Radius Bug and more

[eric_strebel]

I have created a very simple three point ark with a 94mm radius and extruded it to 102mm in length. I then wish to fillet the edge to create this simple pill shape. I am able to select one upper edge and radius it to exactly 94mm and get a wonderful circular end cap. However is I select both edges I gat a fail and am only able to radius to 93mm before the operation fails. It does not matter what end I choose (second image), I can only radius one of them to the correct perfect radius. I have done this sucessfulky in the past, not sure why this is not working. Also, now when I go to take a screen shot of the this issue and press control option 4 the radius gets undone and I can take screen shot to show you, so you have an OSX hot key issue as well (first image)

Good luck.

[TrippyLighting]

A differnt more efficient methodof creatingthe pill shape would be to draw half of the pill

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@eric_strebel wrote:

I have created a very simple three point ark with a 94mm radius and extruded it to 102mm in length. I then wish to fillet the edge to create this simple pill shape. I am able to select one upper edge and radius it to exactly 94mm and get a wonderful circular end cap. However is I select both edges I gat a fail and am only able to radius to 93mm before the operation fails. It does not matter what end I choose (second image), I can only radius one of them to the correct perfect radius. I have done this sucessfulky in the past, not sure why this is not working. Also, now when I go to take a screen shot of the this issue and press control option 4 the radius gets undone and I can take screen shot to show you, so you have an OSX hot key issue as well (first image)

Good luck.

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profile and then revolve it around the center axis.

[TrippyLighting]

I must have pressed the wrong button too early.

What I wrote above is of course just another way of creating the shape that is more likely not to return errors. That does not mean the way you create the shape should return an error.

[eric_strebel]

Yes, perhaps. Remeber however its not actaully half a pill, I need to do mutiple design variations at varius heights for my client. So, I need to be able to make the model adjustable in its initial radius/ height. Either way, Fusion has some sort of an issue going on that nees to be investigated.

Also, I am curious why the transition/ tangent area from radius to straight portion of the model is so harsh. You can really see this in the model rendering. I recently has some REN shape cut of a similar model and foud the transition to be medeocre at best.

[eric_strebel]

Please feel free to suggest and alternative way to making the shape.

Thanks

[TrippyLighting]

I don't have access to my machine right now ( kid is gaming on it 🙂  but will post something tonight.

The transition you are describing as harsh is not due to a limitation of Fusion but due to the limitation of your design. The transition from a radius into a stright surface is a tangent or G1 transition. In order to provide a better visually appealing transition you need at least a G2 or better a G3 transition. Here's a link that exxplains this.

@cekuhnen can tell you how to do that and I hope he'll chime in. That will make the highly revlective surface of your "pill" more visually attractive.

[cekuhnen]

LOL while you were writing I was doing my post already.

G1 transitions are as stated harsh - or what I would consider engineer grade design work 😉 they look boring while being geometrically sound.

What you need is to use the G2 option. But here Fusion lacks the ability to weight G1 and G2.

Also such shapes while looking easy are incredible hard. Plane nose type shapes are crazy complex in nurbs because you want to get a smooth

result and not that typical click and forget G1 stuff.

The form is stupid and cannot include images I uploaded so here is archive only.

But the process is this:

1. build a frame work of sketches for side top front view with arcs (g1 bahhh)

2. make a new sketch for top view with a spline that is smooth constraint to the start and end (g2 yeah)

3. edit the spline handles to make it close to the arc in top sketch

4. make a new sketch for the side view and again create a spline that is smooth constraint to the top end (g2 again)

5. break the front arc into two parts so you can extrude each half as a surface

6. use each broken front arc to extrude half of the profile into a surface

The whole idea is that now you have two half extrusion which provide arc edges you can use for loft.

Loft in Fusion can work like sweep so you start loft with doing this.

1. edge: 1st surface edge

2. edge: side view spline

3. edge: 2nd surface edge 

4. rail: top view spline

Set edge 1 and 3 to smooth

DONE

[cekuhnen]

second approach would be TSplines

Make again sketches for frame work and then sculpt the shapes into it.

You build a much bigger shape with a quad ball

sculpt the ends

mirror it

and then trim loft stitch everything together

[eric_strebel]

Claas,

Lets chat in the morning quickly. I think we chatted about some solutions previously. Thanks

[cekuhnen]

Sure - call my tech support line. 😉