Houston - we have a floater!
Start deleting parts one-by-one and try zoom all each time.
Does it suddenly work as expected?
Attach your assembly here if you can't figure it out.
It could also be a corrupt file that is reporting an incorrect bounding box size.
The CADWhisperer YouTube Channel
Try doing a Windows Encompassing Box, it may require you to zoom out a bit more to find the offending part. As JD posted, look for a "free-range" part. If you do the select in the corner areas you may find it easier than looking for a part in the Browser Window. Do the Window Select and then hit the Delete key.
Then you have a part that is reporting an incorrect bounding box size (do you have any imported STEP or IGES files).
Attach your assembly here
or
here A360 and end all doubt.
(only need one part in the assembly - you can Save Copy As and erase reference to all the others).
The CADWhisperer YouTube Channel
I feel as though I have also seen this behaviour with out-in-space sketch entities. This could be a very large radius where the center point is veeeeerrrry far away from your model.
Though I've not thoroughly tested that theory... I think that will sometimes give the results you're describing. Maybe if the sketch is turned on in the part but turned off in the assembly?
Either way, JD is right about the "bounding box" of some part being incorrect.
I've seen that issue on parts with large radii as well. Mind you it was older versions and only in the sketch model or a sketch that was shared or not consumed in a feature.
@antwanhodges wrote:
I've had situations where when selecting various views from view cube it will zoom in too close to model. Can it be same issue?
The only way I can think of it zooming too close when clicking the view cube is if you have a part or set of parts pre-selected before clicking the cube. I use this all the time while doing in place modeling to get a side or top view of the piece I'm working on without zooming out over the entire model.
Is there any clearance about this issue?
Now, after installing the latest service pack (SP2) i'm experiencing the same problem here. When i hit the "home view" button in an assembly it zooms extremely out. Also in assemblies that worked fine befor.
I have no floating parts, extreme work features or whatsoever. But what i do see after turning visibility on/off for some parts is that these parts cause this behaviour. Strange thing is that when I open these parts separately or place them in new assembly the "fit to view" behaviour is normal. These are all parts that worked fine in the past and i can't see anything strange about them.
Because i haven't found a solution to this problem i've tried to turn off this behaviour. Unfortunately with no result. The "fit-to-view on view change" in the ViewCube options only works for manual view change on the cube an not with the "home view" button.
Anyone any idea how to fix the problem or at least work around it?
Greetings,
Niels
IV 2015 Professional SP2
Dell Precision T3500
Intel Xeon W3670 @3.20GHz
12.00 GB RAM
64 bit Win 7 Pro SP1
Right click on the ViewCube and select Set Current View as Home > Fixed Distance (be sure to set your view first).
Sam B
Inventor Professional 2015 SP2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
thanks for the quick reply.
I've tried that option earlier but unfortunately without result. This only works for the view that is set as the "home view" as soon as you switch over to another view and hit the "zoom all" button it's zoomed out again. Seems to me that it has got something to do with the "zoom all" function and visibility of some features but i can't find any visible elements that far from my main assembly.
What happens if you use the Rebuild All tool (Manage > Update > Rebuild All) in one of these assemblies?
Sam B
Inventor Professional 2015 SP2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
No result.
Stupid thing is that the problem occurs with a sub-assy in the main assy. But when i open the sub-assy itself everything behaves normal and i can toggle views in a normal way.
Sounds like one for Autodesk to figure out. I haven't experienced anything like this, and I don't recall anyone posting about it, either.
Sam B
Inventor Professional 2015 SP2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
Anyone figure out a fix for this. Incrediblly agravating. I can't spend days rebuilding my model from scratch.
Try these steps:
Zoom into the main view
Create New L.O.D.
Window Select Everything
Right Mouse Click and Select Supress
Double Click Mouse Wheel to zoom home
Floating Part should be right there
Mark Lancaster
& Autodesk Services MarketPlace Provider
Autodesk Inventor Certified Professional & not an Autodesk Employee
Likes is much appreciated if the information I have shared is helpful to you and/or others
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Thanks Mark,
Tried as you suggested, still nothing. There are no "floating parts". Model is completely constrained to origin planes.
I was able to find the part that was causing the model to zoom out by deleting each part one by one. This part did have a big radius curve in the sketch. But this part was imported from another file format. I'm not sure which since the file is already saved as an IPT. I did the fix geometry command and fixed the errors it found and that seemed to fix the part and the top model. No more zoom problems. I'm not sure if this is a true fix for everyone but hopefully it helps.
The mates is what is causing the issue. I have this problem too and I cant seem to solve it..it happened when I right click on the workplane and show relationship..it showed up the mate way way up and now my assemblies zoom out far whenever I open this drawing.