Measuring and/or extruding from imported STEP file

[eli_duykers]

Hi folks,

This is a recurring issue for me, and I'd like a higher level solution to improve workflows in future. The problem goes something like this:

1. I import a shape from other engineering suites, usually in the form of a STP/STEP file. Inventor does a good job of interpreting it. Nice!

2. I want to measure or work with profiles in the shape. Say I want to measure the area of an orifice:

Well, Inventor's Measure tool won't let me do that. Okay, I'll create a solid there instead.

3. Project geometry, going well.

4. Go to extrude. Get a red outline, with no further clarification. Click okay, and am met with the mega-informative error message:

There's really nothing I can do with this lack of information.

5. Fearing it's the "Project Geometry" not being tangible enough, I redraw the shape over the top, snapping to the projected geometry. It's fully constrained and, to my understanding, a simple closed shape. Try to extrude that? Nope, no bueno.

This raises several issues. It hamstrings both Inventor's ability to inspect geometry originating from other apps, and to use it as a frame of reference. I don't understand how, within Inventor's basic workflows, none of these options can work. I'm also very disappointed with the lack of user feedback, guidance or meaningful information provided. Feels very amateur, but I'll open the floor to suggestion.

[JDMather]

@eli_duykers 

This should just work - not sure why it isn’t. Can you Attach file here that exhibits this behavior?

[CCarreiras]

Hi!

It should work, but Yes, sometimes can happen some manifold errors.

Check this process:

Sorry about the bad resolution, but we cannot upload big files here.

If you don't understand something about the process, we can manage it... 

[johnsonshiue]

Hi! Is the geometry outside of the valid model range (+-100m in X, Y, and Z)?

Many thanks!

[eli_duykers]

Thanks for your patience folks, the original part contained IP so I've replicated the issue with a nonsense part (see attached zip). Interestingly I made sure the nonsense part was under 100mm in all dimensions - although this one is news to me. What is this +/-100mm model restriction? Isn't Inventor used to model enormous structures?

At any rate, the issue recurred. Here's the example file, including the STEP, the Inventor-generated assembly from importing it, and a fresh screenshot of the issue. I just used the circular hole this time, as the slot had some artefacts that complicated it unnecessarily.

CCarreiras - that looks like an interesting workflow, but unfortunately the gif compression makes it quite hard to follow.

[CCarreiras]

It's not 100 mm.... it's 100 meters

[eli_duykers]

Ahh, I misread 🤓 No, definitely below that!

[CCarreiras]

HI!

Your goal is to have this, right?

[JDMather]

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@eli_duykers wrote:

...the slot had some artefacts that complicated it unnecessarily.

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The ends of the slots are planar facets rather than cylindrical faces.

Now let me look at the holes..

[JDMather · Accepted solution]

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@eli_duykers wrote:

I just used the circular hole this time...

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The sketch that you are attempting to Extrude is at the assembly level - not at the part level.

Can only Extrude-Cut material at the assembly level and there is no material to cut.

This is logical behavior and has nothing to do with being imported STEP geometry.

To edit the part - right click Edit on the part node to edit within the context of the assembly or Open.

Note the additional options besides Cut when editing at the part level.

BTW - iProperties would seem to indicate that you have not installed the Updates for 2022.

[eli_duykers]

Thanks, that's a workable solution. I think the program shouldn't have a great big "start sketch" button that defaults to the assembly, if indeed an assembly sketch is hamstrung to not work properly, and I definitely think an extrude error for something so prevalent needs an informative error message. Better app design, in my opinion, would allow a fully featured sketch to be driven by the selected face in an assembly. After all, the face belongs to one solid, not multiples... right?

But yes, empowered with this information, I can now do what I need to, so thank you.

[JDMather]

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@eli_duykers wrote:

1. ... if indeed an assembly sketch is hamstrung to not work properly, and

2. I definitely think an extrude error for something so prevalent needs an informative error message.

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@eli_duykers 

1. Not "hamstrung" but rather closer duplication of the real world.

If I go out to the shop floor and I assemble two components - I do not generally add more material (except in welding or similar processes).  I only subtract material after assembly.  The parts generally come to the assembly stage fully formed.  So if the part has a requirement that it should be edited - that is done in the real world at the part level, not at the assembly level.  There are some cases where parts are modified (material removed) like match machining for dowel pin registration.  Inventor permits this removal of material that does not propagate to the part level - only exists at the assembly level.  So Inventor is replicating the real-world processes in the modeling process.

2. The error message could certainly be more helpful.

[eli_duykers]

Must say, I can't agree with you there. In my many years fabricating parts, it's extremely common to need to design and manufacture a part that goes between two other parts in an assembly. The first thing anyone does in in the field is (where possible) look at the full assembly and use it as a reference. Measuring or even cardboard templates using the assembly as a reference are invaluable. An idealised digital embodiment of this would be extruding, lofting etc from one part in an assembly to another. Alas, Inventor has a very rigid way of building material. It is what it is I suppose.

[JDMather]

@eli_duykers 

That is not what I wrote.

You have missed my point.