Hatch pattern disappearing in section view

[alexander.naljot]

Hello dear Inventor community,

In my sectional view, my hatch pattern disappears. There is a part where you can see the hatch on one side, but not on the other side. I would be very grateful for any assistance.

[Gabriel_Watson]

Do you have this on?

Also, right-click the section view and pick "Edit Section Properties...", then:

[alexander.naljot]

Hello Gabriel,
Thank you for the fast answer it works, but I can not adjust viewing depth.

[Gabriel_Watson]

De-select "Slice all parts", set your distance, then right-click the components inside the section view by the browser to change the section participation... see if that works.

[alexander.naljot]

I have tested this it's not working. I can not adjust the view depth.

[Gabriel_Watson]

Please attach a sample for testing here. You could delete most other components and just leave a minimum set of files (drawing plus a few components) to reproduce the problem.

[alexander.naljot]

Hello Gabriel,

Thank you very much that you try to help me. Attached you will find all the components.

[Gabriel_Watson]

Quite a unique structure here... enormous complexity for a relatively simple part. Perhaps too complex for Inventor, and I would guess you could probably create better ways to build this geometry to avoid further issues.

However, this seems to be all due to Inventor's inability to capture a complex scenario like this one. I will tag @johnsonshiue here to check with the quality team.

As a workaround, if you right-click your view and select "Make view raster", the section view behaves normally:

[alexander.naljot]

Hello Gabriel,
Thank You very much for your help. This design it's not completed yet and I am open and grateful to any suggestions that you could give.
I already knew that, that it works with raster view. This isn't the first time that it doesn't work with complicated geometries.

[Gabriel_Watson]

I found another workaround:
Exporting this part to STP format and then importing it back in will "cut" the complexity, although it converts all geometry to dumb solids. See attached.

You may also try deriving this part into another to cut away the many references to create the geometry. Perhaps a derived part will be fine on the section view.

[alexander.naljot]

Thank You very much Gabriel, somehow it works every time.

[johnsonshiue]

Hi! This is probably a leaky section profile issue. There are places on the model with tolerant edges (edges with gaps). When sectioning, the closed profile isn't as tight as it should be. As a result, the hatch isn't applied because it was considered not a closed profile.

Please share the files here. I did not see the files. I would like to understand the behavior better.

Many thanks!

[alexander.naljot]

Dear Johnsonshiue,

Thank you for your prompt attention to this matter. Please find all the necessary files attached.

Best regards,

Alex

[johnsonshiue · Accepted solution]

Hi Alex,

Many thanks for sharing the files! I took a quick look. It does seems like a leaky profile issue. There are a few edges having loose tolerance. The bodies check fine. But at certain view angle, the 2D section profiles in the drawing may not be as tight as they should be.

Here is a simple workaround to bypass the issue. Open 16065404-7-Querschläge-Skelett.ipt and create an offset workplane passing the center axis of the middle cylinder. Then use Split command to split all faces on the middle body. After that, the hatch should be displayed correctly.

Thanks again!

[alexander.naljot]

Hello Johnson,

While I didn't follow the recommended workflow, I believe the essence is the same, and now it works with the hatching. I connected the middle solid with another solid using booleans. The hatching is functioning now. The question is whether all the 2D profiles are actually closed. I used the "Close Contour" command specifically, but I'm not sure which profile is not closed.

Thank you a lot for your help!