Hello
I have been learning how to draw a rubber hose with a helical wire but now want to add the two bodies together. When I do so I get the following message
I have tried editing the dimension of the "Wire Profile" and editing the "Helix construction" but that didn't seem to sort the problem.
Any help much appreciated
Julian
I am not sure what the problem is in this case. I see no issues with the way this was constructed. The curvature of the intersection curve looks fine. Sweep profiles are perpendicular to the sweep paths. Looks all fine and should work.
@Phil.E who would I tag with this?
The problem is the seam of the wire twists as it goes along the path. If you use a sweep with guide surface to stop the twist it will work, see attached file.
Mark Hughes
Owner, Hughes Tooling
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You beat me to it. Thanks for putting up the solution.
I can easily point you to a thread where the Sweep with guide surface is the problem, and effectively prevents the user form completing his work.
As a user if you come across that thread you would never again look at the sweep with guide surface.
I see no reason what a simple sweep should great this problem. The pipe tool would actually be much more efficient tool to model this, but suffers form the same problem.
We've answered posts with these spiral "things" for years and I've never come across this. It did not even cross my mind.
We need more robust tools and that particularly relates to the loft and sweep tools!
@HughesTooling thanks for the help!
@P.S. Here is that thread. where the sweep with guide surface crates geometry garbage that isn't even tangent to itself. I works as a solution in this case, but absolutely miserably fails in another. As a user, how would you navigate this ?
@HughesTooling wrote:
The problem is the seam of the wire twists as it goes along the path. I
The sweep profile is circular and as such that twisting of the seam should't be a problem.
We've created all sorts of coil structures before the sweep with guide surface was introduced and I don't recall this being a problem.
@TrippyLighting wrote:
@HughesTooling wrote:
The problem is the seam of the wire twists as it goes along the path. I
The sweep profile is circular and as such that twisting of the seam should't be a problem.
We've created all sorts of coil structures before the sweep with guide surface was introduced and I don't recall this being a problem.
I usually need to create parts that are not circular so the twist has always been a problem for what I do, just thought I see if it was the problem here. With that said I also always try and use Path + Guide Rail as it usually creates a cleaner surface but that didn't want to work if I tried to use the tube's path as the guide rail. Might get better results with 2 helixes. Using the guide surface is actually splitting the coil in 360° sections.
Mark Hughes
Owner, Hughes Tooling
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@jdpreynolds One bit of advice after looking at this again. Really you should use the edge of the surface rather than using Project - Include 3D Geometry because the surface edge is calculated to a tighter tolerance.
@Phil.E I just tried this again using the 2 edges of the swept surface to create the coil without the twist but now it fails to combine. So it's not the twist that's the problem. Using the guide surface only creates a set of 360° sections that are not as nice a solution but I guess more simple for the combine? I've attached the design with the new cleaner coil and the failed combine.
EDIT. Forgot to attach file, now added.
Mark Hughes
Owner, Hughes Tooling
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Is the file attached to your last post? (didn't see it)
Thanks for testing around this. I'll have to defer to the modeling team that handles face to face intersections like this and send them the information now.
@TrippyLighting - I think it is a bit of an over-generalization to say "you would never again look at the sweep with guide surface". Certainly you have found a case where it generates questionable geometry, but I think it is a bit extreme to imply that you should never use that feature for anything. There are plenty of cases where sweep with a guide surface generates reasonable geometry. Certainly, you, personally, are free to never use it again, but I'm not sure that I would recommend that to everyone.
@jeff_strater I think you misunderstood what I was trying to convey.
I understand that this is a single case where this happens to cause a problem. As I’ve already said, we’ve been making all sorts of coils happily before the sweep with guide surface was even around.
Look at the other thread and look at the curvature at the outer edges of the wedge. In that case, the sweep with surface creates surface patches with edges which aren’t even tangent to each other. As a relatively inexperienced user - that covers 80-90% of Fusion users - If you identified that as the problem, would you try that as a solution in this case?
I doubt you would.
I appreciate that @HughesTooling posted this solution, and personally I will use it if I come across problems again.
I don’t think anything speaks against looking into why this problem exists and perhaps creating a more robust solution.
@Phil.E wrote:
Is the file attached to your last post? (didn't see it)
Thanks for testing around this. I'll have to defer to the modeling team that handles face to face intersections like this and send them the information now.
@Phil.E Sorry thought I'd attached it. Latest version attached to this post.
Mark Hughes
Owner, Hughes Tooling
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@jdpreynolds wrote:
Thanks for all of your replys will now attempt to re sweep the profile using a guide rail Will be great if this is something that Fusion is able to rectify!
Regards
Julian
Initially I used a guide surface and that worked but broke the coil up into 360° sections. I didn't really like that so thought I'd try with a guide rail using the helical surface edges. That created an nice coil without a twisting seam but still failed to combine, which points to the seam not being the problem but the complexity of the coil.
Mark Hughes
Owner, Hughes Tooling
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@Phil.E I noticed the menu when you right click the combine icon in the timeline with an error is missing the edit option! It should be above the Configure option.
Mark Hughes
Owner, Hughes Tooling
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Not sure, but it looks like some kind of corner case.
In a simple example, there is an edit command.
Hi Mr JDPReynolds, Sweepers, both Content or Not,
I have gibed out the 6-year-old design with an underlying API blob simulating phone cable cords; old-fashioned ones, not the WiFi connection. Consider visit a museum or the Oval Office if you want to see one.
If I recall correctly, it was one of my first grilling encounters with meanders of F360 API … which, after a blood&sweet&loss-of-hair … resulted in something workable … the object simulating bending a telephone cord dynamically, allowing for its extension, twisting and selection of bending strategies. One of them calculated a 'helical' twist around tightly bent sections, accounting for a cable geometry and avoiding a sweep intersection.
So, I dug out the design … to check it in the context of the post with the title as paraphrased by Mr LippyLighting – "We've answered posts with these spiral "things" for years …" (well said!)
The test design opened correctly… but the underlying API object refused to cooperate. I have not spent too much time investigating what I poorly stitched years ago because… the current UI Sweep Feature also failed with the 6-year-old geometry supplied. Thus, the problem seems to have fungi roots … difficult to trace … and more likely than not, rotten mycorrhiza is on my side also. I would do the task differently now, … anyway.
In order to somehow put a memory stamp on the 6-years-old event and the current encounter with "spiral things" and also encourage TF360 to labour on the issue more intensely, I am attaching a 6-years-old flexi cable example (the excerpt from more extensive design) with underlying input geometry as my contribution to … the potentially satisfactory solution. I hope that the Surface Sheriff will notice how smooth the examples are!
Hopefully, the next 6-years should be enough for TF360 to gib out the practical method of generating a "spiral thing". Too long? What is the 6-years?… the last one went soooo fast!
Attached files:
SpiralThing.f3d F3D ( 14MB) https://a360.co/3RUx0dE
SpiralThing_arcd.png 4K_stereo ( 3.3MB) https://a360.co/45V3kDk
SpiralThing_mono.png 4K_mono ( 2.6MB) https://a360.co/3xLQoTw
SpiralThing_arcd.mp4 4K_stereo ( 46MB) https://a360.co/3XOdAuO
SpiralThing_mono.mp4 4K_mono ( 25MB) https://a360.co/4eRVApu
Postface:
The spiral-type topological object requires a 'dense' numerical definition of their surfaces.
It is a challenge, as in the Fusion, the traditional approach creates a bulky, costly, unresponsive design entity.
What would be the alternative then?
The current mighty computing hardware is vastly underutilized, particularly in the Ultimate Fusion processes. I am unsure what is beyond Ultimate, probably … Nihilness; thus, who would like to progress there? …if one can not go beyond …, start the journey… from scratch … defining spiral-thing as a run-time, close to a silicon procedure with only a few basic and dynamic parameters. The quite different CAD kernel constitution paradigms…
Regards
MichaelT
P.S.
I adopted the phrase 'spiral thing' wildly&widely throughout the post. It is so ... appropriate!
I hope that you don't mind Mr TrippyLighting :)!
