Inventor

Attach Documentation in Autodesk Inventor

30 Apr, 2013 By: Mark Flayler

IMAGINiT Tricks Tutorial: Manage your views correctly, and they'll move with your geometry when the design is updated.


Editor's Note: This tutorial courtesy of IMAGINiT Technologies.


I'm sure this has happened to you at one point or another when documenting with Autodesk Inventor. You start placing Base and Projected views and then maybe a Section, the occasional Broken View, and then your Detail views. Design changes happen, documents update. Somewhere it's 5:00 and everyone else is getting off work on time — but not you, because you have to fix those Detail, Section, and Break Out views that didn't move with your geometry when the design updated and changed. So how do we get out of work sooner and with fewer headaches next time? By making logical attachments to our views, that’s how.

Attach Detail Views to Geometry

When you place a Detail view in the drawing manager, you can move it around if you don't like its initial placement on your view.



This flexibility is also the reason why the detail may not move with the update when a design updates. This can cause incorrect dimensions, as well as those pink orphaned dimensions we hate to see.



The next time you place your Detail view, take an extra step and attach it to some geometry. This will essentially anchor it to a point so when it updates in the model the corresponding detail attached to it will also move in conjunction with it. Simply right-click on the center green dot of your detail boundary on your view, select Attach, and choose the geometry you'd like to attach to.

 

After our adjustment in the model making this design two inches longer, the detail stays with the geometry we want so our dimensions still show our intended values.




Section Views

Given the nature of our part here, we want to see a sectional view inside it for proper dimensioning.



So we begin with our standard views we want in our drawing and leave room for our section view placement. When you initially start the Section View command, you might feel the urge to just draw a line a haphazardly. However, if you just draw a line in anywhere without regard for where it is referencing, you will have a floating section line that will not be directly tied to geometry. Just like our last detail attachments, the section view will not update intelligently based on changes made to the initial geometry.



With that in mind, how can we properly create a section line for our view? There are a couple of ways. The first is to watch closely when referencing geometry for the line; another is to use a Sketch on the View to distinctly locate the view.

Method 1: Don't click with abandon. When you are starting the section view command, carefully hover over midpoints and center points (don't click on them) and use Point Tracking to better reference where you are with a section line. While you are not actually creating a Sketch directly here, it is actually doing just that and creating coincident constraints on your hovered references. Once the section line is created, you can right-click on the section view line and choose Edit to see just that.



This works great when you are going right through something where you can use a Midpoint or a Center point of an object. As you can see from the original intent for our documentation, this is not what we want to get our desired section view of the part.

 

Method 2: Be methodical. First select the view with your mouse, then choose the Create Sketch command in your Place Views tab of the ribbon. This will start a new sketch just on the view of the part. If you do not select your View first then the sketch will be on the entire sheet of the paper and your section view command will not be able to select the line you are about to draw. Just make sure your view has its extents highlighted before you select the button.



From here, use Project Geometry and Dimensions to properly locate the section line where you want it to fall in the geometry. Keep in mind that it will update based on the change to the model geometry as well — do not attach it to geometry you know will be destroyed or drastically changed or shifted.



You could also consider using a Work Plane and projecting that if you can't decide on good reference geometry to project in the view. You can include Work Features in a drawing view by right-clicking on the referenced file in your view in the Model Browser. Of course, you can still use the haphazard method and use the Edit option on the section line to fix your quick placement with the sketch tools, but I just prefer the upfront methodical way.

Break Out Views

This type of view in the Drawing Manager is a very easy one to mess up when you first start using the software. In fact, it's downright confusing until you know exactly what the command wants to operate. The proper way to start a Broken view is not to start the command first, but to do something similar to the sectioning method previously discussed by first placing a sketch on the view for location of the broken boundary for the view. If you don’t do this step first you will get the error message shown below.



After sketching the correct boundary on the view with a sketch, you have full control now to create your Broken view. One of my favorite usages of this tool is to break a standard orthogonal view, then project it to get some nice revealing geometry. Of course this view is more commonly used on assembly views to see behind walls and other obscuring geometry, but Broken view is pretty versatile.


About the Author: Mark Flayler

Mark Flayler

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