Inventor General Discussion

Inventor General Discussion

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Valued Contributor
Scott_Stubbington
Posts: 85
Registered: ‎02-03-2004
Message 1 of 4 (441 Views)

Drawings - "Break" view and Parametric parts

441 Views, 3 Replies
10-25-2012 08:48 AM

Hello, :-)

I have a paramtric assembly and some of the parts in this assembly require a "Break".  When the part dramatically reduces in size the part view disappears as the part is now located in the "Break".  Delete the "Break", re apply the "Break" fixes the problem, however this is a little frustrating.

I would like to be able to constrain a Break to the part, either a sketch on the view or maybe from Workplanes in the part.

 

Thanks

 

Scott :-)

*Expert Elite*
Cadmanto
Posts: 3,356
Registered: ‎12-07-2011
Message 2 of 4 (429 Views)

Re: Drawings - "Break" view and Parametric parts

10-25-2012 11:40 AM in reply to: Scott_Stubbington

Scott,

What version and SP are you running of Inventor?

What I would like to know is, why are the parts dramtically changing in size?

If you have a scale specified for the drawing view, and your sketch is constrained to the view

I am not getting what exactly you are talking about.

Can you provide some images as well?

Best Regards,
Scott McFadden
Inventor Professional 2014
(Colossians 3:23-25)

Valued Contributor
Scott_Stubbington
Posts: 85
Registered: ‎02-03-2004
Message 3 of 4 (421 Views)

Re: Drawings - "Break" view and Parametric parts

10-25-2012 12:57 PM in reply to: Cadmanto

Hello Scott,

Inventor 2013, SP not installed yet....

 

I cannot provides images this week as I'm at home.  I will next week.

 

Imagine you have a pipe, cut into the pipe are a load of holes.  The pipe is 6m long, 0.5m each end is clear of holes, then the middle 5m of the pipe there is a hole every 200mm.  I have a section through a hole to define the hole detail. I have a "Break" on the viewfrom 1m to 5m leaving 1m of pipe each end showing.  Some person tweaks the assembly and the pipe is now only 3m long, 4m of the original view is "Break" view which now completely covers the tweaked pipe and I have to "sigh" redo the views.

 

I hope that helps

 

Thanks

 

Scott  

*Expert Elite*
cwhetten
Posts: 1,090
Registered: ‎09-03-2008
Message 4 of 4 (415 Views)

Re: Drawings - "Break" view and Parametric parts

10-25-2012 01:26 PM in reply to: Scott_Stubbington

Unfortunately, there is no way to directly constrain a break view.  This ability has been requested for a while now, but...

 

If a break view is a must (as it is for some of our drawings), there is a workaround.  What we do is outlined below:

 

1. Place the base view of the model.

2. Create a breakout view (which is defined by a sketch attached to the view, and this sketch can be constrained to model geometry) that takes out the middle portion of the view that we don't want to show.

3. Create detail views of each end of the base view.  This allows us to control the spacing between the views, and ensures that the views will not jump off the page when the model gets longer/shorter.  Be sure to attach the detail view to an area of the model that will not move relative to your break edge.

4. Align the detail views to each other.

5. Add a sketch or sketched symbol for the break line.

6. Move the base view off the printable area (or suppress the view), as it is only used for building the other views.  This view will get longer and shorter as the model changes, so it isn't useful as a real drawing view.

 

It's a lot of extra work for something that Inventor should just do for me, but like I said, it's a workaround.  So far it has served us well.

 

Edit: If you like, I can post a simple example of this when I get some time.

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