw, you ll probably notice the parallel and perpendicular symbols: this is Inventor creating constraints as you draw. Don t worry we ll learn more about constraints as we go.

5 Select the Trim tool and click on the line pointed to in the image below: You should be left with this: Trim removes lines between or after another line intersects. In this case it removed the portion between the two intersecting lines. Trim is very useful for creating geometry. Next select the circle tool and draw a circle inside the shape we have made. This should be your result:

6 Before our sketch is finished we need to apply some dimensions and constraints. Dimensions force the given section to be a certain length and constraints for a certain geometric relationship. You can add a dimension either by clicking on a line itself or by clicking on the lines on either side like the illustration below: Clicking these 2 lines will allow you to dimension how much should be between them and because the other line is connected its length will change too. Add these dimensions to your sketch:

7 Next we are going to apply a constraint to the circle. Select horizontal from the constraints. Pick the center of the circle and then carefully hover along the vertical line at the right end of the rectangle, when you pass the midpoint of this line your cursor will change to a green circle instead of yellow, click to finish the constraint your circle should now be centered vertically in your shape. Apply a dimension of 10 mm between the center of the circle and the vertical line on the right and make the diameter of your circle 10 mm. Finally lets apply a coincident (fancy way of saying in the same place) constraint between the center of the circle and the sketch origin (the intersection of the darker blue lines) The result should look like this: I would like to take a moment and mention a few things, first there is no right way to do things in CAD; there are often many ways to accomplish the same thing. I recommend always using the simplest way you can think of. For example we could have used many complicated constraints to make this sketch but instead we used a lot of simple dimensions, this is good for 2 reasons, it was easy to do and easy to understand if we have to come back to edit it later. In this lesson so far we introduced 2 of the many constraints horizontal and coincident. The remaining constraints are pretty self-explanatory just think about geometry class!

8 Also notice how we only needed to dimension 1 side of the rectangle, that s because Inventor automatically created constraints for us that keep the sides equal to each other. If you try to dimension the other side Inventor will warn you about an over-constraint this happens when the shape is already fully defined with constraints and dimensions in other words that side length is already determined: it cannot be anything else or it would disobey the laws of geometry. Don t worry about learning every tool in CAD: Neither I nor any of your other mentors know them all; we just know the basics and then we need something else we look at what tools are available and play around until we get our result. Let s finish our part. Click on finish sketch in the top right of the screen. Observe how the view changes to a 3D or isometric view. On the ribbon interface switch to model and then select the extrude tool. Select the profile of our sketch (it will become shaded light grey), choose 10 mm for the distance and press okay. You should see this on your screen.

9 Now look at your screen on the left. A tree view is being created of how your part was made. At any time you can edit any step of how your part was made, sometimes this works great and we can easily change the part other times when the part is really complicated it doesn t work so well. There are ways to fix this and work through it but for now let s just focus on the basics and we can help you with making changes to complicated parts. Click the plus next to Extrusion one and then right click on sketch 1 and select edit sketch. Change the diameter of the circle to 5mm click finish editing sketch. Observe the result:

10 Now let s make a new sketch. Click Create 2D sketch and click on the main surface of the part. Your screen should look like this: Click the circle tool and hover your mouse over the hole through the part when it turns green draw a circle. Make the diameter of that circle 10 mm. Your part should look like this: Finish the sketch.

11 Make sure you are on the model tab then select extrude. Select the profile of the new circle we just drew then from the extrude pop up select cut and make the distance 5 mm. Click OK and look at your new part. Save your part as lesson1.ipt you ll need to submit it later.

12 Before moving on take a few minutes to familiarize yourself with looking at a part in 3D. You can access all the move/rotate/zoom commands from the dock bar on the right of your screen, however I recommend using the keyboard short cuts. Pressing in the roller wheel on your mouse will pan or move your view of the part around. Holding shift and clicking the roller wheel will let you rotate the view of the part rolling the roller wheel will zoom in and out. You can also use the cube in the upper right corner to select certain viewpoint. It is important to note that you are not moving the part; think of it as moving yourself around the part so you can see different things. Congratulations you have finished lesson 1 and are well on your way to be CADing robots! You might not believe me now but CADing is actually quite simple, there may seem like a lot of tools, and there are, but 95% of parts are made using the simple sketch, dimension, extrude, cut process you just learned!

13 Lesson 2: Open Inventor and start a new metric part. In the new sketch draw this shape (Don t worry about the exact shape we ll dimension it later). Now add these dimensions: Now try and dimension the angle between these 2 lines by clicking on them:

14 You should get this error: Because the other side lengths are dimensioned the angle must stay at its current value or else the geometry is impossible. A driven dimension will show up but it cannot be changed it just displays the dimension. Click cancel and delete the 25 mm dimension of the top line (press esc to make sure you re not using the dimension tool still if you are having problems doing this, esc is the Inventor cancel and resets your tool to be a plain cursor). Now dimension the angle and make it 120 degrees:

15 Now try and dimension the top line again, you should get this error again: Hopefully this helps make sense of over constraining the sketch. Press cancel and finish the sketch. Extrude your part 15 mm.

16 Start a new sketch on the front face: Click on the view tool bar and select view face, click on the sketch face. Your screen should now look like this:

17 Draw and dimension this sketch (it s only 1 line): Finish the sketch and extrude cut the upper left profile away from your part. Instead of distance in the extrude pop up, change to all, this will cut through all material. Result:

18 If you ever have difficulty selecting your profile for extrusion it is probably because your profile is not closed, one of the lines does not actually contact or connect with one of the others, think of how the fill tool in paint works. Also when you are creating more complicated sketches you may need to use construction geometry these are lines that you draw to help you position and dimension other elements of your sketch. When you try and extrude though Inventor doesn t know the difference and it will make it hard to select the profile you want. Thankfully in the sketch mode you can select lines and make them into construction geometry so that Inventor knows the difference. Save your part as lesson2.ipt. Congratulations you ve finished lesson 2.

19 Lesson 3: Open Inventor and start a new metric part. Draw 2 circles a fair distance apart: Dimension both these circles to be 20 mm in diameter and then apply a horizontal constraint between the 2 circle centers: Select the line tool and hover in on the top of the circle right above the center. Observe the tangent symbol that pops up and the dotted line that appears on its way to the other circle. Click and draw the line tangent from one circle to the other. Do the same for the bottom. Hover and then click here

20 The result should look like this: Now use the trim tool to get rid of the inner circles: Add dimension of the upper line of 30 mm.

21 We are going to draw 2 new circles, the first one just draw anywhere, for the second one snap it to the center of the arc of one of the end circles: Now select the coincident constraint and constrain the first circle to the center of the other sides circle. Dimension both circle to 10 mm. This was to demonstrate the difference between letting Inventor generate constraints as you go vs. adding them yourself later. Select the circle on the right and change it to construction geometry. Finish the sketch.

22 Open the extrude tool and observe only the one circle cut out is part of the geometry, extrude the part 10 mm. Open the sketch again and return the other circle to non-construction geometry (click on the circle, then click on construction again). Extrude the part again. Wait the part is the same! Right click on the extrude feature in the model tree and click edit feature. Select the profile button and then while holding ctrl click on the second circle, this will deselect it from the profile. While you re in here change the height of the extrusion to 5 mm. Save your part as lesson3.ipt. On to lesson 4!

23 Lesson 4: Open Inventor and start a new metric part. In this lesson we are going to learn the second most common way to make a 3D part from a sketch a revolution. To demonstrate this we re going to make a model of the Stanley Cup! Start a new sketch and draw a long horizontal line, immediately make it construction geometry. Then draw something like this: (Note: Dotted is construction geometry.) Notice how if you move your mouse to a point of interest (like the circle center) and then up it tracks your movement, this is to help you create a line from above that will pass through the center of the circle. Inventor will help you like this in lots of ways, you just have to get used to it. Now let s do some clean up with trim and add some dimensions (you might need to delete the circle at the end, add the dimensions, and then redraw the circle): Also draw a line from to close the bottom of the profile.

24 Finish your sketch: instead of clicking on extrude this time pick revolve. Pick the profile for the profile and then pick the original long construction line for your axis, this should be your result: Doesn t look much like the Stanley Cup, but that s not important. Revolve is a useful tool especially for making shafts! Save your part as lesson4.ipt

25 Lesson 5: The best way to learn how to CAD is lots and lots of practice! You ll develop your own style and learn most by modelling lots of things! For lesson 5 you need to create solid models of the following parts, save them by the name indicated underneath the picture. You need to submit all these drawings to get your K-Botics CAD certificate! Practise by drawing all these simple shapes: Just pick dimensions that make your model look close to the picture it doesn t have to be exact. Save the files using the naming convention simplea.ipt through simplef.ipt

26 Model 6 Parts from this page of your choice, again just pick dimensions that make it look similar not exact:

27 Model these 3 Blocks, again picking dimensions that make the part look right. Name files according to the name that appears under the image. Block-A Block-B Block-C

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