
A plane on which you want to sketch may be hidden inside a cavity or obscured by other components.	Use a plane or work plane to slice away a portion of a model temporarily, and then create a sketch on the plane.	Create sketch geometry and define features on the sketch plane in the cross section view.

What section views are available?

Section View has these options:

Quarter section view: Select two perpendicular planes. The three-quarter section facing you is removed.
Half section: Select a plane. The half-section facing you is removed.
Three-quarter section: Select two perpendicular planes. The quarter section facing you is removed.
Unsectioned restores the view to the whole assembly.

After you have selected a section view, you can right-click and select Flip to cycle through available views. Quarter and three-quarter views can show the opposite view.

To move a section plane, right-click and select Virtual Movement Section Plane 1 (or Section Plane 2). Then drag the section plane, set its offset, or rotate the mouse wheel.

NoteBoth the quarter or three-quarter section view allow selection of any two planes, not just perpendicular planes. You can define the type of section cut and display sectional slices, if desired.

What is the workflow for modeling in a section view?

Determine if you want to section standard parts in the assembly. By default standard parts are not sectioned, but if desired, select the Section Standard Parts check box on the Assembly tab of Application Options dialog box.
Determine which section view to use, making sure that the planes you must use is visible.
Insert a new component or activate an existing component.
Sketch on the exposed face of the section, projecting geometry to the sketch plane as needed.
Use sketch and feature commands to create or modify a component.

To create a component when viewing a section cut, you select the plane used to define the cut as the sketch plane. You cannot select the cut face of a section cut.

NoteYou can control the visibility of a selected component by using options on the context menu. Clear the check mark on Visibility to hide a component. Likewise, clear the check mark on Enabled to disable a component and display it in wireframe.

Can in-place editing be used with slice graphics?

You can use assembly Section View to view an assembly or subassembly in cross-section, and then activate an individual part. With the assembly sectioned as you specify (quarter, half, or three-quarter), you can activate a part, and then use Slice Graphics to slice away a portion of the active part so that you can work on an obscured sketch plane.

Procedures

Create assembly section views

Create a section view to visualize portions of an assembly within chambers or obscured by components. While the assembly is sectioned, use part and assembly commands to create or modify parts in the assembly context.

To begin, open an assembly file containing one or more components.

If appropriate, specify if you want to section standard parts in the assembly. Click OptionsAssembly tab. Select the Section All Parts check box.
Set visibility for components. Select the component in the graphics window or the browser, then:
- To hide components, right-click and clear the check mark beside Visibility.
- To show components in wireframe for context, right-click and clear the check mark beside Enabled.

On the View tab, Appearance panel, click one of the Section View commands, then select any planar or work plane to define the cutting plane.

	Creates Quarter section view.
	Creates Half section view.
	Creates Three-Quarter section view.
	Sets assembly to no section view.
NoteFrom Quarter section and Three-quarter section views, you can right-click and select the opposite view.

Right-click and select Flip, if necessary, to display the desired view of the section.
To move a section plane, right-click and select Virtual Movement Section Plane 1 (or Section Plane 2). Then:
- Drag the section plane to the desired position.
- Set offset of the section plane in the Offset dialog box.
- Place the cursor on the Offset dialog box, and rotate the mouse wheel to move the section plane.
  NoteTo edit the mouse wheel scrolling step, right-click and select Virtual Movement Scroll Step Size.
On the ribbon, click Assemble tabComponent panelCreate. When prompted to select a sketch plane, select the plane used to define the section.
If desired, click Sketch tab Draw panel Project Cut Edges to project edges of a part cut by the section plane onto the sketch plane.
Use sketch and feature commands to create new geometry.

Show Me how to move a section plane in a section view

Comments

Comments7

thu-hang.taMon Aug 27, 2012 6:46 amI wanted to move a component while I am in section view so I can see if it will hit another component or not. So I did the section view but as soon as I click 'move' in the assembly bar, the section view disappears. Is there anyway to keep the section view while I am moving parts of my assembly?
paul.normandMon Aug 27, 2012 12:55 pmHi, dragging an underconstrained component (using the mouse to push or pull in the direction of a degree of freedom), or driving a constraint is allowed in an assembly section view. If you are using a different method to check for intereference, such as the Move command, it cancels the section view and restores the full view.

Hope that helps.
Regards, Paul (autodesk)
pquenziTue Sep 11, 2012 9:02 amPaul,
I just installed Inventor 2013 and assembly section views do not work as they did in 2011. In 2011 after I made the section, I could press the escape key and then select parts or measure or perform any other commands while in section view. In 2013 section view is canceled as soon as I try to measure or if I press the escape key. I cannot select any parts while in section view. Is there some setting for this? Thanks. Phil pquenzi@starband.net
pquenziTue Sep 11, 2012 9:17 amPaul,
I found the trick in a discussion group search so I'm good to go. Thanks. Phil pquenzi@starband.net
paul.normandWed Sep 12, 2012 9:33 amHi Phil,

I am assuming that the trick you are referring to is the fact that you have to click OK to complete the section view command before you start to measure. If the solution you found is different, please post it here.

Thanks,
Paul
PesjanWed Nov 21, 2012 10:42 pmIt seems like they added a step in the half section view creation. Whe you have selected the work plane or face, Right click and select "continue". Then right click again and click "Ok". It should now work.
trumpy81Tue Dec 25, 2012 10:53 pmUnless I am mistaken, in 2013 this doesn't work for allowing you to take measurements whilst in a quarterview/halfview etc.. in either assembly or part mode.

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