Inventor 2018 not recognizing solid body intersections?

[Anonymous]

I'm working on a spaceship, and I have run into a problem with a specific set of fillets. In the image below, inventor isn't recognizing that there is an intersection and won't allow me to fillet the corner so that the two bodies blend better, but instead is only trying to fillet the edge, which should be part of the other body. Does anyone know what the problem with this is?

[johnsonshiue]

Hi! Are they two separate solid bodies? To create the fillet on the intersection edges, you will need to combine the two solid body (Combine -> Join). If you cannot figure out, please share the file here.

Many thanks!

[Anonymous]

Whenever I use the tool it just says there aren't two solid bodies, and only one. 

[WHolzwarth · Accepted solution]

This is a rather complex part, respect to your ideas.

But you could have done easier with using different bodies, creating their shape, and patterning them later. Thickening instead of some extrusions would be cleaner, too.

I've noticed some tiny edges, that need to be cleaned up. Similar with some faces caused by too long extrusions. On the other hand tiny gaps need to be filled.

But the main problem for you is turning the initial solid into a surface body. This happened with Delete Face1, and the following Delete Face operations. You can do this, and it works pretty good in many cases. But the Heal option needs to be checked.

These issues need a change. I only could find your other problem by looking at the coordinate system and zooming into the geometry. Repairing there is possible, too, by thickening the end face after deleting with healing some of the existing fillets.

Enough for now. It's time-consuming. Show us your progress.

[JDMather]

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@Anonymous wrote:

Whenever I use the tool it just says there aren't two solid bodies, and only one. 

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Right click on the Surface Bodies(1) folder and uncheck Visibility.

What do you observe?

[Anonymous]

I see this...

From what it looks like, solid bodies are bodies that I can build off of while surface bodies are bodies that I cannot, such as the twists because they have curved surfaces

[JDMather]

Beginners should (almost) never use the Delete Face command.

Your design has a lot of cylindrical geometry - yet I do not see any Revolution features.

The first 24 features can be simplified to one sketch and three features (including the Pattern as a feature).

Your entire design can be significantly simplified.

I recommend that you start over using what was learned from this attempt.

I would probably do two more trials.

Trial 1 - simplify to Revolve(s).

Simplify to reduced number of Patterns.

Trial 2 - repeat Trial one simplifying as far as can go.

I am pretty sure I would not have ANY Delete Face features.

BTW: You can build off surface bodies - but you must use the surfacing tools.

And you had several unconstrained sketches...

[Anonymous]

Thank you so much for the help, I decided to go back and delete the delete face operations I had done and find the original feature and remove it from the part. Once that was done my project dropped its surface bodies and formed two solid bodies that I was able to combine using the tool. I still don't know why deleting an unrelated surface created this whole problem, but thank you for the help!

[Anonymous]

Thank you for the tips, I have been using inventor for over 3 years now actually, I use it for school things. This was my first time using the delete surface tool and I am probably just going to let it be for a bit until I understand it more. I was able to fix the problems by removing the delete surface features and using the combine tool to join the two separate bodies. I'll also check out possibly simplifying my features, it has always been something that I am bad at since I usually build my things in pieces and don't think ahead that much.

[JDMather]

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@Anonymous wrote:

... something that I am bad at since I usually build my things in pieces and don't think ahead that much.

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I consider my first attempt to be merely a trial to understand the geometry.

Then I start from scratch using what I learned from the initial attempt(s).

Some people might consider this a waste of time, but then I watch them fight for hours (days? weeks?) trying to "put lipstick on a pig".

[Anonymous]

I think that's a good way of putting it, make the first design just a rough image of what it should be, and instead of trying to constantly go back trying to make things better just start over and create a cleaner end result

[johnsonshiue]

Hi Joshua,

I think the major issue with the approach you were talking is scalability. When you use a feature-based parametric solid modeling CAD system like Inventor, always think about how you can scale and configure your design. For example, somebody wants you to change the structure a bit, changing from 3 prongs to 4 prongs. You will have hard time doing it with your current model. The geometry will be too brittle to modify.

It looks like you are doing conceptual design on Inventor. I personally don't think Inventor's power lies on conceptual design. This kind of stylish design is done on a more free-form or free-style environment without thinking too much about dimensions or accuracy.

In reality, the model should be broken up into components in an assembly. Each component is driven by some parameters. Any component can be replaced by a new one. You can tweak the geometry on an individual basis.

Many thanks!

[WHolzwarth]

These are the basic shapes for a multibody approach. Only a few separate solids, that can be filleted before patterning and combining into a single solid.

I wouldn't recommend an assembly. Constraining is a challenge, and  melting back to a single part has no benefits versus a multibody.

I've used Construction Environment for doing this. The initial geometry is set in Solid1 and can be deleted, after the new approach is completed. Only a few sketches were used, without any dimensions, but that can be done in some refinements.

2018 IPT attached.

[Anonymous]

I have been working on remaking my project, and so far I've only used one revolution, one extrusion, and one circular pattern to create my base shape, and since I now know what I want it to look like, I can copy the dimensions off of my original and apply them to my cleaner version

I am thinking about making an assembly for the arms and spiral parts as on the real design (that I am basing my model off of) the arms will rotate as the ship moves

[Anonymous]

This is something that I have come to terms with, that I generally do not use inventor for its intended purpose, which seems to be more industrial based rather than open 3d design. I have 3d printed things that were made in inventor, but of course when doing that things must be broken up if they are large and complex. Since school is not in session, I have been spending some time just making things for fun, and this project is one of them. If my school used a program such as autodesk maya I would probably utilize that more than inventor, at least for these types of projects

[Anonymous]

Hello! Its me again, I've decided to redo my design like you suggested. The main reason why my original project was so messy is because I didn't know what it was going to look like at the time, and now that I do I've been able to massively reduce the amount of features needing to be created. The only downside to me doing this in my opinion is that I'll have to spend a bit of time remaking the twisting portion of the ship, mainly just getting the rails in the 3d sketch to be orientated properly. Here's what it looks like so far, with only 3 features.