In 2013 idw the section depth is ignored for frame generator members, so that they show up even if they are outside the section depth.
Can we have a hot fix please.
Did you change the setting for "Section Standard Parts" in your view editor? I would agree this part should not be there, and maybe it is a bug... not sure. But you should be able to make it go away with these settings. One of the choices is never.
I cannot say from your picture what's a problem yet. But I'm thinking about one issue which I think wasn't fixed in 2013. So I have questions:
1) Is there any break in the view?
2) Is the distance of the section limit line from the section line approriate to Distance value 50?
3) Can you post the 'same' image with Distance value set to 1?
The best would be if you can send me the dataset to ladislav.pcola(at)autodesk.com
Please find attached a sample assembly showing the problem. Every view in the attached idw is incorrect because idw is having problems with frame members. Its not just limited to sections, even the base views are wrong.
many thanks for the dataset.
I see two issues here:
1) All the views shows a non-existing portion of the Aluminium 100x10 Flat Bar 00000005:1 component
- I'm not sure how this happened. Seems like a model changed but drawing wasn't notified about the change
-- Do you please have some steps to reproduce this issue? Steps would help me a lot to analyse the issue. Thanks
- For now a workaroud is to update the views manually - the issue is gone after updating views on my R2013 SP1.1
2) Second issue is the component Aluminium 40x4 Flat Bar 00000006:1 not sectioned in Section view D-D
- this is actually as designed as the component has set Section Participation to None. So it is included in the section view but without being cut
- to make the component cut please change the Section Participation to Section
-- e.g. by RMB on its Browser Node under D: Section view Node
Thanks for your reponse
1. The model was created in 2013 SP1.1. The model didnt have any changes. All I did was place the FG member on the edge of the plate. It looks like it is extending it to the limit of the view rather than the length of the edge.
2. So it seems that FG members are set as default to not participate in sections. We have far too many to manually change each one. How can I set the default for FG members to be included in sections.
I just went to dosome more testing this morning. The drawing looked ok, so teh views updated after restart, so I added a new FG member and have a similar problem, but can not find a way to update the view to fix it. Even completely exiting Inventor and opening again wont allow it. Will try a full machine reboot and see what happens. No luck, even after full shut down the drawing is the same.
thanks for all the information - I'll try to reproduce the issue today.
Regarding your questions:
1) To update all views just select all three views in the browser and press update
2) To allow all FG components sectionable in a view please RMB -> Edit the view; Switch to Display Options tab and change the Section Standard Parts to "Always"
- you'd need to do that for all the created views
3) To change the default of the option for new views you need to change it in Application Options -> Drawing tab -> Section Standard Parts
I hope this helps
Thanks, I didnt realise FG members were treated as standard components like nuts and bolts, I thought they we treated as parts, so that has fixed the sectioning problems, but the incorrect views are still there and refrshing the view does not fix it.
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