Inventor 2013 section views missing

[wvoet]

I am using Inventor 2013 professional.  I have a drawing file that I need to make some revisions to.  When I opened the IDW, all of the assembly section views do not show any parts.  The section views for ipt files are fine.  Does anyone have a solution for this?

[jletcher]

Try a rebuild on the assembly but close the drawing 1st. keep the assembly open and then open the drawing

 Question do you have any step files imported into the assembly?

[wvoet]

The rebuild did not work.

Yes, I do have some ipt files that were converted from stp files.

[wvoet]

I did start a new idw and was able to make a section view of the assembly.  So it appears that something has happened to the IDW file itself maybe???

[jletcher]

I have all ways had issues with some step files and IDW all the way back to Inventor 4 that is why I asked. Never had issues with any idw unless step file was in the assembly.

I will lose views all the time but if I delete the step ipt file my views come back. Sometimes a rebuild worked and sometimes it does not.

 Sometimes the view will work the next day depends on the mood of Inventor.

If you have not saved yet try this close the idw go open the idw but hit the options and defer the idw and see if you have your views.

I don't have 2013 so I can't look at your converted step files.

And no has nothing to do with the idw. I was always able to make new drawings but the next day or so they too lost the views.

Don't know how many files you have that are step files converted but I did find a trick that worked 90% of the time.

Take the converted step file insert it in a idw and do a section thru it. If the step covert is bad the section will not work. This is how I found the bad files and just remodeled them so I will not keep losing views.

So now when I do a step the 1st thing I do is make a drawing and section it in two directions left to right up and down..

[wvoet]

I believe that the converter stp files are ok because when I first made the drawings a couple of months ago everything sectioned fine.  Today I opened the idw to make some revisions that were requested by the customer and that is when the section views disappeared.  I also made a new idw and made section views of the exact same assembly without any problems today.

[wvoet]

I have attached a screen shot of the problem.  Notice that in the model tree there are no models listed under the assembly and note the small size of the section view where I have it highlighted in hte drawing space.  I am hoping someone form Autodesk can help me with this problem.  I need to get these drawing revised and released for a new production run.

[kstate92]

All I have are dumb suggestions such as: it the view still associative with the source? did a LOD, view, or position change or get out of sync?  The tiny outline of current view makes me wonder about a scaling issue as well.

[Anonymous]

Try moving the Section Line that the section is referenced to.  Sometimes by moving the line or detail, it will update the view.

[wvoet]

I have tried moving the section line. No luck. The only hting that has partially worked is to delete my crop of the section view.  The parts re-appear but I loose the association with the balloons and my dimensions do not come back.

[Anonymous]

What about adjusting the Crop Sketch?

[wvoet]

Tried that as well with no luck.

[t_pcoll]

Hi,

I'm sorry for the troubles. So, you tried adjust Crop sketch - so it looks at correct position? The best way to verify whether the Crop is the culprit or not is to delete the Crop. Is Section view still empty after deleting the Crop? Asking because we've seen some Crop views causing problems in Section views in the past.

Thanks

Ladislav

[wvoet]

If I delete the crop the section does return but I am missing all of my dimensioning still.  Is there anything I can do to get the entire section to come back with my dimensions?

[t_pcoll]

OK, then this is probably a known issue.

If it is the same issue as we've seen, you may try to play with the crop sketch (Edit the sketch under Crop item in browser). Flip the rectangle determining the crop area by dragging edges and make it big enough to see some geometry.

Ideally, please send me the dataset to ladislav.pcola(at)autodesk(dot)com - I can take closer look.

Thanks

Ladislav

[wvoet]

Ladislav, I tried flipping the rectangle in the crop sketch but that did not help.

I cannot send you the entire data set because I have some proprietary data from my customer in the drawings. What is the minimum would you need to attempt to determine the problem.

[wvoet · Accepted solution]

Ok. I figured out what the problem was after moving the crop rectangle around some more.  The origin in the assembly had been moved which shifted the parts in the section views.  After some discussion here I found out the assembly model had been used for a presentation by one of the sales engineers and I guess he moved the assembly relative to the origin.  I have it all fixed now.  Thanks to everyone for their help.