How to create a 3d Shape from Curves ( Loft?)

[NiceNico]

Hi everbody,

I'm trying to model the following and can't get any further.

It is the blade of a Whopper Plopper lure. In Rhino I would loft it using several 3D curves, but in F360 I just can't get any further. Thats my progress so far:

Any advice would be appreciated.

Thanks everybody for their help.

File is attached.

Best,

Nico

[Drewpan]

Hi,

It is possible to create 3d sketches in fusion. They are not used often but people

do use them. I am currently doing a project where I required complex 3D curves

but I couldn't get anything accurate enough using 3D curves. The method that I

am using is very crude and may not be the best way but it does work and it creates

very accurate shapes.

My Project is a Ducted Fan that rotates at 20,000rpm. At those speeds the airfoil

shape of the blade is critical. The method that I use is this.

I start by creating a Front View Sketch of what the 3D curve looks like. This is the

Leading Edge of my fan blade.

Then I do the same with a Side View.

I do the same for the Trailing Edge.

I then change to Surface Mode and extrude these lines into Surfaces.

I then use the Thicken command and turn these surfaces into Bodies.

From here I do a Combine Intersect operation that creates the portion

of these bodies that intersect with each other.

Now I have two 3D shapes that I can use as Rails for a Loft.

The end result is a Blade with complex curves.

As I said, very crude - but it works.

The trick is to make the thickness of the surfaces thick enough to get

a usable rail. The Rail is the edge of the Body you just created. Lining

up the profiles to Loft is a little bit of a fiddle but you get it by zooming

right up close then click and drag if necessary.

Cheers

Andrew

[laughingcreek]

---

@Drewpan wrote:...I then use the Thicken command and turn these surfaces into Bodies.

...

---

Drew-I'm still at a loss as to why you thicken the surfaces.  it's an extra step that increases the possibility of selecting the wrong edge for the rail/profile.  just trim the surface and use the resulting edge.

[Drewpan]

Hi @laughingcreek 

For whatever reason I cannot get it to work that way. I do it this way because

I can then just select the edge of the resulting body and use this as a rail. It

works for me.

Cheers

Andrew

[laughingcreek · Accepted solution]

Nico-thought i'd take a stab at this over my morning coffee.  attached is a possible approach you could try.  let me know if you have questions-

[NiceNico]

Hi and thank you both @Drewpan  and @laughingcreek,

I thought modelling this would be similar to what I would do in Rhino- similar to what @Drewpan  did.

Somehow I had the impression that there is probably another way in Fusion and that's why I wanted to post the whole thing.
Thank you @laughingcreek for your interesting solution suggestion, which I would definitely never have thought of on my own.

I will try to remodel both for practice.

Thank you again and best regards,

Nico

[NiceNico]

Hi @laughingcreek,

could you tell me how to retunr the axis and plane system to the original position?

Couldn't find the setting.

Thanks again!

[laughingcreek]

I'm not at a computer right now.  It looks like you may have dragged a component out of alignment?  Are there 2 L shaped icons in the upper right corner of the screen? Hit the one that says something like "revert position."

FYI-a lot of information is conveyed to an experienced user from being able to see the whole screen.  Screen shots that include the entire window (including the top menus, the timeline at the bottom, and the browser on the side) can be helpful when answering questions like this.

[NiceNico]

sorry for the incomplete screenshot. I did not changed anything, just dowmloaded your file and this is how it appears on my end. Seems like local coordinate system, or something. I thought, you adapted it, to draw the geometry. I think I probably explained myself very poorly as well. 

[laughingcreek]

oh.  that's just the view cube being off.  I had changed it to get better lighting on the render.  weird that the grid aligns with the view cube and not the model origin.

anyway, reset the view cube from the pull down menu accessed by clicking on the little triangle next to the view cube-

[NiceNico]

perfect! That's it.

In the meantime I modelled the body:

Hope to get some time theses days to keep on the tail.

Thanks again and have a nice week!

[NiceNico]

Hi again @laughingcreek,

finally I had the time to try your approach and at least I got my head wrapped around - I think.
But I fail in the execution. If could have a look and give me a hint I would really appreciate - I already learnt a lot from your file ( about loft:))

Thanks and have a nice weekend,

Best,

Nico

[davebYYPCU]

Couple of things, 

Too many spline points in the sketches, and the height of the two splines in each sketch are "öut of level" on your file, compared to Alex's file.

He has a spline point at top dead centre of both splines, that are exactly Horizontal to a projected point in sketch 3. (Advanced level working)

Allows for the selection of a bottom, front and back body edges for the Patch command.  (Advanced level working)

You do not have a point at top dead centre in either sketch, and that makes the Extrude Cut leave a big curved cross over.

In other words, the front sketch in my pic is too high, and must line up with the side sketch height.

Might help...

[NiceNico]

It definitley helps! Thank you! 

I did not noticed the contraints in @laughingcreek 's sketch

It makes totally sense now. 

I managed to apply this in my file. The second sketch is constrained with the first:

Just one more question: How can I constraint the first sketch with the second one, like it Alex's example? 

In the image is the first sketch ans somehow it is coantrained with the one later created. How is this possible?

Thanks again and have a nice sunday!

Nico

[davebYYPCU]

Learn to love Purple Points (articles)

when starting a second sketch, Project the top point from sketch 1, then turn sketch 1 eyeball off.

You should see a purple point in sketch 2, if done right,  can’t see it happen if you keep sketch 1, visible.

Same for other needed alignments, wasn’t looking for those.

Draw the spline, 

make the top point horizontal with the purple point.

If you later edit the sketch 1 curve, sketch 2 top point will update. Doesn’t / can’t work in reverse.

You have a green point, (dangerous unfix it) not needed and will cause errors.

Might help…..

[NiceNico]

Thanks a lot! That definelty helps a lot. 

Think the the constraints are better now, they adapt accordingly just as in the file from Alex.

I am surprised how many things just happen in these two sketches - they turned out to be very well planned and strategic.

Something I am still missing - I hope I can get my hands on these (busy) days.

[davebYYPCU]

Almost - but you are not accurate enough with your setting up.  (You missed - Top Dead Centre - is required to make it work.)

You got this part correct.  Project to show the purple point, and horizontal, but

Earlier the splines were not equal in height.  You have not fixed that - earlier version did not create 2 bodies, now just a bit the other way, the two bodies are not touching.

Easy fix, edit both sketches and add a Horizontal to both the green tangent handles.

Now you can Loft the two separate body edges. (Not using patch because the loft works without a bottom connected edge / line.)

Might help...