Solid, visible parts showing up as hidden lines on idw

[Anonymous]

I'm having issues involving hidden lines that should not be hidden lines in the idw environment.  I have searched the forum boards and have found nothing that adresses this issue specifically, other than http://forums.autodesk.com/t5/Autodesk-Inventor/idw-with-most-of-the-lines-missing/m-p/608278/highli....  This post is seven years old and doesn't ever get around to telling exactly how to resolve the issue.  It references a couple of possible solutions, but doesn't explain what they are.

I am using Inventor 2010 suite, 64-bit.  I have  largish assembly modeled with several sub-assemblies and a few reference assemblies.   Some of the reference models are shrinkwraps from other large assemblies (surface type shrinkwrap, link broken), and other reference models are acutal assemblies that I am unable to shrinkwrap because I need the positional reps that they provide.

When I place my parent assembly, with all the normal and reference models included, on an idw, large portions of the reference models do not show up.  If I change my line style to show hidden lines, the missing parts show up.  At first, I thought that it may be because the reference parts in question were not originally in the view due to the reference data margin, so I started a new sheet and set the margin large enough to show the entire machine, as well as the state of Michigan, before I set the base view, but I still don't get those parts unless I enable hidden lines.

Even at that, Inventor is not behaving consistently.  Some of the parts that won't show unless hidden lines enabled are fabricated  parts that I or a co-worker modeled, some of the parts were imported from SAT, STEP and IGES files, and some of them are shrinkwrap parts.  On top of that, some of the parts will show up normal (without hidden lines shown) if I change the part's BOM structure from reference to normal, while others still will not show unless hidden lines are enabled, regardless of the BOM structure.  Keep in mind, none of these parts are hidden behind anything in the model, even with everything visible in my design view rep, so I have no idea what's causing Inventor to think these parts are hidden.

Anyone have any hints, suggestions or clues?  I'd be glad to entertain them.

I would post my assembly, but a.) It is way to large, even zipped, to post, and b.) due to client confidentiality, I'd get fired, or sued, or both.

Computer Specs:

Dell Precision M6500 mobile workstation (purchased in April 2010)

Windows 7, 64 bit OS

Intel i7 processor

8 GB RAM

NVIDIA Quadro FX 2800M graphics

Inventor Suite 2010, Subscription Advantage Pack, SP3

[johnsonshiue]

Hi! Please send me an email so I can set up a secure account for you to upload.

Thanks!

[SBix26]

I have seen this happen with imported parts, where for some reason the part extents are corrupted or miscalculated.  I'd try turning off the visibility of your imported parts one at a time (or half at a time if there are many) to identify the culprit.

[Anonymous]

I did eventually find a "solution" for this.  If I set my referenced data margin to something really HUGE, like 1000+, the line types show up correctly.  I end up with geometry off the border, but it works.

[Mark_Wigan]

i don't think you are referring to this though but it will potentially help in some cases.

i know in earlier versions if the assembly was corrupted by an instance of a part but this made the entire view invisible. maybe things have changed so that they show as hidden lines in recent versions?

in such a case to solve the problem you need to find and delete the problem causing instance and reinsert it... (only able to find which one is causing the issue is through trial and error sequencially deleting sub assy's from the parent assy, re-checking idw, if no change then undo delete, try next part etc) .

i've seen thid happen with flat patterns that require a forced update. the hidden lines indicate that even though the view is there, it is not necessarily valid geometry.

i've seen the hidden lines problem on flat pattern views, and to fix flat patterns that do this, you need to edit the flat pattern defenition in the part, and it will force an update, and if you save the file afterwards, the views end up okay once again.

[Inv_kaos]

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@Anonymous wrote:

I did eventually find a "solution" for this.  If I set my referenced data margin to something really HUGE, like 1000+, the line types show up correctly.  I end up with geometry off the border, but it works.

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Did you wan't your reference data visible? If so select 'As Parts' , if you don't want your reference data visible turn the part off in the ViewRep or select 'Off' from the Line Style under reference data in the Model State tab. Note, if you want your reference data visible then you probably want to change hidden line calculation to 'All Bodies'. Then adjust the margin as required.

[oldgrey1]

A similar case tripped me up. Only one sub-assembly, which should have presented as solid, presented as hidden lines in all the views. I eventually realised that I had upgraded - I had done some edits in Tube & Pipe - then shuffled my personalised library files around in the folders and then come back in to print, which was when the problem occured. My error was that my personalised library file (*.idcl) was not available (I assume), so I eventually went in to Edit View > Model State and checked "As Parts" and "All Bodies".

Solved.

This post is just to record this scenario - it's unlikely to be the common cause of the condition.

[Anonymous]

I had the same problem in Inventor LT 2014. I just clicked on "Rebuild All" in the "Manage" Tab in the model environment and it fixed the problem!

[eef]

I had a kind of similar problem. One part (the frame) in my assembly showed up as a reference in the drawing. I first thought it has something to do with: edit view, tab model state, all bodies, margin 100000. 

But unfortunately this was not the case. It was something very simple: 

Go to the assembly. Right mouse click on the part, in my case the frame. Go to BOM structure. Change "Reference" in "Default"

[johnsonshiue]

Hi! Another way to make the change is within the drawing. You can edit the view -> Model State -> Reference Data -> Line Type -> As Part. In this way, the BOM will stay as is but the reference components still appear like regular components.

Many thanks!

[Anonymous]

I had no issues with the reference parts showing with reference lines (it would not display visible reference lines on reference parts, the same as it would not display visible lines on non-reference parts), the original issue (which I've seen rarely in the past seven years) was that large parts of assemblies and sub-assemblies were being calculated as hidden, when they were not hidden in or behind anything.  For example, to simplify the issue, if I were to draw a cube, and put a view of the cube in an idw, set to show visible lines only, the view would be empty, but if I were to edit the view to show hidden lines, the cube would show up, but every line would have a hidden linetype, and there would be no visible linetype lines on the entire drawing.

As I recall, I also tried the "edit the view -> Model State -> Reference Data -> Line Type -> As Part" route, and the issue persisted.  This wasn't a 'reference line' issue, it was a 'for some reason, everything is calculating as hidden, even though it is not hidden' problem.

To this day, I have no idea what caused the issue, but I think I had to finally start over in order to resolve it. Like, 'recreate the parent model from scratch' kind of start over.  I don't really remember for sure, I've slept approximately 18k hours since then, and forgotten a few details in the process, I'm sure. We were also trying some new stuff back then, as far as modeling procedure goes, and it could have been any number of issues.

Thanks, though, guys, for still trying, even after all this time.  I really like this community for just this reason!

[HAITH_TICKHILL]

One of my guys encountered this exact problem today. He was doing a GA of an area of gantry and strangely the same small part showed as visible at one end of the view and hidden at the other. I got around the problem by placing the views at a different scale. He placed his views at 1:50 on an A2 sheet. By deleting the views and replacing them at 1:10 then switching back to 1:50 inventor calculated the views normally showing the part as visible at both ends. Just changing the scale from 1:50 to 1:10 and back again from the broken view didn't work so I suspect it is a glitch in the initial view calculation.

Probably a bit late for your initial problem but it might help someone in the future!

[designteam101]

Check if the part is Reference component or not in BOM Structure. 

[johnsonshiue]

Hi! This is an old thread. But, yes, checking Reference component is the first step. The second could be related to the geometry state. For some reason the geometry is not fully computed. It can be fixed by opening the part and do Rebuild All. It will be displayed in the correct line type. If not, there is a bug.

Many thanks!