topic Re: Why is this shape not closed? in Fusion Design, Validate & Document Forum

Why is this shape not closed?

Anonymous — Sun, 20 Nov 2016 09:00:55 GMT

I created two horizontal lines on two different sketch planes and then joined the line ends.

I was playing with this yesterday and the horizontal lines turned into horizontal lines with weird dashed lines underneath that could not be deleted?

Re: Why is this shape not closed?

davebYYPCU — Sun, 20 Nov 2016 10:03:23 GMT

Are you sure you snapped to each endpoint?

The two dark dots indicate they may not be coincident. A closed profile will turn orange, unless you turn that function off in the sketch pallet.

The way you describe the creation of the articles, do you have three sketches, "two sketches on different planes", and a third sketch to join the end points?

I may be wrong here, but profiles should be on the same plane, so I would expect all 4 lines in one sketch, on a plane at an angle to give the desired outcome, with all endpoints coincident.

Might help.

Re: Why is this shape not closed?

HughesTooling — Sun, 20 Nov 2016 10:35:39 GMT

If I understand correctly you have 2 sketches with lines in both. You can not make a closed profile with curves in different sketches, in this sort of situation you'll need to use project include 3d geometry so all the curves are in the same sketch.

Mark

Re: Why is this shape not closed?

Anonymous — Sun, 20 Nov 2016 11:00:22 GMT

Thanks for the replies; this is confusing to me as the program should know the shape is closed regardless of how many sketches we use as we have the 3d sketch option.

Re: Why is this shape not closed?

HughesTooling — Sun, 20 Nov 2016 11:20:47 GMT

What if you had 10 sketches on the XY plane with lots of overlapping curves? If it worked the way you want you'd have all sorts of closed profiles generated between the sketches and it would be a nightmare.

After reading a few of your posts are you sure Fusion's the right program for you, you seem to want to fight against the way it works. Fusion works pretty much the same way most solid modelers work and have worked for 25+ years, it's not new. It sounds like you are used to Autocad or Rhino, they work differently plane and simple, if you try and make Fusion work like those sort of programs you're just going to get frustrated and waste time. An analogy for you, it's like you've moved to a foreign country and you're complaining everyone's driving on the wrong side of the road and speaking the wrong language but it's not them it's you!

Mark

Re: Why is this shape not closed?

Anonymous — Sun, 20 Nov 2016 11:49:19 GMT

Lol Mark, this is how engineers work, we discuss things and from those discussions come solutions and enhancements.

I gave Rhino a brief test around two years ago and have not touched AutoCAD since release.........????

The attached screen shot shows a shape that was created on the ground plane and in free space.

I can create surfaces or extrude solids from that shape and the program used is a low end solid modeller from 2010.

A major difference with Fusion 360 is that if the program does not recognise the shape as a closed shape then it cannot be extruded.

Whereas with the program I used for the screen shot did not recognise the shapes as closed but the shapes could be extruded or used to create a surface by individually selecting a set of curves with the shift key.

Re: Why is this shape not closed?

TrippyLighting — Sun, 20 Nov 2016 14:07:10 GMT

@Anonymous wrote:

Lol Mark, this is how engineers work, we discuss things and from those discussions come solutions and enhancements.

True. In this case it would not be an enhancement though!

The sketch engine has to perform calculations whether a sketch is closed. These calculation only need to be done when actively editing a sketch.

If the sketch engine would also need to show a closed profile outside of editing a sketch it would have to continuously re-evaluate every sketch and every possible connection between every sketch. That would induce quite a performance penalty.

Re: Why is this shape not closed?

jeff_strater — Sun, 20 Nov 2016 16:34:04 GMT

to add to what @HughesTooling and @TrippyLighting said, I'll offer one other reason why region detection is limited to a single sketch: To allow you to segregate regions by sketch.

A sketch is really just a container of curves and points. This allows you to create groupings that make sense to you. If you want all those lines to participate in regions, why would you not want them in the same sketch?

The performance point that Peter makes is a good one. If Fusion had to look around at other sketches to do region detection it could get quite expensive, and lead to failures. Consider this case.

Start with a simple sketch:

Extrude the results, and create one sketch on one face:

Create another on the other face:

If Fusion supported this kind of region detection, the overlap of those circles would be a valid sketch region:

And you could, for example, Extrude it. But, if you go back and edit the original sketch so that those faces are no longer coplanar:

then Fusion would have to figure that out, by looking at each sketch in the entire design, and reject those that are not coplanar. It would be quite expensive:

Anyway, this is a good discussion, and I want to encourage more of these kinds of discussions.

Jeff

Re: Why is this shape not closed?

HughesTooling — Sun, 20 Nov 2016 20:00:17 GMT

@Anonymous wrote:

A major difference with Fusion 360 is that if the program does not recognise the shape as a closed shape then it cannot be extruded.

Whereas with the program I used for the screen shot did not recognise the shapes as closed but the shapes could be extruded or used to create a surface by individually selecting a set of curves with the shift key.

You can use curves from different sketches and even edges to create a patch in the patch workspace then thicken.

Mark

Re: Why is this shape not closed?

Anonymous — Sun, 20 Nov 2016 20:27:58 GMT

Thanks for that Jeff, I am on record as saying that something about Fusion 360 has been confusing me and another Autodesk employee asked what.

At that time I did not have a definite answer and I think it’s fair to say that the Sketch function in Fusion 360 has caused many new users confusion.

After reading the replies and thinking about it I have come to the conclusion that my confusion is caused by the 3D sketch capability.

On one hand my brain knows there is 3D capability but to use the Sketch function I must enter a 2D world.

3D Sketch to me means I can sketch in a 3D environment, in other words I would not have to leave the modelling workspace to sketch and that’s what has been causing me confusion (I think).

Don’t get me wrong, I actually love the way the Sketch function is laid out and have found it very productive of late.

In the attached screen shot I copied the angular line, then moved it off the sketch plane, connected the ends and up with a closed shape, who knows, it might come in handy and it’s fun to try things.