Inventor drawing , Parts not showing

[Aldred]

Hi,

With a particular assembly I have an interesting dilemma when it comes to the drawings.  

If I put my base view on an .idw sheet and then project them, some of the channels that I have in the assembly do not show in the base view, but they do show in the projected views.   This happens on an A4 sheet.

If I create a new drawing and then have the sheet size to be A3, then everything shows.  

Has anyone seen anything like this before?

Aldred

[Cadmanto]

Is it possible that you have the visibility turned off for those parts on that particular view?

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[chrismudd]

Can you expand the assembly in the browser/tree and find the missing channels in the base view?  Assuming you can, try right clicking on them and making sure their visibility is active and they are not transparent.  If both of those are good, try selecting "Include All Surfaces," and see if that brings them back.  

it's very strange they show up on the projected view and not the base view though.....  Hope this helps.

[Aldred]

Hi,

The visibility is on in the browser for those parts.

Aldred

[chrismudd]

What about transparent?  

Did the "Included Surfaces" help?

[Aldred]

Hi chrismudd,

The visibility is on and the include surfaces is on as well. The strange thing is the following.

1. I create a new sheet. I change the size to A4. I put in my base view and projected view. The channels do not show in the base view and they do show in the projected view. If I create a new sheet then and make the size A3 then the base view will not have the channels but the projected view will have the channels.
2. I create a new sheet. I change the size to A3. I put in my base view and projected view. The channels do show in the base view and they do show in the projected view. If I create a new sheet then and make the size A4 then the base view will have the channels and the projected view will have the channels.
Could this maybe be a bug?

Aldred

[Aldred]

I turned transparency on and then I could see it.

[chrismudd]

That's really weird.....but, glad it worked for you.  

[johnsonshiue]

Hi Aldred,

There are two common causes leading to this behavior. 1) The part bodies have bad geometry. It cannot be displayed properly in the drawing. Edit the view and change it to Raster view. If the parts appear, usually it is because of bad bodies. 2) Culling error. This can happen when part bodies intersect or interfere with one another. Because of the condition, Inventor have trouble figuring out who is behind whom in the view direction. Open the assembly and do Interference Analysis. If there is interference, please clear it up. It can lead to manufacture error. After that, the parts should appear properly in the drawing.

Many thanks!

[Cadmanto]

This does look to be a bug.  Have you tried this on another machine to see if you can duplicate this behavior, and are you up to date with all of your SP's?

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Aldred]

Hi johnsonshiue,

I have checked for interference (there is none) and I have changed it to raster view it does not show the parts. What troubles me is that if I put it on an A3 sheet it shows everything and if I put it on an A4 sheet it does not show.

If I make the parts transparent then it does show.


I have no clue as to why it would be doing this.

[johnsonshiue]

Hi Aldred,

It does sound like a bug then. Could you share the files with me or send them directly to me ([email protected])? I would like to understand the behavior better.

Many thanks!

[j.glim]

Hello Aldred,

Is there already a solution to this problem?

I'm having the same issue with a not-showing part in Inventor 2022. (2022.4.1)

Turning on transparency in the model resolves the issue. 

[johnsonshiue]

Hi! I could be wrong but based on your description, it sounds more related to the geometry itself. Open the part or assembly and press Ctrl+F7. Is there any bad body reported? If yes, please use Repair Bodies workflow to fix up the geometry. Please feel free to share the files here. The forum experts can take a closer look.

Many thanks!

[j.glim]

Hi Johnson Shuie,

The model contains only solid bodies, no surfaces. It has no bad bodies to repair.

The part not showing is a 1,5mm sheet metal plate, placed under a platform.

When the distance to the platform is about 2 cm, it is shown in the main (frontal) view.

When the distance is shortened to 15 mm, it disappears.

It is always shown in the projected, detail, and section views.

The issue is identical as described by Aldred, however I do not have the A3/A4 issue.

Many thanks,

Jaap

[johnsonshiue]

Hi Jaap,

I could be wrong but I don't think your missing part issue is the same as the OP's, if I recalled correctly. Please share the files in zip here or send it to me directly [email protected]. I am more than happy to take a look to understand the behavior better.

Many thanks!

[j.glim · Accepted solution]

This issue was further attended to in an e-mail conversation.

Just to close the argument for forums sake.

Reply from Johnson Shuie:

The particular part is removed from the drawing view probably due to its relatively thin body compared to other geometry. For better drawing view compute performance, Inventor does remove certain detail geometry.

Thicken the part and it will show.

The thin geometry is hardly visible in a print, I have left it this way.

Greetings,

Jaap