Participate in Assembly and Drawing Sections

[Anonymous]

I've got a spherical roller bearing, inserted
from the Content Center as a custom part (i.e., it's in the project's folder,
not the CC folder, so it's modifiable).  The Modeling tab of the bearing's
Document Settings has "Participate in Assembly and Drawing Sections"
checked.  It's placed into an assembly with a shaft, bearing housing, etc.,
the assembly is in a half-section view, but yet the bearing does not get
sectioned.  The entire bearing is visible.  I must be losing my
mind.

Inventor 2009 Pro SP2.

brian r.
iwaskewycz

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">inventor
specialist

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">core furnace
systems

[Anonymous]

Have you checked Application Options > Drawing
tab > Section Standard Parts?

--
Patrick Miller
Autodesk Manufacturing Industry
Group
Technical Publications - Subject Matter Expert
Novi, MI

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"brian r. iwaskewycz" <
href="mailto:biwaskewycz@REMOVETHIS.corefurnace.com">biwaskewycz@REMOVETHIS.corefurnace.com>
wrote in message
href="news:6179705@discussion.autodesk.com">news:6179705@discussion.autodesk.com...

I've got a spherical roller bearing, inserted
from the Content Center as a custom part (i.e., it's in the project's folder,
not the CC folder, so it's modifiable).  The Modeling tab of the
bearing's Document Settings has "Participate in Assembly and Drawing Sections"
checked.  It's placed into an assembly with a shaft, bearing housing,
etc., the assembly is in a half-section view, but yet the bearing does not get
sectioned.  The entire bearing is visible.  I must be losing my
mind.

Inventor 2009 Pro SP2.

brian
r. iwaskewycz

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">inventor
specialist

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">
style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">core furnace
systems

[HallStevenson]

I've never thought to look at the setting you refer to but hate to think that this is the root of the problem. That is, ALL content center parts by default do NOT have this option checked.

Checking "Section All Parts" on the Assembly tab of the Application Options doesn't help either.

I have to ask (someone from Autodesk):

What is the logic in not sectioning CC parts ? Why are they any different ? I can understand the "you can't modify CC parts (easily)", but sectioning them is NOT modifying them. It's a view of them.

[Anonymous]

This isn't a drawing, Patrick.  It's an
assembly.

brian r.
iwaskewycz

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">inventor
specialist

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">core furnace
systems

[Anonymous]

Oops, my bad. I focused right in on the "drawing"
part of the option. Did the "Application Options > Assembly tab > Section
all parts" fix this (that Hall mentioned)?

--
Patrick Miller
Autodesk
Manufacturing Industry Group
Technical Publications - Subject Matter
Expert
Novi, MI

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"brian r. iwaskewycz" <
href="mailto:biwaskewycz@REMOVETHIS.corefurnace.com">biwaskewycz@REMOVETHIS.corefurnace.com>
wrote in message
href="news:6179953@discussion.autodesk.com">news:6179953@discussion.autodesk.com...

This isn't a drawing, Patrick.  It's an
assembly.

brian
r. iwaskewycz

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">inventor
specialist

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">
style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">core furnace
systems

[Anonymous]

With "Section All Parts" checked, yes, the
bearing appears sectioned, but so does the shaft, which, by standard drafting
convention, should NOT participate in the section.

brian r.
iwaskewycz

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">inventor
specialist

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">core furnace
systems

[HallStevenson]

It's not a "shaft" to Inventor, it's just another part.

[HallStevenson]

> {quote:title=Guest wrote:}{quote}
>

>
>

Oops, my bad. I focused right in on the "drawing"
> part of the option. Did the "Application Options > Assembly tab > Section
> all parts" fix this (that Hall mentioned)?

>

Patrick, having that checked does not, in my experience, have any implications to IDWs or drawings. From your earlier post, you pointed to the "Document Settings" option for sectioning a part in a drawing. Is that what controls it ? If so, that's a huge mistake. Users shouldn't, and typically can't, edit CC parts. I realize that you're not actually changing the model, but I'm positive that Inventor is going to see turning this on as a change and prompt you to save it. Regardless, I do NOT open CC parts individually.

[Anonymous]

I seemed to have confused things more when I zeroed
in on drawings. For drawing section views, you can use the application option
for all or none, OR set it to browser and use the drawing browser on an
individual occurrence basis. This eliminates the need to edit the CC part
file (doc settings). Where the doc setting is beneficial is if you always want
that part to participate you can set that once instead of using the browser on
each occurrence.

What I now understand Brian's question to
be is: in an assembly section view, can you have a CC
part participate and a regular part not participate? I, too, am finding the
answer to that to be "no" but will research further to see if there is a way or
if I need to log a wish.

Enjoy the weekend!

--
Patrick Miller
Autodesk Manufacturing Industry
Group
Technical Publications - Subject Matter Expert
Novi, MI

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<HallStevenson> wrote in message
href="news:6180056@discussion.autodesk.com">news:6180056@discussion.autodesk.com...

>
{quote:title=Guest wrote:}{quote} >

> >

Oops, my bad. I focused right in on the "drawing"
> part of the option. Did the "Application Options > Assembly tab >
Section > all parts" fix this (that Hall mentioned)?

>

Patrick, having that checked does not, in my experience, have any
implications to IDWs or drawings. From your earlier post, you pointed to the
"Document Settings" option for sectioning a part in a drawing. Is that what
controls it ? If so, that's a huge mistake. Users shouldn't, and typically
can't, edit CC parts. I realize that you're not actually changing the model,
but I'm positive that Inventor is going to see turning this on as a change and
prompt you to save it. Regardless, I do NOT open CC parts
individually.

[Paul.Normand]

Hi Brian,

Doing some checking. Hope to have an answer for you sometime early next week.

Regards,

Paul Normand (Autodesk)

[HallStevenson]

I'll have to add that to the settings/options adjustment to make on everyone's machine. I always added the checkbox for the "Section all parts" option, but miss the other one. I've seen it, but forgot about it.

[Anonymous]

or not...

brian r.
iwaskewycz

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">inventor
specialist

style="FONT-SIZE: 14pt; FONT-FAMILY: Verdana">
title="http://www.corefurnace.com/ CTRL + Click to follow link"
href="http://www.corefurnace.com/"...

[Paul.Normand]

Sorry for the delay, but I suspect that this is the behavior of content center parts that are initially flagged for no section.

I got the same results that you did when I tested this workflow so I sent an email to the developers. They said they would have an answer for me within a day (on Monday). Today is Friday and still no word. I sent them another request for an update on the issue.

I am hoping they have a suggestion for a work around. I will let you know what they have to say as soon as they respond.

Regards,

Paul

[Paul.Normand]

Hi Brian,



I am working on finding out what is causing the behavior we are observing. Turns out it is a more complex issue than it seems. Thanks for bringing it to our attention!



In the meantime here are a couple of work arounds that will get you the section view you require:



Save the part out as a STEP (or SAT) file and then import it as a replacement for the original. The section view works as expected.



If you are using Inventor 2010, you can use the following workflow without exporting:



1. Start an empty part file.

2. Exit the sketch and then use the Derive command to import the Content Center component into the new part file.

3. Replace the original component in the assembly with the derived part.



The section view works as expected.



If you have 2010 this workflow might be preferred because it maintains the link to the original and can also import iMates and Work geometry.



Regards,



Paul Normand (Autodesk) Edited by: Paul.Normand on May 18, 2009 8:05 AM

[alexander.room]

Inventor 2012

Assembly

Combining two assemblies into a larger assembly.

Dear all,

I understand that this thread is a bit old, but I am having an issue associated with this.

Working in an assembly I am trying to section specific parts only.

The core problem is that in: Tools - Document Settings - Modelling Tab -  the 'Participate in assembly and drawing section' is not visible?

Any ideas how I can get it back?

Thanks

Alex