Model from ContentCenter after Refresh get's a hatch in drawings section

[MarkusGreifeneder3360]

Hi!

Usually the Inventor-drawing recognizes (in a section of an assembly) a ContentCenter-Part and does no section (no hatch).

After "Refresh standard components" with the designated Inventor command this "automatism" is gone.

We have a customized CC (with our partnumbers and some other information in the customproperties), and only edited some customproperties. (no model geometry).

Is this a known issue?

Did we do something wrong?

How to fix this issue?

I attached the files for testing.

[Mark.Lancaster]

@MarkusGreifeneder3360

When posting and sharing files, its important to indicate what version of Inventor you're using.  Not everyone has the same version as you..    In your case these files are Inventor 2016.

Are both CC parts standard or were they placed as custom?

[MarkusGreifeneder3360]

Hi Mark,

Yes, we use Inventor 2016.

Both files were placed as "As Standard", but one was refreshed afterwards.

[Anonymous]

[Mark.Lancaster]

@MarkusGreifeneder3360

I'm seeing the same results in Inventor 2018.2.3.  When I reviewing the drawing browser structure, that given CC component is selected to participate in the section.  Not sure why that's defaulting that way when the settings are the same for both CC.

@Anonymous

In this case, one of the CC standard component is being sectioned, while the others are not.

[smilinger]

It's really a myth to me why and how inventor decides to section these standard parts. I think this is a bug and should be reported to Autodesk.

@viktor.bednarik, @johnsonshiue

There is a workaround, it's a little complicated:

1. Save a member of the standard part As Custom instead of As Standard.
2. Open the part, unselect the option "Paticipate in Assembly and Drawing Sections" in the Modeling tab of Document Settings, save.
3. Select the family in Content Center Editor, right click and select "Replace Family Template" and select the part as replace.

[johnsonshiue]

Hi! I could be wrong but I think the CC part was published with "Participate in Assembly and Drawing Sections" checked. Then the behavior seems as designed to me. You may want to replace the family template associated with the particular CC family.

Many thanks!

[smilinger]

@johnsonshiue, I am also aware that the CC parts was published with "Participate in Assembly and Drawing Sections" checked. Then where is the magic switch on the part that inventor use to decide NOT to section the OOTB standard parts, and why is the magic disappear after content center editing? Is that the way how Autodesk say OOTB standard parts are superior and content center editing sucks?

Or, why is it designed this way? That does not sound right to me, and ask the user to replace family template for EVERY edited content family is just absurd.

[johnsonshiue]

Hi! I am an engineer, not a politician. I am trying to help here. Let's focus on the issue. For any given component, Inventor determines if it participates in sectioning based on an option in Document Setting. Go to Tools -> Document Settings -> Modeling. You will see the check box "Participate in Assembly and Drawing Section."

I checked the two parts you attached here. The option is checked. This is why I said the behavior was designed. Purely based on the files, I cannot tell when and why the option is checked. It is possible when the part was published, the option was already checked (on by default in Standard.ipt). Or, it was checked afterwards.

If you don't want the option checked, there are two ways to do that. You can find the original source iPart and make sure option is unchecked. Then re-publish it to Content Center. Or, you can use the template replacement workflow in the following page.

https://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/2017/ENU/Inventor-Help/files/G...

Many thanks!

[smilinger]

I think you didn't get the point here.

The point here is, why the OOTB standard parts have that option checked and however ARE NOT SECTIONED, and edited content center parts ALSO have that option checked BUT ARE SECTIONED! Why the different behavior?

[johnsonshiue]

Hi! I am sorry I think I got mixed up. What is OOTB library? Could you provide an example showing the unreasonable behaviors you are talking about? It does not sound right to me.

Many thanks!

[Mark.Lancaster]

@smilinger

I think what @johnsonshiue is stating..  We don't know when that option (document settings) was changed.  Before it was published to CC or after CC (family template has been updated).  Sometimes when things are changed after it was published to CC and the family template is updated, certain things may not really take. I've seen this a few times and this may be the case (or perhaps not).  Or its just a fluke..   

[smilinger]

I mean the out-of-the-box content center library. The standard parts from the ootb library are not sectioned in the drawing. If you copy the family to a custom library, edit the family, add/remove/edit some columns in it, then the new standard parts generated will be sectioned.

[Mark.Lancaster]

@smilinger

I'm wondering if this is the reason...  Content Center was introduced so many years ago and really hasn't changed (It came from another source)..  So that info (OOTB) cannot be edited, so I'm wondering when the information gets generated, it really doesn't consider that participation in drawing section view option (since that option was introduced as some point after the implementation of CC).  But when you create your own library, the information is really generated as new..  Anyhow my 2 cents.

Nope I just proved that's not the case (never mind what I said )..  However @smilinger I never really sectioned my CC parts in the past so I placed a component from my read-write library and it still doesn't section it.

[smilinger]

@Mark.Lancaster, I also did more test and I am also confused, it seems it will be sectioned only when using the Refresh command. If you place a standard part from content center it will not be sectioned, if you edited the library and refresh, it will be sectioned.

[Mark.Lancaster]

I need to stop working on this stuff late at night..    Here's what I found..

My application options, drawing tab states to obey browser for sectioning standard parts.

I created an assembly that I placed a hex nut, the larger one from my read/write CC and the smaller hex nut for a read only CC library.  I then placed the two cc hardware attached by the OP and look what happens (it doesn't sectioned)

  I created another simple assembly with the 2 content centers attached by the OP.  The first component in the browser is the smaller screw that's being sectioned.  Why now?

Also after I made different assemblies using different combos of these CC components, the smaller hardware from the OP is still being sectioned.

[johnsonshiue]

Hi Guys,

The behaviors are indeed confusing. Let me take a closer look tomorrow and I will report back my findings.

Many thanks!

[Mark.Lancaster]

@johnsonshiue

This is really getting confusing..

So this morning (Inventor was open all night), I created a new Inventor drawing using the assembly that had the 2 hex nuts and the OP hardware and guess what? The screw is now hatched in the new drawing.

[johnsonshiue]

Hi Guys,

I think I may have found the behavioral pattern now. The option "Participate in Assembly and Drawing Section" option has an interesting behavioral model.

When the option is checked, the followings will happen in the drawing.

1) The part (regardless of CC or not) will be sectioned in a part drawing view by default. You will need to change the Section Participation option in the drawing manually.

2) If the part is in an assembly, the assembly drawing view will honor the browser default (Obey Browser). All CC parts are not sectioned by default regardless of the option.

When the option is unchecked, the followings will happen in the drawing.

1) Above #1 behavior applies here too.

2) If the part is in an assembly, the assembly drawing view will honor the browser default and exclude the part from section view. Changing the option will trigger a change in Section Participation in the drawing.

In the assembly, the virtual section view behavior is much more straight forward. All CC parts are excluded from sectioning regardless of the option. Non-CC parts will depend on the option.

In the part itself, the virtual section view behavior totally depends on the option. When it is on, it can be sectioned and vice versa.

I have to say it is indeed confusing since the behaviors can vary in different document types and different sectioning operations. I hope my explanation makes sense and it is consistent with what you are seeing.

Many thanks!

[smilinger]

The option behavior is actually logical and reasonable, albeit a little confusing sometimes. What caused the initial confusion of OP and this whole thread is the Refresh behavior of the Content Center. What I am talking about is this:

As I said above, the default behavior of CC parts is NEVER sectioned in assembly or assembly drawing, however, if the CC parts are REFRESHED, then the CC parts will be sectioned in assembly or drawing.

That screw from OP is apparently a refreshed CC part, so it gets sectioned and cause more confusion to @Mark.Lancaster.

The steps to reproduce this issue:

1. Place a CC part As Standard from a customized CC library.

2. Check the assembly and drawing to confirm it's not sectioned.

3. Edit the family table of the CC part in CC editor, Add a new column to the table, and map the column to some iProperty.

4. In the assembly containing the old CC part with virtual section turning on, click the Refresh command, refresh the CC part.

5. Now check the result, the refreshed CC part is sectioned.

6. Place a new member of the family, the new part is not sectioned.