Balloon command not recognising .ipn part in .idw views.

Isoma_Tom · ‎08-08-2016

Hi all, this is my first post so sorry if I miss anything. I've got an '.idw' spares drawing which contains an assembly view and several exploded views.

The problem is with the balloon command not recognising parts in several of the exploded 'ipn' views. The balloons recognise one shaft washer but not the other shaft washer in the same view (identical parts). The same occurs in the other view where some parts are recognised but identical parts in the same view are not (bearings and sprockets this time). I've tried deleting/redoing views and parts, updating the drawing, turn it off and on but to no avail.

I'm currently using Autodesk inventor 2016, windows 7 pro 64-bit operating system.

Sofia.Xanthopoulou · ‎08-25-2016

Hi @Isoma_Tom,

and welcome to the Community

Well, that is not supposed to happen, when you balloon same parts. I have tried to recreate what you explained here, but failed. Failed means in this case that I had no issues with the balloons.

Two things:

if the dataset is not too big, can you upload it here? Or create a smaller one where this issue happens
Is your software fully patched? You can check this on this download site.

Looking forward to your response

Regards

-----------------------------
Please accept as solution if my post fully resolves your issue, or reply with additional details if the problem persists.

Sofia.Xanthopoulou · ‎09-05-2016

Hi @Isoma_Tom,

it would be nice to hear from you again. Without any feedback from you I will not be able to assist you

Looking forward to hearing from you...

Regards

Daniel248 · ‎09-05-2016

Could be the same problem I had before - have a look at this thread

Sofia.Xanthopoulou · ‎09-16-2016

Thanks for this input @Daniel248,

I don't think he is talking about this. His issue is not view related. Claimed that in the same view identical parts are not recognized as such.

But if @Isoma_Tom does not come back to his thread - unfortunately we will never know.

Regards

Sofia.Xanthopoulou · ‎09-26-2016

Hi @Isoma_Tom,

any chance that we get a feedback here If you still facing any issues all posters/readers here, including me, would be more than happy to support you.

In case everything work fine, please mark an accepted solution or tell us what solved your problem, so all readers can benefit from your experience.

Thank you

hncarle · ‎09-26-2016

Probably not the problem but I have had balloon not recognize parts in the past and digging a little found out the parts were Phantom.

Sofia.Xanthopoulou · ‎09-26-2016

Aha! So, when those parts are not on Phantom, they are working fine with the balloons?

If so, please mark your post as accepted solution, so that other readers can benefit from your experience.

Thanks

SBix26 · ‎09-26-2016

The OP (original poster) posted the question and never came back-- only one post from that login.

Another possibility is parts set as reference, which would account for different results for different occurrences of the same part.

Sam B

Inventor Professional 2017 R2
Vault Basic 2017
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

hncarle · ‎09-26-2016

If a part is reference in the drawing it would show up as a shadow. The original poster didn't mention that the parts were shadows.

SBix26 · ‎09-27-2016

@hncarle wrote:

If a part is reference in the drawing it would show up as a shadow. The original poster didn't mention that the parts were shadows.

Not necessarily-- you can set options in your view(s) to make reference parts look exactly like any other part.

Sam B

Inventor Professional 2017 R2
Vault Basic 2017
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

Sofia.Xanthopoulou · ‎09-28-2016

Hi guys,

as the OP does not come back to this I will try to give a possible explanation for all readers, how to run into this situation.

Taking all your thoughts together....(and thank you for this )

If ballooning does not recognize one part, let it be one single part or a copy of another component, you probably made some crucial changes.

Watch the steps:

pic 1 : highlighted part not recognized

pic 2 : BOM structure in .iam on reference

pic 3 : display referenced component as Part - Margin 1

The result is that this part, although displayed as a regular part, will not be recognized.

I hope this helps.

Regards

SBix26 · ‎09-28-2016

Hi, Sofia,

Also need to select Hidden Line Calculation > All Bodies-- this, along with the linestyle As Part makes the reference parts look exactly the same as normal parts.

Sam B

Inventor Professional 2017 R2
Vault Basic 2017
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

Sofia.Xanthopoulou · ‎09-28-2016

Little details make the difference...

Thanks a lot @SBix26 - pictures changed

Regards

Anonymous · ‎09-26-2021

Hello

It seems there is a solution to this probelm.

First of all, make sure your target part is set in BOM Structure : Normal ( not in phantom; not in reference)

go to edit view.

select the tab: dispaly option

check the option : interference edges.

now, you target part will be visible in continous line type.

click balloon icon from Annotate pull down menu.

now you should be able to select the target part and do the ballooning.

hope this helps.

Regards,

Babu Raj