How to make the a part section view show more of the full part

[bgough]

Hello, trying to create a section view of a part detail (embossment).  I want the section view to show more of the full part, not just stop at the edges of the part detail.  How do I grow the section view to make it wider?  See attached picture that may help explain my challenge.

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[sundars]

Hi @bgough 

Right now your section line stops at the two ends of the slot. So, the resulting section view bounds align with the ends of the section line. If you make the section line bigger then you should be able to cut more of the parent component and get a bigger section view. See if you can drag on the ends of the section line and make it bigger.

See image below:

Hope that helps.

-shiva

[bgough]

Thank you for the information.  It appears that when I drag the section line out, it doesn't keep it on the centerline of the embossment.  It can be eye-balled to get close, but I am looking to keep it exactly on the centerline so I can pull a key dimension.   If there is not a good solution, then I might be able to get what I need through some sketch dimensioning instead..

[sundars]

Hi @bgough 

You should be able to inference to the ends of the slot/cutout when you select the section. I agree, that sometimes, that can get tricky and not be accurate. You can however, create a view sketch and create a line and dimension it to get it to be perfect. Then right click on that line and issue "create section view". That should do the trick.

Thanks

-shiva

[SBix26]

Creating a section view automatically creates a view sketch containing the section line(s).  Find that sketch (in the browser under the view you're working with), right click and choose Edit.  Now you're editing the sketch, and you can project geometry from the view and constrain your section line to it, as well as dimension your line however you wish.  Exit the sketch, and the section is updated accordingly.

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Sam B

Inventor Pro 2022.2.1 | Windows 10 Home 21H2

[James_Willo · Accepted solution]

To add to what Sam has said, if when creating the section you have snapped it to geometry, it is sometimes necessary to remove the constraints when in 'edit' mode for the section line so that you can drag the ends of the line. You would then need to reapply constraints to get it back on the centre of the slot. 

From what you said it sounds the ends were not constrained.