Imported Step File Is Not Visible

[wklarich]

I imported a step file of an assembly and although all parts are present in the Browser, nothing is visible in the Graphics Window.  In the Import window, convert model, solids, surfaces and wires were all checked.  In the opened file, everything is checked visible in  the right-click menu, and nothing is checked transparent.  When I open one of the parts in the assembly, I can see the wire frame, but can't make the part solid.  In the iproperties, the material is generic, and changing it to  steel doesn't help.  If I promote the wires in the construction group, the wires become darker in the opened part and the wires for the part do appear in the assembly, but still not solid.  I hope someone can tell me what button to push to make it all better.  I work with step files frequently and haven't had this problem before. 

I have attached a screen shot and one of the part files.  I can't share the assembly without getting permission from the owner.

Thank you in advance.

Bill

[hncarle]

This has happened to me occasional.  The problem has always been the view settings.  Click the view tab and open the Object Visibility.  Make sure the "Construction Surfaces" is clicked. 

[wklarich]

Thank you, but Construction Surfaces was checked.  In fact, all boxes were checked.

[JDMather]

This is probably a difficult question to answer - but does the size of the STEP file make logical sense for the geometry (that should be) included in the file.  Or is it "unusually" small file size?

You might Save Copy As a different assembly as STEP (check the translation) and then open the two files in NotePad and compare the text for some indication of differences.

[johnsonshiue · Accepted solution]

Hi!! The STEP file you are trying to import seems to only contain wire bodies. When they are imported to Inventor, the wire bodies are stored in Construction Environment. At assembly level, geometry in CE is not shown because they are not parametric and not associative. What you need to do is to open each imported part and expand Construction folder -> right-click on the wires -> Promote Wires. They will become a 3D Sketch in the part. Then you will see the geometry in the assembly.

Many thanks!

[wklarich]

Thanks for your help.  The file size is 9 mb, and it looks OK to me based on another step file I have.  I could compare the translation reports, but I wouldn't know where to go from there.  I had another answer to my question suggesting that the solid info isn't in the files.  I believe that's right.

[wklarich]

Thank you for your help.  I believe that you are right.  The parts in this step assembly have wires in the browser, and other step files that I have, have solids.  I have received step files from the same source before and have had no problems with them.  The person who made these files for me doesn't think he did anything different from the past translations.  However, I think something changed on his end.  We got around the problem by using an igs file format.

[ptnovak]

Hello,

Had this similar problem and noticed that for an unknown reason the specific type of .STEP file that was imported to my assembly automatically showed up as non-visible in the model tree of the corresponding assembly drawing.

Meanwhile everything was visible in the .iam file. Wanted to leave this here in case someone else finds themselves scratching their head on this issue.

BR,
PTN

[JDMather]

@ptnovak 

Did you figure this all out?

Are you aware that you have a surface body rather than a solid body?

[ptnovak]

I'm certainly aware of that. Why it appeared visible in the model state but was invisible in the drawing state I have got to be honest I have no clue.

This was merely something I felt someone might encounter and look up. As I tried to before figuring it out.

[SBix26]

From Inventor 2024 Help | To Work with Surfaces in Drawing Views | Autodesk:

Create Views Containing both Solid Bodies and Surfaces

By default, when you create a view of a part that contains solid bodies and surfaces, the view contains solid bodies but no surfaces.

Inclusion or exclusion of surfaces in child views is the same as the base (parent) view. If you include or exclude surfaces in a parent view after child views are created, they are not reflected in the child views.

1. On the ribbon, click Place Views tab   Create panel   Base.
2. In the Drawing View dialog, select a part (or assembly file in Inventor) that contains parts with a mixture of solids and surfaces.
3. On the Component tab, specify the Representation, Scale, Label, and Style.
4. On the Model tab, specify Reference Data, and weldment information when enabled.
5. On the Display tab, specify the display options to use in the view.
6. On the Recovery Options tab, specify whether or not to include surface and mesh bodies and work features.

Create Views Containing Surfaces but No Solid Bodies

When you create a view that contains surfaces but no solids, the view in the graphics window automatically includes surfaces. Surfaces are included in dependent views based on their inclusion or exclusion from the base (parent) view.

1. On the ribbon, click Place Views tab   Create panel   Base.
2. In the Drawing View dialog, click the arrow on the File box, and select a part file that contains only surfaces.
3. On the Component tab, specify Representation, Scale, Label, and Style.
4. On the Model tab, specify Reference Data, and weldment information when enabled.
5. On the Display Options tab, specify the display options to use in the view.
6. On the Recovery Options tab, specify whether or not to include surface and mesh bodies and work features.

---

Sam B

Inventor Pro 2024.2 | Windows 11 Home 22H2

[johnsonshiue]

Hi! These base view options are remembered last used per source doc type basis (iam, ipt, or ipn). For example, if you create a base view from a part with desirable options, the next base view for a part will have these options turned on by default.

Many thanks!