Inventor 2022 - Some views in the documentation are broken

[jsek]

Hi everyone.

During putting views, some of them seems to be inactive (damaged).

Attached film shows that only one view is fully correct and can be dimensioned ( view is marked ,,OK,,). Most edges of damaged views are fuzzed and we can't dimensioned them. Only sharp and clear edges are able to dimensioned.

After clicking on th full correct view you can see correct rectangular boundary made of red dots. Rectangular boundary of damaged views show only part of the area.

When you turn off the colour, you can see even more which view are damaged.

We are working in Polish version of Inventor 2022.

Thanks for your attension, we are hope you take care of this problem as soon as you can.

Best regards

[johnsonshiue]

Hi! I suspect this could be related to the geometry or interference. Try this. Open the assembly and press Ctrl+F7. Is there any bad body reported? If yes, you want to use Repair Bodies workflow to fix the data.

Another thing to check is interference. Go to Inspect -> Interference Analysis -> select all components. You may want to clear out the interferences, since they can lead to manufacturing error.

If you turn on Hidden Lines, does it work?

Many thanks!

[rhasell]

This looks like it could be the "demoted assembly" bug.

I still see instances of it in 2021.

I have no suggestions on how to fix it.

[jsek]

Hi everyone!

Thank you for the fast reponse. Unfortunately, the problem still persists. This also applies to our other designs.

Pressing Ctrl + F7 reports a problem with two parts (attachments). These parts were made in Inventor 2018 or earlier. It wasn't until version 2022 that this problem appeared.

Turning hidden lines on or off doesn't change anything. Projections only look better in raster mode.

We are still waiting for your help. It makes our work very difficult. We would love to go back to version 2021, but after updating the Vault database it is obviously impossible 😞

[johnsonshiue]

Hi Jurek,

Something is wrong indeed. Somehow the bad bodies are causing the view compute to fail. I will need to work with the project team to understand it better.

Many thanks!

[johnsonshiue]

Hi! I have found a workaround to the issue. For "Uchwyt Toolflex 20-30.ipt", the bad body was created by Emboss1 (KORPUS TXT1). Edit the text sketch and change the font for the text to Tahoma. The drawing view will be created.

For "Obudowa elektryczna 175x151x95 EX171.ipt", the bad body was from the box part in the derived source assembly. If you do Rebuild All (Manage -> Rebuild All), the error will go away.

Many thanks!

[jsek]

Hi johnsonshiue!

Thank you very much for your help and your time. For the "Uchwyt Toolflex 20-30" item, replacing the font helped. Why wasn't this bug in earlier versions of Inventor?

In the case of the element "Electrical enclosure 175x151x95 EX171", the "Rebuild All" does not help. I still get the error. I am enclosing the detail and the Ctrl + F7 report after the rebuild.

[johnsonshiue]

Hi! This is absolutely a bug (reported as INVGEN-48652). It seems that the 2022 drawing environment is more sensitive to bad bodies. The thing with bad bodies is that it may appear working (in the past). But, it could lead to downstream failure. The behavior can be unpredictable. It is always better to have good bodies. However, bad bodies could be generated by Inventor itself. So, some level of tolerancing badness should be expected.

At the moment, we don have a fix yet. Regarding "Obudowa elektryczna 175x151x95 EX171.ipt", Rebuild All seems to work for me. Another thing to try is to suppress the bad body (expand the derive node -> EX171 - Obudowa.ipt:1 -> right-click on the nested node -> Suppress). This will allow you to place the drawing, because the bad body is suppressed. After that, go back to the part and unsuppress the bad body. The drawing view will be updated (including the bad body).

Many thanks!