topic Re: Issue with IDW section views, obey browser vs always in Inventor Forum

Issue with IDW section views, obey browser vs always

Anonymous — Tue, 10 May 2016 19:28:09 GMT

Ok, so for the life of me I do not understand why Autodesk "obey browser" setting for section views do not follow proper drafting rules. In the attached doc, I show the issue I'm having. The green arrows show geometry that I expect to see hiden lines of, as that section view is facing that geometry, and sure enough the section view shows hidden lines for that geometry. But why on earth am i see the geometry of the red arrows in the section view? That slot is ABOVE the section view, not to mention facing the complete opposite direction as the section cut is facing. If you literally cut that tube steel at the section view and look down, you would not see the geometry at the red arrows, yet Inventor shows it. This is very frustrating for me, and confusing for our fabricatiors. Does anyone know why this happens or how to correct it? That's just not proper drafting, plain and simple. So confusing. Thanks in advance.

Ryan

Re: Issue with IDW section views, obey browser vs always

mcgyvr — Tue, 10 May 2016 19:37:27 GMT

Can you post the IDW instead of a picture/word doc?

Re: Issue with IDW section views, obey browser vs always

Mark.Lancaster — Tue, 10 May 2016 19:48:08 GMT

@Anonymous

In addition to @mcgyvr request also include all the files that make up the IDW and always indicate what version of Inventor you're using. Not saying this is the reason but a service pack and/or update could resolve this issue if we knew what version of Inventor you have.

Re: Issue with IDW section views, obey browser vs always

Anonymous — Tue, 10 May 2016 19:53:04 GMT

Sure, here are the files. And i'm using Inventor Pro 2016. Thanks...

Ryan

Re: Issue with IDW section views, obey browser vs always

Mark.Lancaster — Tue, 10 May 2016 20:06:56 GMT

@Anonymous

Not all files are provided.. Missing 16034E1-Item b, 16034E1-Item c, and 16034E1-Item e.ipt. My first suggest would be to upgrade to Inventor 2016 SP2 that was just released yesterday. You are still at the Inventor 2016 RTM version.

However are you on subscription? If so install R2/SP1 and then consider upgrading to the 2016 R3 release. IF you're not on subscription then you need to apply SP1 first to Inventor 2016 in order for SP2 to be installed.

Service Packs and updates can be found here:

Re: Issue with IDW section views, obey browser vs always

Anonymous — Tue, 10 May 2016 20:11:20 GMT

Sorry about that. Also, I am on perpetual license with maintenance subscription.

Re: Issue with IDW section views, obey browser vs always

Anonymous — Tue, 10 May 2016 20:12:01 GMT

Last 2 parts.

Re: Issue with IDW section views, obey browser vs always

mcgyvr — Tue, 10 May 2016 20:23:20 GMT

edit base view... change "section" to "always"..

never will never section.. just show the full part

From help..

Section controls the sectioning of standard parts in the drawing views of assemblies.

Never Standard parts are never sectioned even when the Section Participation property is set as Section.
Always Standard parts are always sectioned even when the Section Participation property is set as None in the browser.
Obey Browser defaults to browser setting. By default, the Section Participation property is set as None for all standard parts.
Tip: To change the Section Participation property, in the browser, expand the drawing view node, and change the setting for specific parts.

Re: Issue with IDW section views, obey browser vs always

jletcher — Tue, 10 May 2016 20:24:47 GMT

Easy fix..

Change priority to part click on part in section change none to section.

Fixed

Re: Issue with IDW section views, obey browser vs always

Mark.Lancaster — Tue, 10 May 2016 20:33:30 GMT

@mcgyvr is way too fast... Beat me to the response...

Update: Or another solution is to save as custom when you pick structural shapes from the content center and then you don't need to worry about those settings (for standard parts).

Re: Issue with IDW section views, obey browser vs always

Anonymous — Tue, 10 May 2016 20:37:16 GMT

Those two solutuions definitely did the trick, thank you very much! But i'm a curious nerd engineer by nature...does anyone know WHY we have to do this? It's like we're forced to overrride poor drafting results from Autodesk. In this case, to show features above the section is simply not correct, that's the entire point of a section view, to cut off things we don't want to see. To even have this oddity be an option (1), and to have that option be the default (2), seems very very very odd to me. Does anyone else seem shocked by this? I spent 15 minutes looking for supressed features simply because in my mind anything below the section line HAD to be there. To show features above the section line (in the opposite direction of the line no less) is just baffling to me. Maybe I'm missing something, or maybe there is some special 3D drafting rule for section views. Just curious. This thing got me all riled up for no reason haha.

Re: Issue with IDW section views, obey browser vs always

Anonymous — Tue, 10 May 2016 20:40:34 GMT

Actually, I do save all CC parts as custom. We take basic structural steel (HSS, L, PL, etc) then add features (holes, etc) to them.

Re: Issue with IDW section views, obey browser vs always

Mark.Lancaster — Tue, 10 May 2016 20:44:12 GMT

For standard/content center parts its designed like that so when I create a section view I have the option to show a bolt, hardware and etc as being sectioned or not included (not sectioned) in the section view.

So your steel member is a standard part from content center so it falls under that rule. Just because you think your drafting standards needs it doesn't mean the next person requires that.

Update: Just saw your reply.. Well there's something about the main vertical piece where Inventor still thinks its a standard part.

Re: Issue with IDW section views, obey browser vs always

swalton — Tue, 10 May 2016 20:48:14 GMT

You can also set this in Tools:Application Options under the Drawing tab. That way it will apply for all drawings. This will control section behavior of Content Center components such as fasteners, structural sections, square and rectanglar tube.