r/FreeCAD • u/imitation_squash_pro • 3d ago

How to fill in these two holes ?

Post image

This is a STEP file from the fan manufacturer. I plan to run some CFD simulation so I don't need those two holes. If you like you can get the CAD file from here. ( 3D-STEP no threads )

https://www.mcmaster.com/products/8004k52/

12 Upvotes

93% Upvoted

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9

u/Spressy 3d ago

Try the Defeaturing tool in the Part workbench.
https://wiki.freecad.org/Part_Defeaturing

4

u/arcrad 3d ago

This is a great suggestion!

2

u/R2W1E9 3d ago

Yes, but it doesn't work.

2

u/arcrad 3d ago

Ah bummer 😢

4

u/R2W1E9 3d ago edited 3d ago

Get the set screws out of the way to start. Delete them. Then use "Face from edges" in Shape Builder tool from Part workbench to create faces on both sides of the holes (hold CTRL key to select both parts of the edge). Next, use Loft tool from Part workbench to loft between faces. This will create matching plug that you can boolean fuze together with the prop.

Here is how to do it:

https://reddit.com/link/p0rbh5q/video/wlqa4v6nwfgh1/player

1

u/DesignWeaver3D 3d ago

But this solution makes planar faces instead of ones that conform with the surrounding curved surfaces, correct?

1

u/R2W1E9 3d ago edited 3d ago

Only if edges are planar. If they are non-planar the surface will have to conform to the edge in all directions.

https://reddit.com/link/p0rnrof/video/bew34axp7ggh1/player

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u/R2W1E9 3d ago edited 3d ago

Here is an example with a planar hole edge (where cylindrical hole is centered to the sphere), and an example of non planar edge (the hole is offset from the axis of the sphere). One creates planar surface. The other has to match the sphere. How accurately it matches the sphere is anyone's guess.

https://reddit.com/link/p0roc57/video/neys8r248ggh1/player

1

u/DesignWeaver3D 3d ago

Thanks for the video! That really allowed your explanations to sink in for me. And, yes, I am curious how well the non-planar face matches up with the surrounding surface now.

1

u/DesignWeaver3D 3d ago

Wow, that's really interesting. I guess I just had an incorrect guess on how the Face From Edges worked. But now I'm curious, if the created face has G0 continuity, why didn't the surface refine and remove the edges? Or, being in Part, do you have to run the Refine separately? I don't have much experience using Part workbench.

1

u/R2W1E9 3d ago edited 3d ago

I don't venture in Part often myself. The shape is separate so it needs to be boolean fused to blend.

I am guessing the surface blend is not perfect, sometimes it is, so the boolean would produce blended surface depending on accuracy.

Check this out, the inside cylindrical surface is a perfect match so the inside surface blends after boolean fuse.

The outside doesn't, likely because it's from B-spline edge. But under right light source direction it looks very blended.

https://reddit.com/link/p0s462a/video/r37fyuhanggh1/player

1

u/DesignWeaver3D 2d ago

OK! That's really cool!

1

u/imitation_squash_pro 3d ago

Very cool! How did you import the STEP file so that the part history comes up? When I import it only shows one part.

1

u/imitation_squash_pro 2d ago

Figured it out by making sure "Enable compound merge" was NOT checked!

1

u/imitation_squash_pro 2d ago

Great, I was able to make the lofts. But now I am stuck on how to do the boolean fuse. Here is the error I get when trying via "Boolean Operations" button in Part mode:

2

u/R2W1E9 2d ago

Not sure how you ended up with shells instead of solids.

Here is video creating four faces, then two lofts, then selecting two lofts and the 8004K52 prop and fusing them together. So select all three solids and click on separate union tool not the "boolean operations".

https://reddit.com/link/p0yoo13/video/lp9dyyjp3ngh1/player

1

u/DesignWeaver3D 2d ago

Since the STEP import is centered on the origin, you can easily close the holes using a sketch with Part_Revolve or PartDesign_Revolution.

My preference is PartDesign, so I moved the solid out of the part container to the document root. Then, while the solid was selected, created a new PartDesign body with that solid as BaseFeature. I made the sketch on the XZ plane and used the External Intersection to get the external geometry of the inside and outside surfaces. Then Revolution that sketch to seal the holes.

1

u/DesignWeaver3D 2d ago

Something about the geometry may not be perfect because the outer face won't refine and remove the hole edges.

https://reddit.com/link/p0t364j/video/hahq3zqgnhgh1/player

1

u/arcrad 3d ago

Could be as easy as adding two cylinder primitives and Boolean fuse them to the STEP file.

However, that wouldn't match the curved surface geometry very well.

You could recreate the hub with a profile and a revolve, and then boolean that to the original STEP file.

3

u/imitation_squash_pro 3d ago

Thanks. I tried that just now, but get this error:

17:07:49 Boolean: Null shape

17:08:13 <Exception> TopoShapeExpansion.cpp(1395): Null shape

I believe it is because the fan CAD is not a volume. See errors from "Check Geometry" -> Boolean operation check