Fillet wont work

[nick.jeuris.hotmail]

I have a problem executing a fillet R30. Sometimes 3 out of 4 edges work, but I never get them all 4 working. Maybe it has to do something with the loft?

I am using Inventor 2013.

Greetings,

Nick Jeuris

[nick.jeuris.hotmail]

Anyone who can help?

Nick

[JDMather]

Your design intent (at this point) doesn't make sense to me.

What about those four corners - will they have fillets?

Can you post a hand sketch or pic of similar part?

[johnsonshiue · Accepted solution]

Hi! There are multiple issues with this part. The way the solid Loft feature was created is not ideal. There are actually overlapping faces on the body. You can use Delete Face command and select the top square face to see the faces.

This particular Loft is better to model as surface and then use Sculpt command to join it with the main solid body. However, the fillet problem still persists after that. It seems that the fillet is having trouble with the top square face. I am forwarding it to development team for review.

In the meantime, I am able to find a way to get the desirable shape created by using surface modeling technique. Please take a look at the solution in attached part and let me know if you have any question.

Thanks!

[nick.jeuris.hotmail]

JDMather, my design intent is to make a surface from the 3D edges to the square. This has to be a smooth surface, therefore I used the fillets. The four corners will have small fillets.

johnsonshiue, I thought it was only the loft that gave me problems. I would never think of the top square to obstruct the fillet. Your solution works for me.

Thank you very much!

[JDMather]

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@nick.jeuris wrote:

The four corners will have small fillets.

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I would fillet those corners before adding Loft or Boundary Patch.

[kenjacques8585]

In my experience, the loft command in Inventor creates mathematically weak geometry that seldom can be used with solid modification tools like chamfer & fillet. Possibly because of some inaccuracy in which the vertexes are calculated or perhaps the way fillet/chamfer is calculated. I've notice fillet & chamfer causing logically weak geometry on vertices of  the intersections of compound curves.

Lofts + Fillets are a combination that rarely work well. I'd suggest filleting the corners of both the square and the cube prior to loft. (In other words reverse the modelling order Fillets + Lofts instead of Lofts + Fillets) Use the loft options to adjust the strength and direction of the curves to your desired geometry. Remember to have the same number of vertices for each profile used in the loft. If you don't, you'll most likely get ugly geometry or errors.

Use loft last.

[johnsonshiue]

Hi! I personally do not agree with the statement that Loft and Fillet/Chamfer don't work well together. If you have cases exhibiting the behavior, please let me know asap. I would like to take a look and see why they are not working.

I think Inventor Loft is a little bit too flexible allowing too much degree of freedom in terms of forming the shape. In some cases, the mathematically valid shape defined by limited constraints applied by the user may not be consistent with what the user anticipates. To get the shape precisely, sometimes it requires more constraints in terms of sketch or guide rails or sections.

Anyway, there is always room for improvement in Inventor. If you have an example showing an unexpected behavior, please let me know.

Many thanks!

[JDMather]

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@kenjacques8585 wrote:

In my experience, ...

Lofts + Fillets are a combination that rarely work well.

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I notice in this thread that your system exhibits instability in general
http://forums.autodesk.com/t5/Autodesk-Inventor/Utterly-Unstable/m-p/3596630#M446047
that doesn't appear to be resolved.
 
I would agree that if there are other techniques - use them rather than Loft.
But for many many designs I have successfully used Loft + Fillet

[kenjacques8585]

The other thread you are reffering to is about software stability. I don't think it is relevant here.

The loft & fillet.ipt is my suggestion to Nick Jeuris. Note that the first solid's fillet cannot be increased in radius. The second solid presents more along the lines of what Nick was expecting.

Fillet on Compound Curves.ipt demonstrates my statement of odd fillet behaviour. Note that the projected cut edges in sketch 5 properly identify the cross section of the compound curves as an arc and provide a center point. The fillet however does not generate a center point though it should when bisected at this plane (at least it is expected to).

[johnsonshiue]

Hi! Thanks for attaching the examples! I am trying to understand what you meant by the following.

"The fillet however does not generate a center point though it should when bisected at this plane (at least it is expected to)."

Are you talking about splitting the body in half (on XZ plane) and trying to create a workpoint on the filleted edge maybe?

Could you help me understand the question better?

Thanks!

[kenjacques8585]

What I was attempting to demonstrate is the result of the fillet command is more of an approximation than a fillet. In sketch5 the projected edge of the fillet should have a center point. It does not.

[johnsonshiue]

Hi! The constant radius fillet in this case is a spline face. It is because the fillet edge is spline. I added a few features in the part to kind of explain how the fillet is created.

Look at the sweep surface in "Fillet on Compound Curves_surf.ipt." It is a bit similar to how the fillet is created along the edge. Please note that the fillet algorithm is much more comlpicated than the simple sweep. Basically, the circle is rolling along the spline edge. Inventor tries to simplify the geometry (utilizing analytical faces) if possible. In this case, an analytical face is not possible.

The reason why the intersecting edges from Revolution1 and Revolution2 in Sketch 5 get the center is because the faces are analytical (torus). And, the reason why the intersecting edge from Fillet1 does not get the center is because the face is spline. It is not because the fillet is less accurate. It is purely because the fillet face in this particular case has to be represented by a spline face, which was created by a constant radius arc rolling along a spline edge.

Thanks!

[kenjacques8585]

It is unfortunate that in this instance the centerpoint of the curve is lost even with the sweep command. What's more concerning is that a swept spline still retains this centerline.

[wilkhui]

Hi kenjacques8585,

Thanks for your posts, I hope I've understood your concerns with the below.

The fillet you mention in 'Fillet on Compound Curves.ipt' is not an approximation and the reason that a centre-point is not shown is because the fillet in that case is represented by an exact spline surface.

As Johnson points out, the fillet algorithm is much more complicated than just a swept arc and to compare the two wouldn't be a valid comparison. For the sake of completeness, an arc swept along a straight line appears to retain its centreline because in order to create valid topology it needs a prop edge (which isn't required for the fillet made from a spline surface in your example).

I hope this clears things up - does this address your concerns?

Please feel free to ask further questions!

Indy