Sweep - Cut with Solid Body

[JDMather]

I am seeing an increasing number of requests for a Sweep - Cut with an imported stl body.

I know I did this in the past with a particular figure, but with the last two figures I could not get it to work.

Any ideas on this?

[Lucas.dolinarVFXZU]

Can you also Attach a 2022 Version of that? i'd like to try...

But i dont think you can work with Stl meshes without first converting them? I used to have an Addon for that called Mesh enabler.

[JDMather]

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@Lucas.dolinarVFXZU wrote:

But i dont think you can work with Stl meshes without first converting them?

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The stl has been converted to a solid body.

I will post earlier version when I get back to my computer.

[blandb]

Just curious the output exactly, just sweep the solid up the 20?

[JDMather]

Not sure I understand your question.

The idea is to cut a cavity in the base such that the tool body can be removed or replaced back into the base (in the real world).

Because of the undercuts in the organic shape - the solution is not as simple as using Combine - Cut.

To reduce processing load I included only the geometry that will rest in the base.

[JDMather]

@Lucas.dolinarVFXZU 

Attached is 2022 version.

This is for a student thesis project - essentially a display trophy of their research.

The idea is to create a cavity in a display base that a model protein can be placed or removed.

I have seen numerous other similar examples - typically a foam insert for packing and shipping protection of an item.

Molding will not work (Combine-Cut) because undercuts would prevent insertion/removal of the item.  It must be a Sweep - Cut.  The profile will probably need to be simplified for this to work, but I thought in the past that I got this to work with a complex piece (Chess Knight from stl model).  My memory could be wrong.

[SBix26]

By slicing the protein body into 1mm segments, I was able to solid sweep most of them to create new solid bodies, which I then subtracted from the base.  But two of the slices would not sweep, until I divided them again, and two of those would not sweep.  No idea why, though.

Also no idea why solid sweep would not work with the Cut option, but New Solid, followed by Combine-Cut would do the job (in most cases).

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[WHolzwarth]

Good morning, Rhino perhaps has some functionality for this with Drape command.

But a first test shows, that it's not good enough. I'll have another look later in the evening.

[WHolzwarth]

Rhino's Drape doesn't really do it, but there's another command: Meshoutline.

Perhaps it helps some more.

[blandb]

Fusion has something similar to that in the projections for 2d sketch. I believe it is "Project Body"? But will basically do this same thing...Just a thought.

[Cris-Ideas]

Fusion in deed does this. Inventor is not really able to project bodies (I still use AI 2021).

This should be however easy in Atocad.

And even using STL should be easier as STL is just straight edges and triabgles.

So only thing needed is a projection of (probably very many edges) and an envelope of all of that.

Autocad should cope with this quite easily as it has this option to only work with projection.

Simplifying geometry, to a flat projection only will speed up the process. 

Alternatively maybe inventor is able to project stl (do not really have an experience here).

If this stl is not very big I can try. can you pot it?

Cris.

[JDMather]

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@Cris-Ideas wrote:

Fusion in deed does this.

This should be however easy in Atocad.

Autocad should cope with this quite easily…

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@Cris-Ideas 
You must not understand the problem description.

Fusion will not solve this issue.

I will attach the original *.stl when I get a chance.

@Cris-Ideas 

Edit:  >>Here<< is the original Fusion discussion thread.

[cadman777]

Have you tried FLATSHOT in AutoCAD?

That will give you a silouette.

But there's still work to be done to clean it up.
That's what I intend to try when you post the original STL.

Update:

So if I understand the challenge correctly, there would be 2 phases to this solution. The first is creating a profile of the whole part from the top view, and sweep cutting it into the base as far as necessary so the part can slide down into the base and touch bottom without any of the extreme most side protrusions interfering with the base. The second is to determine how much of the bottom segment of the part should be subtracted from the base so that when it touches bottom, there is no interference with the base by any of the protrusions. That would probably need a boolean subtract. That's how I would approach this, if I correctly understand the desired result. In order for me to test my method, I need the original part. I'd first have to convert the mesh to a solid.

[johnsonshiue]

Hi JD,

This is an interesting case. But, I am not surprised Solid Sweep fails. The issue here is that the toolbody is way too complicated. I am wondering if Fusion can help create a smoother toolbody from the mesh.

Here is what I would do.

1) Import the STL file in Fusion and go to Mesh Design environment -> Repair Mesh -> Convert it to Brep.

2) Export the solid body as a SAT or SMT.

3) Import it back to Inventor -> Solid Sweep.

Many thanks!

[cadman777]

Update:

Find attached 2 part files.

One is native inventor, the other is a piece of the protein.

I don't have ToolPath or SolidSweep in IV2010.

Maybe someone can set the protein on the base and do a ToolPath/SolidSweep UP and see if it works.

No point in me wasting time on this by trying to write a Grasshopper script for Rhino.

[cadman777]

Hey Walter,

I did a little research on SweepCut for Rhino.

Here's a forum thread on it.

Scroll down to Pascal's comment on June 30.

Since my R7 trial is just quit, I have to do this the hard way.

But there is a way to do it in Rhino.

Either way (R6 or R7) it's a lotta work, b/c there are at least 30 areas that need cutting/patching.

If I have time next week I'll give it a try and see how much I can get done.

I used Silhouette in Top view like Steve said to create the CurveOnSurface.

Then I had to delete and cut the CurveOnSurface so there's no overlap and so they extrude.

Then it's a simple matter of Trimming one against the other and vice versa, then Jointing the patch to the main polysurface.

I think the lesson in this for Inventor users is, Inventor isn't a surface modeler, and doesn't have the horsepower to do this level of surfacing. That's why I've uses both Inventor and Rhino for at least 20 years.

Below are some screencaptures (SC) of the surface.

Note the DraftAngleAnalysis coloring.
The CurveOnSurface follows those outline contours.

The curves are green (bylayer) and highlighted Yellow to show up better.

SC of a cut-and-patched area:

SC of DraftAngle analysis:

SC of CurveOnSurface that Silhouette created from Top view:

SC of one CurveOnSurface (faint green line - note the complexity!):

One thing I forgot to mention is, I tried offsetting the entire surface outwards by 0.1mm to create a little leeway for the part to fit into it. Rhino6 did a pretty good job. But when I imported it as STEP into IV2010, it failed. There were many problems. I was hoping for better.

Model is attached if you want to play with it...

[WHolzwarth]

Good evening Chris,

thanks for the file. Silhouette curve is an attempt for easy shapes, but this is a complex task. Not much can be done with Silhouette.

But both Rhino6 or Rhino7 have a better one: Curve -> Curve from Objects -> Mesh Outline. This command creates a "shadow curve" from a solid or surface rectangular to the view. I've used it three times for Top, Front and Right view, and imported the 3dm file in Inventor.

There I did three patches with the outlines, thickened them to separate solids, and did a Boolean intersion with them.

The resulting body was cut out of base body.

I think, it's no bad fit, but it can be improved with additional outline curves at 45° between Front and Right view, or more.

STEP in zip attached.

[cadman777]

Hi Walter,

Thanx for the file.

Looks good!

Yeah, that's one way to do it.

If it was a wood base, I 'wood' have done it that way using a router.

It would be routed to one depth, and then a small pocket would be routed for the bottom most protrusion to fit into.

So you have constraints in all directions but up.

That would make your method simple and easy to fabricate.

Plus, you can easily make a 0.1mm offset of your profile (intersection) line.

The 'hand-in-glove' fit is very difficult. Plus, there needs to be an offset of at least 0.1mm all around for the object to be able to fit into the cavity without fighting it. For a 'hand-in-glove' approach, I would try using Pascal's method, that is, if I was doing it for money! But at this point, it's way too much work. And I think I'm all burnt out on this little challenge. I couldn't do any of it in Inventor, even though I wishfully attempted to.

Incidentally, you can get a perfect outer profile in AutoCAD using FLATSHOT.

I just inserted the STEP file into AutoCAD and ran the command and instantly got a profile.

The only thing that sucks about FLATSHOT is you have to spend a lot of time cleaning it up and making sure every single line/spline end is connected to create a 'water tight' profile.

Anyway, that profile can be brought into Inventorm and a simple 'impression' can quickly be made with an Extrude into a parametric base.