Confusion over imported files, composites vs. surfaces, construction vs. repair.

[nbonnett-murphy]

Hello, I feel like I am missing something fundamental about the repair/construction environment.

Since I don't have 1 specific question, but rather a general sense of confusion, here is how my workflow goes. Hopefully someone can tell me what I'm missing here.

I have a model that was imported as a composite. There are some obvious missing faces, so what I'd like to do is extrude a surface, then trim, then extrude a cylinder, use that to trim a hole into a face, and then stitch everything up.

My problem is that I can't seem to interact/modify with the composite at all. Any attempt to trim it with another surface gives me an error saying that my cutting surface (extruded cylinder) doesn't intersect any surfaces. Well obviously it intersects the composite, so why can't it trim that inside the modelling environment?

Take 2: open the imported surface model in the repair environment. My cutting cylinder disappears since it's lower in the tree. Ok, I'll just extrude a new one and cut with that. Nope... there are no surface modelling tools for new geometry inside the repair environment. Fine. At the very least I can try a boundary patch on this test model:

Awesome looking good. Let's try it on the real thing:

Ok, the coordinate system isn't aligned with the part. No problem, I'll continue defining patches and then just extend/trim them...

Good, good...

aaand nope. Can't select the opposite edge, can't create a wire at the corner with a sketch inside the repair environment, can't create a new surface in the repair environment. Can't make a sketch to extrude a new surface in the repair environment. Can't patch in the surface manually in the modelling environment, then stitch, because the composite and modeled surfaces apparently can't be interact in any way. Can't can't can't. At this point I'm beginning to wonder what exactly the repair environment can do.

Ok, last ditch effort: create all missing surfaces in the modelling environment, boundary patch, trim edges to line up, extrude the cutting cylinder for the hole. There's no intersect tool in the modelling environment. Fine. We'll do it with a split instead... Split only let's you select faces as cutting tools, not edges. Fine, I'll do a bunch of splits, and then a bunch of delete face operations. Never mind the clutter, at this point I'm beyond caring. Nope, the composite and my new surfaces still can't interact. Ok then, transfer the whole lot to the construction environment. Nope, the surfaces and the composite still can't interact with each other, so no trimming, no splitting, no intersecting, no nothing. As far as I can tell, this is just the repair environment all over again. Scratch that.

Finally I realize the key: zero distance offset the entire import so it's a set of surfaces instead of a composite. Manually patch in the missing surfaces. Whine about the fact that combine, the only tool that would actually make this operation more efficient, only works on solids, and that there's no intersect in the modelling environment.

With that, I was finally able to solidify a portion of the imported assembly. But I'm still left confused as to why so many of the inventor tools failed me. Why can't I build some surface geometry in the modeling environment, pull it into the repair/construction environment, then use those tools to modify/combine the 2? Why can't composites and surfaces interact? Do I misunderstand the purpose of the repair and construction environments? Does inventor have useful surface modelling tools hidden away somewhere?

What's best practice or how do the developers expect us to handle this situation? It seems that importing things as composites is a bad idea, so "don't do that" is probably the answer. But in the real world I have to deal with controlled data that was originally imported as a composite, so sometimes there's no way around it.

Also, why can't I box select surfaces?

[Frederick_Law]

Project the surface/edge to sketches and extrude.

You can split the composite into surfaces.

Use closed "boundary" to create surface.

Use sketch to create "boundary".

Attach your file.

[swalton · Accepted solution]

I find that the "Repair" environment is useful for fixing a few modeling errors, like slivers, or miss-aligned edges.  

If the imported geometry has missing surfaces, or really bad geometry that needs modeling repairs, I use the Construction environment.  This is an older way of working with surface geometry.  I learned it first so it tends to be my goto tool.  I will use the normal modeling tools to create surfaces, then copy them and the bad geometry to the construction environment.  Once there, I rebuild/repair the gaps in the model and create solids.

Overview of both environments:

https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-00960F8C-472D-4B9B-A92D-98144D2883C2

Construction Environment:

https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-70C282A1-DC14-429E-919A-0C16A99BB569

[johnsonshiue · Accepted solution]

Hi! Let me try to provide some clarification. Composite is more like a group. It can consist of solid bodies and surface bodies. It is mainly for referencing purposes. If the Composite contains enclosed surfaces, you may stitch them into a solid body (at the given tolerance).

In Repair Environment (and also Construction Environment), you may transfer some bodies from one Composite to another. Such operation helps narrow the target of interest.

In terms of RE and CE, the major difference is about data persistence. In RE, the geometry is properly tagged and named. It can be used for downstream reference or feature consumption. But in CE, the geometry is more like in raw data. It cannot be used for downstream reference or feature consumption, unless the geometry is promoted to the parametric modeling environment.

Many thanks!

[nbonnett-murphy]

Thanks for the info everyone, it looks like the construction environment is probably the most appropriate for my needs here. I'll focus my efforts on learning to use that effectively rather than jumping around between RE and CE for now.