best way to make custom threading in Fusion?

[cekuhnen]

Normaly in a NURBS modeler or such I use a profile aling a spiral function and how would you do this in Fusion?

my main tricky question is the star and end where the threading flows into the cylinder body.

1 profile revolved with a screw distance

2 modeled solid threading body and sculpted threading start and end

3 threading added to the bottle botle

[cekuhnen]

@Anonymous

Fusion is not able to draw 3D sketches like that - yep it is true ...

So what you have to use instead is make the solid geometry and from that you

can cut the shape you need

convert the brep to tsplines for further sculpting

3d include the edge of the helix as a 3d sketch

[Anonymous]

Hi there, yeah to do that make a sketch defined on any plane (doesn't matter, since will be making a 3D sketch), and be sure in the Sketch Pallete that 3D Sketch is checkmarked.  Then you can just go to Sketch > Project/Include > Include 3D Geometry and select one of the edges of a helix made by the Create > Coil tool in the Model environment, specifically a coil with the square profile choice. 

Let us know if you run into trouble!

Jesse

[Anonymous]

Thank you for your reply, @cekuhnen and @Anonymous.

>Fusion is not able to draw 3D sketches like that

Oh...It is inconvenience...．

>yeah to do that make a sketch defined on any plane (doesn't matter, since will be making a 3D sketch), and be sure in the Sketch Pallete that 3D Sketch is checkmarked.  Then you can just go to Sketch > Project/Include > Include 3D Geometry and select one of the edges of a helix made by the Create > Coil tool in the Model environment, specifically a coil with the square profile choice. 

Thank you for showing the procedure. It is very kind for me.

I successfully create 3D coil sketch by following your advices.

However, please let me ask you two more questions about customthreads file.

The first one, in Sketch5, there are seven points on the coil sketch and Sketch5 is drawn based on one of them.

How did you do this? I couldn't create loft because of inconsistency in my sketch imitating Sketch2, 4 and 5 of customthreads.

I think the cause of this is that I couldn't indicate the point on coil sketch when I drew second trapezoid which is equivalent to the trapezoid in Sketch5 of customthreads.

Next, is plane3 necessary for anything? 

Best regrads

[cekuhnen]

yeah welcome to those typical 2d sketch engines when it comes to true 3d sketching they show the limited usabilities to work fast.

to answer your question about finding the point you can create a c plane as needed and then create a new sketch on that plane and use project/include > intersect to intersect the coil sketch.

[Anonymous]

Hi, I wanted to mention for almost all custom threads I now recommend Cekuhnen's approach, which is much easier and gets better results than using a loft.  Using Chamfer tool there are two side and side and angle options to get a wide range of angles on a square thread made by the Coil tool.  You can also use Press/Pull tool to further modify the thread.

Good luck!

Jesse

[cekuhnen]

@Anonymous Ah it is not my pure idea I just took the tip with the coil a step further exploring how model the start and end parts! You started his with suggesting the coil with champfer compo!

However this approach only works well if you work with some square like stock you want to champfer. More eliptical profiles already start to give you head pain.

This type of custom modeling clearly shows how limited currently Fusions modeling tools for such parts are. And I hope in the future to see usable 3D sketching be implemented.

Everything else is just labor intensive work arounds.

So I still think that actually the spiral and then TS sweep is still a valid and only option for more complex custom threadings - like how I build in it Blender with sub-d.

[Anonymous]

Claas, you reminded me about your new two rail sweep feature!  This is a perfect tool for making very unique custom threads.  It simply needs a single profile to sweep, and two helical rails taken from two edges of a Coil, or just copy-pasting the first helical curve.  The two rails insure there is no twisting as was the case with a single rail sweep.

Works really great, only thing I noticed is it's picky which curves are chosen as path and rail for the 2 rail sweep (actually called Path + Guide rail under the options of the sweep tool, both in Model and Patch environments).  Not immediately evident to me why it's wanting a particular order, as both 3d helical curves look the same to me.  But it works! 🙂

(NOTES:  You can also now use Construction Plane along Path without worrying about axis slight twisting)

Jesse

[LMD001]

Hello Jesse,

The CPlane On Path still twists depending on where it is located on the path.

The "0" and "1" positions seem OK but the Plane rotates on intermediate positions.

Before this behavior was also seen on circular paths, this has been fixed several updates ago but on 3D paths, the twisting still occurs.

As you mention in your post the single rail sweep will twist but also Pattern on Path seems to be affected.

Nice "thread"  though!

Best regards,

Ludo

[Anonymous]

Hi Ludo, thanks for clarifying that, I wasn't very clear about what I meant was since now using two rails, one doesn't care about rotation of the construction plane along path and consequently sketch axises defined on that plane, since now using two external points (Intersect points) as reference instead of axises. 

That's interesting such rotation used to occur around a circle but now that's fixed.  I just noticed like you said Pattern on Path does rotate around a curved 3D path like a helix.  Too bad you can't select two paths for that!

Yeah, I love threads like this 😉

Jesse

[cekuhnen]

@Anonymous

that new sweep function is pretty great - but what Fusion needs is just the ability to draw and edit 3d curves the same way every other surfacing tool can do.

I never understood why software companies think those crippled 3D sketches are useful to designers.

Siemens NX is a pretty good example of how to do it.

You can either sketch like in 2D with 2D sketch solvers.

And you can create 3D curves which act and behave like drawing in Rhino Alias etc.

Obviously such 3D curves cannot use 2D sketch solvers but thats not need an issue in many cases.

[Anonymous]

both links don't exist....

Sorry, the file you have requested does not exist.

Make sure that you have the correct URL and the file exist

[JDMather]

---

@Anonymous wrote:

Make sure that you have the correct URL and the file exist

---

Given that you have responded to an ancient thread - it might be best to start a new thread and link back to this one for reference.

[Anonymous]

i was responding to the broken link that has been shared but it looks like it was taken away.

noted on the new thread if its ancient.

thanks