Square box edges - arc and fillet

[Anonymous]

Hi!

I have been working on a very simple (or so I thought) model for a joint (which is essentially a box), that will join up with some rods, see picture. I've applied a fillet on the edges that need a smooth edge, however there are two planes which require a flat surface but with radius corners which should taper smoothly into the vertical edge. I am referring here to the corners I marked in red. I used the sketch view to position two arcs with the appropriate radius on the edges thinking I could just remove the surplus above or pull the square plane into a curve, but I just can't work out how to solve this sadly.

I gather it is probably something really obvious, like a tool I may not have used before or a different workflow. Any tips?

Really stuck with this, any help would be great!

[TrippyLighting]

In Fusion  360 you’ll have to do this manually, possibly in the Patch workspace. There is currently no tool that allows you to chamfer or fillet a vertex, which is what you’d need in this case.

Hwever , I’d also ask myself how you would want to manufacture such a fillet or chamfer and whether it would really be to be part of the model.

[Anonymous · Accepted solution]

@Anonymous,

I wasn't exactly clear on the geometry you were trying to achieve from your description. However, the model looks to be a corner connector that will need to fit up with extruded tubing. I modeled two possible solutions. Have a look and see if either of these are a solution.

Blessings,

SkillCoach

Extruded cutdiagonal midplane with sketched arc from face projected onto it.Revolved cut using vertical edge as axis.

[Anonymous]

Thanks for the quick responses, the community spirit is so encouraging!

@AnonymousThank you for those solutions, this is exactly what I was looking for! This has been so helpful. Your second example is certainly the most elegant. I will be reviewing both ways in detail to understand the steps involved. I will report back if I have some more questions, thanks!

[Anonymous]

@Anonymous,

I'm glad I could be of help. Given that I have coached you to a solution could you please mark this thread to a status of "Solved."

[Anonymous]

Hi @Anonymous, have been playing around with the example given, and I think I get the steps involved to get to what I need. However, I'm bit lost in terms of the arc you created in sketch 5, can't manage to make it the same radius to match the ones on the side. Would you be able to give any guidance?

[Anonymous]

@Anonymous,

1) The "arc" in Sketch5 is an Include 3D Geometry projection. I selected the arc in Sketch2 and projected it onto construction Plane1.

2) Because Plane1 is on a 45degree it causes the projected arc to look elliptical. However, when extruded outward from Plane1 the geometry perfectly matches the shape of Sketch2 and Sketch3 as it exits the planes each sketch is drawn on.

3) Because Sketch5 is a child of Sketch2 whenever the dimensional value of Sketch2 is changed Sketch5 follows. 

I trust this explanation makes everything come clear to you. I'd appreciate you marking this post as "Successfully Solved" if all is good.

Blessings,

vhaley_skillcoach

Include 3D Geometry used to achieve the arc segment in Sketch5

[Anonymous]

Hi guys, that was an interesting discussion.

Now, what if I want a cube, leave the edges sharp and only round off the tips or vertex at the corners?

I have tried to attach a a construction plan to the vertex in order to be able to extrude cut off the tip as a start but didn't manage...

Any ideas?

Thank you so much

[TrippyLighting]

As I've mentioned previously Fusion 360 does not have a vertex fillet, so you'll have to do that manually.

That'll likely be using the tools in the patch work space.

I simply sketched arcs in the corners and split the corner surfaces with that arc and deleted the three triangular pieces. Then I used the patch tool to create the "fillet".

This is not really the proper method, but the proper surfacing method is even more labor intensive and I've not tried that yet in Fusion 360. You'd have to create several curves and several lofts.

The patch tool creates pretty ugly surfaces and in this case they are outright terrible. In general a vertex fillet will create a NURBS surface that has to collapse into a singularity in one corner and that i generally not a good idea with NURBS surfaces.

[Anonymous]

Great. I tired the same method with arcs on each of the three surfaces and extrude cut with them but that didn’t work. I will try your method later. Thanks for the reply.

Oliver

[Anonymous]

Your solution looks great. will have to try that.

This morning, I had the idea of drilling a large hole into the vertex and thereby at least flattening it, so I could try applying a fillet around it.

But I have not been able to fix a construction plane on the vertex or a construction line trough it...

Best wishes

[Anonymous]

here a way I found to cut the tip of the cube off (easy I guess for the pros but maybe helpful for another rookie like me):

1) apply one plane through 3 tips of the cube or points located on the edges

2 offset another plane towards the corner that you can the use to cut the latter off

3) patch the hole

unfortunately, you can't fillet the edges resulting from that operation so you are stuck with sharp edges... will keep posting if I find another solution.