After Sectioning an assembly in the .idw, missing parts/objects was noticed.

[WillieArolf]

Hi guys/gals,

I have yet another query to ask. I have created an assembly with standards parts and objects mainly;

1. Valve with Actuator

2. Stud Bolts with Nut

3. Angle bar

4. Objects (Clamps)

I wanted to show an ISOMETRIC cross sectional view of the said assembly. I noticed after doing it so, that there were missing standard parts/objects.

How do I make them visible on the cross section ISOMETRIC view?

Appreciate once again any help. 🙂

[Mark_Wigan]

hi Wille,

   i apologise if you have already checked this but can we just quickly check if those items are actually visible regardless of whether they are sectioned or not?

maybe when the views were created they were set to be associative to a particular view representation in the model at the time?

as you may be aware, occasionally when working in assemblies with lots of fasteners and other items that get in the way, it is handy to hide them, so it may be that you need to edit an existing, or, make a new view rep in the assembly that is showing all parts and ensure that the good view rep is what the view is looking at when you get back to the idw (view).

the reason i mention this is that there are settings to section or not section standard parts (as well as the ones you highlighted in the browser) but your invisible parts seem to be a mix of various items, some std, some not ( ie not out of content center etc). yours seems kind of a random mix of visible and non  visible parts so it doesn't make much sense looking through those settings if that is the case.

[WillieArolf]

Hi Mark,

Firstly, let me say thank you for the immediate responce to my query. I apologies if it tooked me this time to reply. It was holiday here in Singapore so we went out of the country for a while.

Anyway,  I cannot attach the zip file as it is a bit big 8.57MB and we are only allowed to attach 1.5 per file so I just put it in yousendit for a while for you to download the files.

https://www.yousendit.com/download/WUJZdFdXSys1bmc4RmNUQw

One more thing I just noticed. On the idw, Place a View > Base > Orientation > Top then, section it. On the tree view of the sectioned view 1 part was missing "Top Side Clamp 1". But, on the original Top view all the part was there. No Idea what happen.

[Mark_Wigan]

hi Willie i loaded this up into 2012 tonight.

and from what i can tell we are unable to fix this issue by changing any of the available settings.

i loaded up your assembly and made some new views. they behaved exactly like you explained. actually i did a few other views and saw a few other issues like the cabinet not being sectioned at times depending on the projection of the views.

i changed various view / section settings in the browser as you also did, also in the application options and view options also to no avail.

it seems like the assembly or several of the parts are now corrupt for some reason. i have never seen an issue like this that was unable to be fixed.

i even ran a macro that did a few years ago to make a content centre part into a normal part. this did not make any difference to the views either.

ps- some years ago there was a bug that appeared on rare occasions. when detailing in the idw, one of the ortho views was entirely invisible for no reason. the only way to fix it was to systematicaly go through the entire assembly and delete one part or assembly at a time until the view came good. i actually thought this may be a new bug variation however i was unable to fix the issue by systematically deleting likely candidates as in the other bug i referred to. it was a bit of a long shot but without anything else i could think of it was worth a try i guess.

the clamp (and many other parts) appear to have originally been generated from a solid non-inventor part? then derived into the other parts of the clamp and then in one case, one of those is mirrored to form the opposite hand part of the clamp. to me it seems that the inventor cannot crunch this part. it should not be an issue as we all do this from time to time.

so considering that the bolts are also not showing up it is a bit of a mystery i do not think that re-modelling any individual parts will fix this. (we both tried changing the section standard parts options and obey browser settings makes no difference as mentioned above and from wha tyou saw yourself).

tomorrow if i get time i will load it up into 2013 to try it to see if it behaves the same.

[WillieArolf]

Hi Mark,

Thank you for looking at it.

the clamp (and many other parts) appear to have originally been generated from a solid non-inventor part?

- All of the parts were created in Inventor Product Desing Suite 2012.

then derived into the other parts of the clamp

- Yes, I use the derive feature as a guide in creating the framework.

then in one case, one of those is mirrored to form the opposite hand part of the clamp.

- You are right

I did create all the parts using the multi-solid body feature then, create's part/assembly out of it. Then, make use of the derive feature as a guide to create another part/assembly.

Hopefully, they can create an SP for 2012 as my boss does not want to upgrade to 2013... 😞

[Mark_Wigan]

hi mate,

thanks for the feedback.

i tried it in 2013 as well with no success. & i am still trying to figure this one out...

do you have problems sectioning on other parts / assemblies or is this the first time?

if you made these parts yourself, how did you go about it & is that what you normally do? do you have the original parent part / solid that you started out with?

if you get time can you make another clamp and make an opposite handed derived part of one piece. see if it does the same thing.

sorry for the questions.  i am trying to understand your workflow.

ps - there is a new service pack for inv 2012 out in the last few weeks just in case you haven't scored it yet.

-mark.

[WillieArolf]

Hi Mark,

To answer your queries;

do you have problems sectioning on other parts / assemblies or is this the first time?

If I could remember it in 2010 version I encountered same problem but, I am not to sure what happend next. I forgot already.

if you made these parts yourself, how did you go about it & is that what you normally do? do you have the original parent part / solid that you started out with?

On the zip file that I have saved on a web cloud yousendit all the files were in there.

Step that I did for creating a Clamp:

1. Created a sketch > derived the Valve with Actuator assembly > then extrude make holes and mirrored on a solid. I did make use of the multi solid body in a single sketch.

2. I then invoke the "Make Components" feature. Parts and an assembly were created.

3. Then "Place" the created assembly into another assembly.

if you get time can you make another clamp and make an opposite handed derived part of one piece. see if it does the same thing.

Sure, I will give it a try. and will let you know.

[okaleja]

Hello,

Currently, when creating section view, all parts fully residing in "removed" zone are removed as well. Doesn't matter what's the setting of the Section Participation. Therefore you are not seeing all the parts in the section view or projected view of the section.

Parts which would be partially cut, are present since the Section Participation setting is set to None.

I have logged an issue (DID 1479115) for this topic to our internal database so people from product design can take a look.

Thanks for reporting this issue!

Oto Kaleja

Autodesk

[WillieArolf]

Hi Oto Kaleja,

So it is behaving wrongly then, as it is not getting the correct response from the Section Settings. Well, at least it is already logged as a defect. Thanks.

BTW, even if creating a simpe object ang put in bolts, washer & nuts after sectioning with settings set to none the standard parts are not showned.

Hopefully, an SP for these issue will be created soon.