how to create a surface loft from a line to a modified version of itself?

[maker9876]

Would like to create a surface loft between a curve and a modified version of the same curve that exists in a different plane. The basic curve is "A" in the screenshot below. Curve B is its projection in another plane.  A spline, C, has then been added to route a part of the curve B in a different way. Would then like to create a loft (surface) between curve A and the "new" version of curve B - which means, in effect, trimming out the section marked in purple and named "D". Can't figure out how to get this to work. Any suggestions?

[g-andresen]

Hi,

Please share the file.

So we don't have to redraw everything to give advice.

günther

[maker9876]

here it is: https://a360.co/2psd486

[wmhazzard]

In order to make a projected line editable you have to go back and edit the sketch, delete the projection altogether, then do a new projection and deselect the projection link box in the menu. You can then delete part of the projection. 

[TrippyLighting]

@wmhazzard You can also simply select the projected entity in the sketch, right-click and select "break link".

[laughingcreek]

seems like it would be nice to be able to trim the projected line in such a way that the short segments that are retained at the end are still linked projections.  the new section could then be constrained with a "tangent" or "smooth" constraint to the shorter line segments.

That wouldn't be necessary if fusion would allow lofting profiles and rails to be defined point to point along a curve, like solid works does.   

[TrippyLighting]

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@laughingcreek wrote:

seems like it would be nice to be able to trim the projected line in such a way that the short segments that are retained at the end are still linked projections.  the new section could then be constrained with a "tangent" or "smooth" constraint to the shorter line segments.

That wouldn't be necessary if fusion would allow lofting profiles and rails to be defined point to point along a curve, like solid works does.   

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Right, so build a surface from the projected spline, trim it where it needs to be trimmed and then loft to the edge.

It's a good bit more work, but but is doable.

[laughingcreek · Accepted solution]

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@TrippyLighting wrote: 

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... so build a surface from the projected spline, trim it where it needs to be trimmed and then loft to the edge...

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I'm not sure of the design intent of the OP, but obviously your approach is going to work better with fusions's tools than breaking the link on a projection is.

I imagine something like the attached?

@maker9876 -your working really hard to get this shape.  do you have any sketches or pics of an object showing your design intent?

[maker9876]

Hey some really interesting stuff here. Thanks a lot guys.

@laughingcreek  am working on an evolution of this design:  https://a360.co/2wrMUm0

Inside you'll see there are a number of parts - including some electronics. The new design needs, amongst other things, to wrap around that curved base and to contain an LED light strip (which is the bulge lower down in the prototype sketch posted earlier). The indented region struggling with here will have an NFC card reader located behind it and is for the NFC card to be sat in. All crazy stuff. 😉 Then divided into sections for 3d printing and assembly.

[laughingcreek]

still not sure what you were looking to do.  but attached is a model with a couple of ideas that might help you.

(p.s. - didn't open the assembly file.  they are a bit of a pain to deal with on my end)

[maker9876]

Elegant. Thank you @laughingcreek , plenty to learn from that.

Just one thing perplexed me: in the very first sketch there are some dimensions seemingly not attached to anything at one end? What's going on? Don't know how to do that!

[davebYYPCU]

They are diameter dimensions, based on the vertical centre line.

[laughingcreek]

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@maker9876 wrote:

... there are some dimensions seemingly not attached to anything at one end? What's going on? Don't know how to do that!

 I did that b/c I knew I was going to mirroring the surfaces, and I wanted to show the intended over all length after the mirror.   It's called a diameter dimension, and is usually used when making a profile to revolve so you can represent the diameter instead of the radius with the dims.

To apply it, while dimensioning, first select the line that will be the "axis" (or center line in this case), then select the other point, then right mouse click and select "diameter dimension" from the menu.

[maker9876]

Neat!

[TrippyLighting]

Looking at your timeline you might have a mine in there that can easily be tripped and cause you some headaches!

The good stuff:

You create a components, make sure they are activated and then create sketches and geometry.

The not so good stuff:

You use the move tool to move the component into some position and then use the position capture feature to keep it in that place. Not too bad yet because theoretically you can still delete the position capture feature once your component is properly joined to another one.

The bad stuff:

You create another component and reference the position captured component in a sketch. Now you cannot delete that position capture feature, because if you do stuff keeps breaking in the timeline.

Also, instead of lengthening that little motor by splitting, moving and extruding it back together, you can just simply use the move faces command 😉

BUT: Progress from your earlier designs is clearly recognizable. Keep going ...

[maker9876]

@TrippyLighting  that is an excellent trick with the faces. Didn't see that coming. Will try to do something about the moves. Since the whole design (the milled parts holding the axle, the pcb layout with its rotary encoder chip) is based around the position of the gears wasn't too comfortable on relying only on a joint either. Will maybe try and lock it down with a projection in a sketch, the link for which then gets broken and fixed.

@laughingcreek  had another go, trying to implement some of what learnt.

https://a360.co/2KCdaS9

Only managed to thicken the part to 1mm and not the desired 2mm. Understand that probably has something to do with the "sharper" edges in the design but don't see how can get rid of all of them?  

A way to go from an aesthetic perspective but a sound basis for the various functional requirements.

[laughingcreek]

Further refinement of the geometry will create better surfaces, that will be more likely to thicken to a reasonable amount.

It's a good idea to check your curvature combs when ever your doing surfacing.  in the sketch "primary verticals" you have a control point close to the endpoint of a spline.  always a red flag for me.  adding that point tends to push the curvature at the very end of the spline towards an infinite curvature situation, which always messes with surfacing operations down stream.

this is what the comb looks like after I fix it a bit

after this the body would thicken a little more-

next I lookes at the loft on the side.  the s curve in the top sweep was causing funkness in the loft because of the way it folded over-

I added a rail to tame that some-

thicken works a little better at this point, but still needs help.  moving on to the next surface, which was a sweep.  same problem with sharp curvature right at the end-

fixing that further improved thicken performance-

Attached is the file up to this point.  hope this helps some.

[maker9876]

Many thanks for that @laughingcreek . Any less of a complete explanation and would never have figured it out, but there were enough examples there that after a couple of hours of now have something that behaves quite well such that was able to make some design modifications as well. https://a360.co/2KCdaS9

In order to be able to 3d print sections of it efficiently, would like to introduce some "vaulting" in places that will be devoid of components on the inside. Typically solid structures at about 45 degrees to provide support to horizontal areas without using support material in the printer. A crude example of this would be as follows, to fill in the body above the slanting plane (for a slicer the area only needs to be properly bounded to be considered solid for printing):

Thought this would be easy (with new found skills!) but seems to be non-trivial because the plane cuts through a variety of surfaces at a variety of different angles and resultant patches, railed lofts and so forth seem to result in surfaces that are set at angles to the existing body that are unfriendly to making a proper join when thickened. Tried a bunch of approaches using surface modelling, solid modelling and hybrid forms but nothing seems to give a clean result. The vaulting is not meant to be a big part of the timeline, just an aid to printing. Is there a clever way to do this without going crazy on design?

[maker9876]

Just about to give up and suddenly may have something: a solid loft from a split internal face to a rectangle external to the body. Then throw away the outside part of the loft and combine.