Why can't i balloon certain parts????

[mslosar]

We have run into this situation here a number of times over the years, and presently i have a bad one that's making me mad.

I have a sub-assembly featured in an elevation view. Balloons in that view work just fine. I take a couple detail view of that sub and the balloons work just fine. I take projected views (projecting the top) of the same views, and 2-3 parts in them refuse to allow balloons to be placed on them. It's extremely annoying. I've looked and don't see anything here that says 'oh it's that'...

The subs are phantomed. None of the parts are shown in the assembly BOM as anything other than NORMAL. And these parts balloon just fine in 2-3 other views. The problem is always in these project views.

I wish i could post it, but it's a proprietary structure that I can't publish. Figures...can't every be on a simple who cares piece, right? 

This does not happen all the time, just sometimes. So, recreating it is difficult.

I did delete the drawing bom and redo it which did nothing. I tried doing auto balloon which missed more parts.

[mslosar]

As a follow up. It isn't just balloons...

Exiting the balloon command i can't select the parts in question by part, body, or edges. If i do a select all edges over the whole view, the objects that won't balloon don't highlight at all. They're just being skipped.

[Cadmanto]

See if this link offers a solution for you.

https://knowledge.autodesk.com/support/inventor/troubleshooting/caas/sfdcarticles/sfdcarticles/Not-a...

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020

[mslosar]

Saw that, and no.

I had one Parts List on the drawing and it had no overrides. I deleted it anyhow and redid it and the same thing.

Weird that it only seems to apply to anything taken from the detail. 

I have a top view, which is the base. Can balloon/select the pieces fine.

That top view has a section down the side of the assembly showing the sub. I can balloon/select the parts there, too.

I take a detail of the sub off that section. I can balloon/select the parts here as well.

I projected a top view and 3 parts refuse to recognize. I take a section from the detail recreating the projected view and still can't access the parts.  The only thing i see they have in common is they cross the cut line line from the detail or the parts i section through.

[Cadmanto]

I am wondering if this is a tangent issue.  Have you tried turning on the tangent lines when you edit the view under the display tab?

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020

[thenottakenname]

This might be a case of the oft-overlooked selection priority setting. On the top bar, you'll see a little green square or something similar -- play with those and see if it helps. Picture attached for reference.

Hope this helps!

[mslosar]

No on both counts.

I just check the tangent edges and no difference.

I checked the selection setting right off the bat, run into that before.

It's not that i can't balloon anything, there are 3 objects out of 12 or so in the view that simply refuse to register in any type of selection, not just balloons as it turns out. If i leave it on edge mode and select the whole view, everything gets selected, except those part. They're completely ignored. Ordinarily i'd think the part(s) were messed up somehow, but they work fine in the 3 preceding views.

[johnsonshiue]

Hi! Are these parts Reference Parts or Inseparable Parts? Could you share an example exhibiting the behavior?

Many thanks!

[mslosar]

They're all set as normal parts. I can't post it here as it's proprietary design.

Staring at the structured tab right now, 26 items, all with Bom Structure set to Normal. Some of the parents are set to Phantom so their individual parts are listed in this BOM. Nothing is Inseperable.

And as noted above, they're accessible in other views, just not after taking a view off the detail.

[mslosar]

Not exactly sure what this means, but here's some new info.

I took a new detail of the area and projected a top view and got the same (lack of) result. So i decided to screw around with some things and see what happens. It appears i can get the objects to recognize in the projected view, but ONLY if the entire object is encapsulated within the detail area. If the whole thing does not fall inside the rectange/circle (i tried both) it fails to recognize in the view, though it's displayed.

[torbjorn]

I have similar challenges from time to time, a typical example would be balloons on hydraulic hoses.

The curve (the hose contour) shown on the drawing  view is a tangent of a spline driven sweep - maybe this somehow is considered as some complex geometry that the balloon cannot connect to ?

Have not found any proper workaround for this, so I cheat. I place the balloon in a view where is works, then drag the leader close enough to the curve in the problem view.

Torbjørn

[johnsonshiue]

Hi Guys,

Please send an example to me directly (johnson.shiue@autodesk.com). The behavior does not sound right but I need to see the files.

Many thanks!

[Yashasvi23481]

Hi @mslosar,

This is not exactly the solution, but a fix. You can opt for "attach balloon from the list" option for those items. Quite often when you cant see the part or on other side of plate like fasteners, you point to bolt and add from list all fasteners like washers n nut which cant be visible. If your part list is showing the mystery part, then you can use it.

Regards,

Yash

[mslosar]

I emailed the files.

I've used that work around before, but i really do not like it. It requires that everyone who edits the drawing be aware of it. If they change anything, they have to know that it will affect those balloons or whatever else may have to be done via workaround. The parts list order changes, you have a problem, or a view moves you could have a problem, etc.

Corporately i've got, i don't know, 50ish? people using inventor in different groups in multiple countries. I'd rather find a proper procedure to get it to work right than try to explain to everyone how to use a workaround and make everyone have to look for those things in every drawing they work on 'just in case'.

[johnsonshiue]

Hi Guys,

Mike did send me the files. I can verify the behavior but I don't have a good explanation. It looks like a bug to me. For whatever reason, some components near the detail crop border in a projected view cannot be selected for annotating (dimension, symbol, and balloon). I am working with the project team to understand it better.

Many thanks!

[llorden4]

@johnsonshiue did you ever find a solution for this?  I am struggling with this issue right now myself.

[johnsonshiue]

Hi Guys,

I did work with the project team to understand the behavior. It is considered a limitation unfortunately. We don't have a good solution at the moment.

Many thanks!

[Jasgyc]

Hi,

Bit late to the party, but I had this problem too.

For me, I had the parent part set as phantom in the "Model Data" tab, and must have accidentally set the inividual part as a phantom too in the "Structured" tab. So this meant there wasn't any trace of the problem part unless I expanded the parent in the "Model Data" tab. I only figured out the problem when the part I was trying to balloon wasn't in my parts list after having a proper look instead of skimming.

Hope this information is helpful.

[Anonymous]

@johnsonshiue 

Another problematic drawing with 3D sweeps.

Still seeing the behavior in 2020.3.3 - Date 9/17/2020.

Turned on tangent edges and we were able to select the one of the 3d sweep generated part files.

The same part could be selected in "back" side view, but not the front side view.

We then changed the view to raster and were able to select the problematic parts.

Created a screencast, but it does not appear to be showing up in my list of screencasts, so I'll try sharing the link.

Link to screencast: https://autode.sk/3eaDGzC

[johnsonshiue]

Hi! I am sorry if I am confused. The 3D Sweep issue does not seem to be the same as the original thread. Do you mind starting a new thread with the screencast and the Inventor files. I am more than happy to take a look and understand the issue better.

Many thanks!