When I training Autodesk Inventor, I always take a little bit of extra time on the break out view in drawings. It's a great way of showing details for internal parts inside an assembly, and not difficult to create in Inventor.
|A break out view shown created|
But when creating a break out view, it's got one place that usually snags everyone as the first few times they use it. I know it got me when I first started it.
That step is, associating the sketch to the view. If the sketch isn't associated to the view, the break out view won't work, and the breakout command will error out.
|This is the error seen when the sketch isn't associated|
I'll talk about all the steps, and specify that special step to create the sketch association.
1. Click on the view that the breakout view will be placed on. The border will highlight, indicating it's selection. This is the critical step that will create the associated sketch!
|Make sure to select the view before creating the sketch!|
2. Now, click the "Create Sketch" icon. The sketch is created, and it's axes will center on the view. It's this centering of the axes that tells us the sketch has associated to the view.
|Creating the sketch|
|The centered axes tell us it's working|
|Sketch the break out view boundary|
4. Now click on the "Break Out" icon. Select the sketch with the view.
|The break out icon|
5. Define the options for the break out. One helpful tip is to point out that projected views can be used to help with the definition, not just the view that will host the breakout. In the image below, I've used a projected view to define the break out depth.
|Setting the options for break out|
6. Choose okay and the breakout view is created.
|The break out view created|
I could say "That's All Folks", but instead, here's a couple of other tips that I find helpful.
There will be times that not every component in the break out view is supposed to be sectioned, as step 6 shows above. Here's how to change that.
The first is to locate the part in the feature browser, right click on it, locate "Section Participation", and changed it's setting to "None".
|Setting the section options from the browser|
The other is to hold down the "Shift" key with nothing selected, and right click. Choose "Part Priority" from the menu.
|Setting part priority|
Now select the part on screen, right click, and the same options for "Section Participation" are available.
|Setting the section participation from the right click menu|
Which ever means you prefer, the sectioning for selected components can be turned off, if desired.
|A completed section, with specific parts unsectioned|
On a last tip, I've shown what happens when the selections are correct, but how can you tell when the view isn't associated, so a mistake can be quickly corrected before the error on view creation appears?
There are two quick ways to tell.
1. If the sketch is created, but the axes aren't centered on the view, the sketch isn't associated.
2. If the "Project Geometry" icon is grayed out, then the sketch isn't associated. This is because Inventor doesn't see any geometry to project. If the sketch is associated it will.
|Two ways to tell if the sketch isn't associated|
For a little extra info, here is the video!