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Creating multiple extrusions

From: Up and Running with Autodesk Inventor

Video: Creating multiple extrusions

Now that we have our BaseExtrusion, we're ready to continue on. The process from here on out does begin to get a little bit repetitive. So I'll make sure to call out all the actions that I'm taking, and more specifically, call out any new actions that will help you better understand the Extrusion process. To begin, we need to create a sketch on the top face of this part. We can select that face and use the heads-up display to create a new sketch. We know that this boss needs to be centered on the part. In order to do that, I'm going to create a line, I'm going to lock it to the midpoint of one of the projected edges, and I'm going to actually enter its dimension here in the heads-up display.

Creating multiple extrusions

Now that we have our BaseExtrusion, we're ready to continue on. The process from here on out does begin to get a little bit repetitive. So I'll make sure to call out all the actions that I'm taking, and more specifically, call out any new actions that will help you better understand the Extrusion process. To begin, we need to create a sketch on the top face of this part. We can select that face and use the heads-up display to create a new sketch. We know that this boss needs to be centered on the part. In order to do that, I'm going to create a line, I'm going to lock it to the midpoint of one of the projected edges, and I'm going to actually enter its dimension here in the heads-up display.

In this case, it's going to be .319 from the edge. I'm going to hit Escape on my keyboard to get out of the command, and I'm now ready to create the circle that will create the boss. From the Marking menu, I can select Circle, and I can lock the center point to the end of the line I just drew by left-clicking on its endpoint. We know this circle needs to be .419 in diameter. I'm going to enter that into the heads-up display and hit Enter on my keyboard to create that dimension and the circle at the same time. We can now finish this sketch, and we're ready to make our second Extrusion.

From the Marking menu, I can right-click and select Extrude. I can select the circle we just drew, and in the heads-up display I'm going to enter a value. In this case, this boss needs to be .278 tall. Now in the previous Extrusion, we chose to make it symmetric, in this case however we can just use Extrusion to a distance, which is actually the default for the command. With that value entered, we can hit the check box and our Extrusion is created. You can see it here in the browser. Next, we're going to use that Extrusion that we just created as a starting point for the third Extrusion.

We're going to select the top face, create a sketch, and this time we're going to create a circle, lock it to the center of the previous circle, and set its diameter to .462. Hitting Enter on the keyboard accepts the entry and creates the circle. Now we can finish this sketch, and we're ready to extrude again. Right click to bring up the Marking menu, select Extrude, and this time you can select both circles that were created. The first one was from the Projected Geometry and the second one was the one we created.

We want to extrude both of those. Now you'll notice the Extrusion is facing in the wrong direction. In this case, we want to make a little lip on this boss. To change the direction from heads-up display, we can simply select the direction icon and select the opposite arrow that is being displayed. You'll notice when we do this, it changes to a cut operation. You can tell this from the red preview which indicates that material is going to be removed. In this case, we want to actually add material. So from the heads-up display, we can choose to join material.

The next problem we have is that it's remembering the .278 that we used in the previous Extrusion. In this case, we need to change this to .128. You'll now see that we have a lip, it's the proper dimension, it's the proper height, and we can now hit the check mark to accept this, and we have our third Extrusion created. The next several Extrusions are going actually take place on the bottom of this part. We can use the ViewCube to rotate to be able to see the model from below. We can right-click and from the Marking menu, select New Sketch and then select the face on the bottom of the part.

It rotates into a normal view so that we can see the sketch, but this one's going to start a little bit differently. We're going to return to our Home view, and we're going to project the circle that we created in the second Extrusion to this sketch. The reason for that is we know they're identical, we know that they're perfectly aligned in the same diameter. So rather than create a completely new sketch, we're going to add intelligence by telling the system that we want to project an existing piece of geometry into the sketch, and by clicking on that we can then rotate around to look back at our sketch, and you can see the new piece of geometry has been created.

We can get out of that command, and that's all we need to do. Because the geometry was projected, it's actually being controlled by another feature. We can simply finish the sketch, use the Marking menu to launch the Extrude command, and select that circle. In this case, we know the distance is .404. We'll enter that, and we'll hit Enter on the keyboard to accept that value. We now have Extrusion 4 listed in the browser, and we're ready to continue on. The next two extrusions are an extension of this one. We're going to start a new sketch from the Marking menu, select the bottom face that we just created, and we can create a new circle to represent the lip on the bottom of this part.

In this case, it's .485 in diameter, I will enter that on my keyboard and hit Enter, and we're ready to finish this sketch. With the sketch finished, we'll return to our Marking menu and launch the Extrude command, select both profiles, and in this case extrude them to a depth of .033. Hitting Enter on the keyboard accepts, and we have another Extrusion. We have one final Extrusion on the bottom of this part. The process is identical. We're going to create a new sketch, select the face we want to sketch on, from the Marking menu, we're going to bring up the Circle command again, walk to the center point, and this time we're going to create a circle with a diameter of .390.

We can finish the sketch and from the Marking menu, again launch Extrude and select the circle we just created. This time we're going to extrude to a distance of .345. Hitting Enter on the keyboard accepts that, and we can return to our Home view and see where we stand in with this part. The final two extrusions we need to create are actually going to be created on the backside of the part. I'll use my ViewCube to rotate into a better view for this, and we can start a new sketch. I'm going to select the face I want to sketch on, in this case we're going to use some geometry to center this part.

We're going to create a line and connect it from corner to corner on the projected edges. We're going to finish that command, and we're now ready to add our boss. We're going to right-click and select Circle from the Marking menu, we'll lock to the midpoint, and we'll set the dimension for this to be .45. Hitting Enter on the keyboard creates the geometry. We can then finish the sketch, from the Marking menu, launch the Extrude command and select the circle we just created. This actually brings up a good point. Now while I was selecting that, because I didn't turn that line that we were using as construction into construction geometry, the Extrusion command is finding that, and it's creating closed profiles because of it.

So rather than accept this, we're going to hit Escape, we're going to go back and edit the sketch by selecting a piece of the geometry, and from the heads-up display, select Edit Sketch. At any point when you're doing extrusions or any other modeling action, if you find that there is a piece that you need to make changes to, you can always return and make edits. I'm going to select that line, right-click and select Construction, and then finish the sketch. This time when we launch the Extrude command, the command is actually ignoring that line, making it very simple to select the extrusion that we need.

In this case, the extrusion needs to be to a depth of .09. We'll hit Enter on the keyboard, and we've created our Extrusion. The final extrusion builds off of the one we just created. We'll select the face on the model and use the heads-up display to create a new sketch. Next, we're going to draw another circle, and we're going to give it a dimension of .548, hit Enter on the keyboard to create that, and we're going to finish the sketch. For the final extrusion, we need to select both profiles, flip the direction by selecting the opposite arrow that's being displayed, set the operation from Cut to Join, and adjust the dimension.

In this case, it's going to be .027. Hitting Enter on the keyboard accepts our entries, and we can return to our Home view to look at our final part.

Show transcript

This video is part of

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

40 video lessons · 8016 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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