Joining Line Segments

[Anonymous]

I have an object made up of a set of curves and then joined that were drawn in Turbo Cad a while ago and when I import the design into F360 the program treats each segment as a separate element.

The has to be some means to join line segments.

Yes I searched the archives and find lots of old posts saying it can't be done and everyone sort of agreeing this would be a good feature.

[lichtzeichenanlage]

This function is not available in Fusion 360. You can (and should) (fully) constrain your sketches but this will not change anything about the segments. It just results in a stable design. 

[jeff_strater]

@Anonymous - can you help me understand why you need these curves to be a single object?  What operation can you not do in Fusion with them as separate items?  This is the thing I have not yet understood about this discussion.  Just trying to better understand the request.  Thanks.

[TheCADWhisperer]

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@jeff_strater wrote:

  This is the thing I have not yet understood about this discussion. 

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Sketch Blocks

[Anonymous]

Screen shot from turbo cad.  The irregular form is treated as a single line.

Saved in a variety of formats, and when imported into F360 it treats the curve as 5 separate segments.

I need to extrude the object to do a test part in 3D printer and subsequently have the part cut out of aluminum on a water jet.

I really do not want to go through the ordeal of trying to re-draw this in F260

Bill

[lichtzeichenanlage]

What formats? Can you share the files here? Segmented lines shouldn't be a problem in Fusion 360 if you e.g. want to extrude it. 

[davebYYPCU]

When imported, does Fusion create the three orange sketch profiles?

For extruding that shape you need just the outer profile for solid, and chain select will do surfaces.

But if the original file is deficient or not compatible, not Fusions fault.  Doubt that you would need a redraw, either way.

Might help....

[jeff_strater]

whoa there...  Sketch blocks are a totally different requirement than what I've heard before about "joining line segments".  I've always heard this expressed as a kind of "composite curve", and I don't see the need for such a thing in Fusion.  Yes, sketch blocks would be useful, in that they can be instanced, etc, but that's different

[jeff_strater]

right.  You should be able to extrude that whole shape, regardless of whether it is one curve or 5.  The fact that Fusion is not recognizing it as a valid profile is the problem, not the number of curves.  If you can share your f3d here, we can take a look at it.  Most likely, there is some gap between the curves, or else it is not exactly planar.  But, share it, and we'll take a look...

[TheCADWhisperer]

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@Anonymous wrote:

I really do not want to go through the ordeal of trying to re-draw this in F360.

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Attach your file here and I will do it for you.

[Claus_J]

Jeff, I would certainly like to give my view, I'm also a TurboCad/ViaCad/Shark user and just used to be able to add, join, edit and convert anything to anything. See an edge you like, convert it to a curve and continue to shape it. Don't like a CV spline, convert it to bezier. It's likely more an artists fuzzy way of creating than an engineers and that whole "I want freedom" habit is what clashes with Fusion and the very opinionated and much appreciated mentors here. I'm sure to get bashed again for writing this. So as an example I may start with a few lines and fillet the corners and in SharkCad I will maybe join those elements and start manipulating the control points of the resulting spline and may end up with something completely different. It will probably make your head explode but it gets me to a result very quickly and with a lot of freedom, it's probably an illustrators approach. So to your question "why" I would like to respond "why not".

[Anonymous]

I thought I had posted these last night, don't see the message.  Here is a repeat.

Bill

[jeff_strater · Accepted solution]

Thanks, @Anonymous - the problem is what I suspected.  There is a break in the geometry from TurboCAD.  I used the technique here:  find-break-in-sketch-geometry to isolate it:

Zooming in, you can see the break:

Depending on what you want to do, there are several ways to fix this.  I would just create a small line segment:

and the profile is recognized:

Then, I noticed that there are two sketches here (presumably 2 layers in the original).  There are several ways to deal with that, assuming the result is a single body with cutouts.  I would just do 2 extrudes - one of the outer body, and one of the cutouts.

[Anonymous]

OK, this helps immensely.  I assumed all along that it might be me, I just found it odd that the join function (which obviously didn't work in TC on this one) was not part of F360

I guess when I had the parts jetted a while ago, they fixed the issue and never commented about it.  In the past they have always bounced it back to me on the rare occasions that an issue like this slipped through.

I jumped ship from TC to F360 when I got my 3D printer about 2 1/2 years ago.  While the learning process for me a was a bit difficult at first, everything I have drawn from scratch in F360 was fairly easy.  I actually prefer F360.

Off to go practice and many thanks!

Bill

[jeff_strater]

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@Claus_J wrote:

Jeff, I would certainly like to give my view, I'm also a TurboCad/ViaCad/Shark user and just used to be able to add, join, edit and convert anything to anything. See an edge you like, convert it to a curve and continue to shape it. Don't like a CV spline, convert it to bezier. It's likely more an artists fuzzy way of creating than an engineers and that whole "I want freedom" habit is what clashes with Fusion and the very opinionated and much appreciated mentors here. I'm sure to get bashed again for writing this. So as an example I may start with a few lines and fillet the corners and in SharkCad I will maybe join those elements and start manipulating the control points of the resulting spline and may end up with something completely different. It will probably make your head explode but it gets me to a result very quickly and with a lot of freedom, it's probably an illustrators approach. So to your question "why" I would like to respond "why not".

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fair enough.  I actually do see value in a "fit a single spline curve to the selected sketch curves".  That, of course, has some limitations (what do we do with sharp corners?), and may require some fit tolerance as input.  Perhaps I was assuming too much from other threads, but I've often heard this requirement expressed as some kind of "composite curve" object, which could be composed of lines, arcs, splines, etc.  That is the requirement that, in my view, doesn't make sense in Fusion.  Given that we can build profiles and paths out of a set of connected curves, I don't see the value that a composite curve would give you.  

Finally:  The answer to "why not?" is limited resources.  We only have so much ability to add things to Fusion.  We should bias our priorities around those things that either cannot be accomplished at all today in Fusion (e.g. designing a cam follower), or are otherwise blocking building real-world designs (assembly performance).  There's another argument about simply adding too much stuff to Fusion, resulting in a cluttered experience.  We've tried (though I feel every day that we are losing this battle) to keep Fusion's "surface area" as small as possible, and still allow our customers to do real design.  We've all had experience with software that is just overwhelming in terms of the total number of commands/workspaces/etc that are available.  So, if there are entire concepts that we can avoid, I, personally, will push to do so.  I don't always get my way...  

[Claus_J]

Jeff, that’s actually a very good answer. I know for a fact that people coming from Adobe Illustrator will certainly want to join two straight lines and not understand that it’s not going to work with the sharp corner. That’s part of the learning that you don’t have to have everything as a single shape or curve and it’s not what I suggest.

I’ll try to describe a situation I often find myself in. Lets say I made a bottle from a large cylinder and a smaller one and make a loft between them to create a smooth transition. At some point I decide I need to tweek the whole bottle profile only I don’t have a sketched profile because I started with two cylinders and a loft. So I will cut the bottle in half and extract the outline which will be two straight lines from the cylinders and a spline from the lofted transition. I then join the 3 elements to create a single spline. It will be a mess of points and probably approximated but it’s a starting point for a new sketched profile. Of course for simple things like a bottle I can simply trace over the elements and create a profile from scratch, but this is just an example off the top of my head.

I would say that this feature should come with the ability to convert to fit point spline, at least for my use since the CV splines are difficult to simplify without loosing the overall shape.

[davebYYPCU]

Primitives are not a short cut, they have limitations, not many here would recommend your example workflow,  for the problem you mention, 

revolving a profile in the first place allows unlimited editing.

Might help....

[Claus_J]

Dave, thanks for your advice but I was just creating an example. The point I’m trying to make is that in my job, what I start with is seldom what I end up with. But it really speeds up the process of going through iterations if you can bring something with you from the previous step, like in the bottle example. If I know from the beginning I’m going to end up with a curved bottle shape and a revolved body I will of course start with a profile. Btw I’m willing to accept that my workflow is “broken” however a cad app that has this crazy free form t-spline tool might consider giving user some freedom in the creation of curves too. Anyway I think I got my message across.

[zalexzperez]

I believe pattern on path misbehaves if your path is a collection of line segments...

[Anonymous]

Actually the issue, which I did not catch, was the part was not closed.
Small gap between two segments tha could be seen when zoomed a bunch,
was causing F360 to not treat it as a closed part.

Fixed the little bugger and all was well.

Beevo