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Drawing with the Line tool

From: Up and Running with Autodesk Inventor

Video: Drawing with the Line tool

In this movie, we're going to focus on drawing with the Line tool. And the time is finally come to begin creating sketches that will turn into 3D parts. We'll pull together all the things we've learned up to this point to begin creating our first part. We'll start by creating the starter mounting plate. I have the assembly of the engine opened so that we can get a feel for the part we're going to be creating. In this case, it's located right here on the back of the engine and attached to it is the starter cover, which covers the mechanism that will be used to start the engine.

Drawing with the Line tool

In this movie, we're going to focus on drawing with the Line tool. And the time is finally come to begin creating sketches that will turn into 3D parts. We'll pull together all the things we've learned up to this point to begin creating our first part. We'll start by creating the starter mounting plate. I have the assembly of the engine opened so that we can get a feel for the part we're going to be creating. In this case, it's located right here on the back of the engine and attached to it is the starter cover, which covers the mechanism that will be used to start the engine.

To get a better look at this part I'm going to right-click on it and select Open so that it appears in its own window as if I've opened part file by itself. This should allow us to see a basic overview of what this part looks like and the components that we're going to begin sketching. Now in this case, the most important part is the base, the large rectangle that everything attaches to. Whenever I'm creating parts I like to try to start with the most significant piece of the geometry and build from that.

To begin, I'm going to start a new sketch file, I'm going to go ahead and close these part files and the assembly file, because we don't need them to move forward. From the Ribbon bar I'll click New and select Standard part. With an empty file we need somewhere to sketch from, and you can remember from the origin video that when creating a sketch Inventor will present the origin geometry and allow you to select a plane to sketch on. In this case, I like sketching my base features on the X, Y plane, so I'm going to left-click on that and the sketch will become enabled, and I'm ready to begin sketching my first part.

Now reality is this is about the Line tool, but more than the Line tool we'll be talking about the heads-up display. I mean creating a line is as simple as left-clicking once and left-clicking again to create a line, that's not so much important. What's important here along with creating the line is the heads-up display, the constraints that are being applied, and how to add dimensions on the fly as needed. So to begin I'm going to right-click to bring up the marking menu, and I'm going to select Create Line.

When I do that the heads-up display appears and shows me the coordinates of where my cursor is located in relation to the center point which was projected to this sketch. As I move closer to the center point, you'll notice that my coordinates began to approach zero. When I get to the center point the icon or cursor will snap to the center point, a green dot will indicate that a coincident constraint is going to be created, and you'll notice that the coordinates are at 0, 0. This is a good practice.

I'm going to go ahead and left-click to start this from the center point and locking sketch geometry to this center point is a good habit to get into. The reason for that is once you've locked to the center point, the remaining sketch geometry that's created is much more predictable. As you add dimensions and constraints you know where things are going to grow from, and that's the center point you lock to. Now that I have selected the starting point, the heads-up display changes and gives me some good information about what's next.

Not only am I selecting the last end point of this line, but you'll notice the dimensions have appeared. I have a length dimension and an angle dimension. You'll notice that the length dimension is highlighted in blue as if it's ready for text input. I know that this part is 1.575 inches square, so I'm going to type that on my keyboard, and you'll notice those are input into the dialog box. If I hit tab on my keyboard a couple of things happen. First I switched to the angle constraint where I could type in a dimension value for that, but more importantly the 1.575 length dimension has received a Lock icon next to it.

This indicates that I have manually input some value there. And as I move my cursor, no matter where I move it, you'll notice that that line is locked to that point. If for some reason I made a mistake you can always hit tab to return to that, type in a new value, hit tab to accept it, or if I hit tab to return to it I could hit Spacebar to clear it, and I'm actually back to not applying an actual dimension. I am going to go ahead and enter it in this case, because I think it's important that you see how dimensions can be applied while you're sketching, but also because as we move forward I'm not going to use the dimensions, and I want to show the difference between the two.

Now that I am ready to select my end point as I hover near Horizontal another thing happens. You'll notice near the end of the cursor a Horizontal icon indicator has appeared. This lets me know that Inventor is ready to automatically apply a horizontal constraint, and if I left-click you'll notice that the line is purple as opposed to green, which if you remember from our previous sketch movie, indicates that this line is fully constrained, and the reason for that is we have a dimension and the horizontal constraint locks it into position.

I am now ready to continue with the Line command. You'll notice that the command is still active and in this case it's using the end point of the previous line to begin this line. So now all I need to do is select an End point here, and as I hover near Vertical, again, a Constraint icon or Glyph shows up near the cursor. It also shows up near the original horizontal line, and in this case it's applying a Perpendicular constraint as opposed to a Vertical constraint. The reason for that is once geometry is created Inventor prefers to use existing geometry to create constraints as opposed to just applying a horizontal or vertical constraint.

In this case, that works for me, I'm going to leave this to be perpendicular, but in this case I'm not going to add the dimension, I'm going to use that length dimension as a reference. I'm going to get it to roughly 1.5, and I'm going to go ahead and left-click to end that line. The next line I create is going to be the horizontal line that runs across the top of the square. You'll notice as I hover around the Graphics window, and I get near where the midpoint of the bottom line is the heads-up display shows me an Alignment indicator.

This isn't going to add a constraint specifically to lock it to the midpoint, but it's a nice way to let me know exactly where I am in the sketch environment. In this case, I do want to go ahead and move all the way over to the end above this center point, and you'll notice that Inventor is ready to apply a parallel constraint based on the icon shown in the heads-up display. If I don't want that, say for example, I really want this to be perpendicular to the line here, I can simply hover over that or scrub over it, and that will become the active piece of geometry that Inventor uses for reference.

In this case, now I'm looking to apply a perpendicular constraint to the previous line and at any point during the sketch process I can select any piece of geometry to make that be active reference point. I'm going to go ahead and let it apply the parallel constraint, I'm going to left-click to end the line and then I'll finish it off by left-clicking at the center point or where I started. I am going to right-click and hit Cancel to end the command, you'll notice here one unique item in this sketch, and that's that the horizontal line at the top is actually green, which means it's unconstrained or under constrained.

To review let's go ahead and right-click and select Show All Degrees of Freedom. Here you can see that the line is allowed to move up and down, but it is not allowed to move to the right or left. We know that this sketch geometry is still unconstrained because we did not apply that dimension to the vertical line on the right. We'll get to that in the Dimension movie, but for now we'll go ahead and hide all the degrees of freedom and continue on with our sketch. I am going to go ahead and launch the Line command one more time, and this time we're going to use the existing geometry to create the overhang that will define part of the starter cover that attaches to this piece.

I am going to left-click on the line to begin our new piece of geometry. I'm going to left-click again to find its end point and then I'm going to return to that original line again and left-click just to define the basic shape of our overhang, and in the next movie we'll look at how to dimension that.

Show transcript

This video is part of

Image for Up and Running with Autodesk Inventor
Up and Running with Autodesk Inventor

40 video lessons · 8603 viewers

John Helfen
Author

 
Expand all | Collapse all
  1. 1m 28s
    1. Welcome
      41s
    2. Using the exercise files
      47s
  2. 8m 3s
    1. Exploring major workflow steps
      2m 19s
    2. Reviewing different file types
      4m 43s
    3. Exploring essential settings
      1m 1s
  3. 21m 39s
    1. Navigating using the ViewCube
      3m 26s
    2. Navigating using the navigation tools
      5m 36s
    3. Using the browser
      3m 17s
    4. Using the ribbon bar
      2m 10s
    5. Using the Quick Access Toolbar
      1m 4s
    6. Customizing the toolbars
      3m 7s
    7. Using the Marking menu
      2m 59s
  4. 48m 42s
    1. Introducing sketching
      3m 18s
    2. Working with origin geometry
      3m 47s
    3. Understanding constraints
      8m 43s
    4. Drawing with the Line tool
      8m 8s
    5. Dimensioning a part
      5m 0s
    6. Creating parameters
      8m 50s
    7. Creating circles and rectangles
      10m 56s
  5. 38m 31s
    1. Introducing part modeling
      2m 34s
    2. Creating a base extrusion
      5m 12s
    3. Creating multiple extrusions
      7m 35s
    4. Creating a cone by revolving
      6m 12s
    5. Creating holes
      6m 12s
    6. Creating a threaded hole
      3m 3s
    7. Using placed features
      2m 33s
    8. Editing part features
      5m 10s
  6. 25m 52s
    1. Introducing assemblies
      54s
    2. Placing components
      6m 29s
    3. Creating and managing constraints
      7m 50s
    4. Assembling parts
      7m 16s
    5. Understanding the Insert constraint
      3m 23s
  7. 25m 12s
    1. Exploring initial drawing creation
      4m 43s
    2. Placing views
      6m 11s
    3. Creating section and detail views
      5m 10s
    4. Setting basic dimensions
      2m 43s
    5. Changing dimension precision
      1m 24s
    6. Creating baseline dimensions
      1m 52s
    7. Creating center lines, center marks, and hole notes
      3m 9s
  8. 1m 20s
    1. Next steps
      1m 20s

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