Improving Lofting

christian_29

There are a couple of features missing related to lofting.  

• Need ability to create multiple planes at a given offset or angle.
• Need ability to join splines, lines and arcs that are touching or intersecting to create a continuous spline. 
• Need ability to "straighten" joined splines to get tangent transitions. Basically remove "kinks".
• Need ability to dynamically move spline, line and arc points of the profiles that generate the loft to dynamically adjust the loft shape.

I'm working on some boat hull design were there are no straight lines and everything is curved. Also these types of features improve the ability to create more natural shapes that don't have straight lines or flat/cylindrical surfaces.

christian_29

Missed a few more:

• Need ability to import curves. Today you can only import solids or surfaces.

andrew_troup

I think it is also crucially important to have control of tangency at all boundaries, namely the ability to separately assign tangency or normalcy to adjacent faces, planes or surfaces along each boundary, along with the nature and extent of the influence across the loft surface. This control should optionally extend to continuity of curvature.
A further desirable enhancement would be some control of the relative weighting of the end profiles vs the side profiles, so that a single feature, with a more straightforward and consistent user interface, could replace both lofts and boundary surfaces from Solidworks.

raino_paananen

Also It would be nice to be able to manipulate the automatically generated "guides" (see the straight line in the pic). This might be the same thing Christian mentioned already. So basically move the "guide" to a desired point on the profile

Raino

andrew_troup

raino_paananen said:

Also It would be nice to be able to manipulate the automatically generated "guides" (see the straight line in the pic). This might be the same thing Christian mentioned already. So basically move the "guide" to a desired point on the profile

Raino

Actually, it is (at least in theory) currently possible to manipulate the "guides" which the software infers, using "Match Vertices"

I assumed the reason for the straight line in that loft was that the number of sectors (and hence endpoints) was different in the starting profile from the finishing profile, and this made it impossible for the software to infer meaningful guide curves.

A guide curve (whether manual or automatic) needs to run between corresponding vertices on all the loft profiles, and this is also a necessary condition for "Match Vertices" to work as it should.

ON EDIT: I have checked back to the original thread relating to the pictured loft and it seems I may have been wrong to  assume it would be solved by providing the same number of sectors for both profiles. I will check the model when I get a moment and see if there's some other issue with it.

raino_paananen

Thanks Andrew,

Yep, making the number of sectors equal didn't solve that issue. To be honest, I think it shouldn't matter as in some cases it would be rather tricky to fine tune the sketches like that. For example when one was to loft something that is a bit more complex. Just for an example an aircraft fuselage that evolves from a circle section to a narrow oval section via triangular section. In that triangular section there would be six different curves in one sketch. I know that doesn't sound like too complicated but it's just an example to show that things might get complicated. Now matching the circle to the complex section by slicing it up. Could it be simpler? Christians pointers should really fix what i'm rambling about...

Raino

andrew_troup

@raino_paananen ;

I've tried making the same number of sectors on the start and finish profiles of the copy I took of your model, and it has actually "fixed" the problem, in the sense that the loft is now symmetrical, AND it conforms to all the information you have supplied it with.

The problem for you is that the inferred guide curve is now present on both sides, and it happens to be straight.

This is because the software cannot know what shape you want this guide curve to follow unless you tell it, by creating it explicitly. If you remove from the loft definition the guide curves you have provided (you can do this temporarily by deselecting "add guides"), you will see that the entire loft becomes straight, so this is the default condition.

Onshape is more restrictive of the ways you can specify your intentions than most other packages for this situation because, in its present beta phase, there is no way to tell it what the global direction of the tangency is at each profile. The guide curves evidently provide only a local indication of tangency.

Nor, as I first mentioned in your other thread, is there a way yet of specifying a "path" or "centreline" for the loft - this would have given the software a better chance of positioning the intermediate profiles, which would probably prevent the undesired inference you see here. 

I have done the exercise of constructing the missing pair of guide curves with Raino's loft just to satisfy myself that it's possible, but I can't pretend it's straightforward.
Someone else can probably come up with a simpler workflow. My model is at
https://cad.onshape.com/documents/da23d67a50174f50a1786062/w/492e406ffc7c4562a84f35e9/e/0245eb45dcaf4a7f97c16684

The lack of 3D sketching makes it a bit laborious to provide guide curves, because the two loft profiles are different widths, so that a pair of angled 2D sketch planes has to be constructed, based on construction lines in one of the profile sketches, and a pair of "3 point " planes. Furthermore, to project one curve across to the other side is not straighforward: I used a surface extrude across to the midplane (so the projection would be normal to the source sketch) then "Use/Convert" to bring the curve across to the opposite 2D plane (normal to the latter)

andrew_troup

One simplification to my workflow would have been to model just one-half of the loft. As well as simplifying providing the same number of endpoints in the loft profiles, it would have avoided the laborious process of transferring the guide curve across to the other side. 
Having modelled the 'left' side, it would be a simple matter of mirroring and using a boolean "Union" to combine the two halves into a single part

raino_paananen

Thanks Andrew, 

Christian, sorry for the thread hijack In the end I didn't have anything to add to your pointers. Your suggestions are what Im looking for too so thanks for posting in the first place.

Raino

onshaper

Definitely need to be able to set normal to profiles!

mikael_jaakkola

The possibility to add normal to profile would be appreciated because if you  model in half and mirror you most likely end up having discontinuity when you mirror see picture below. With the new loft tool I can now do some surface modeling with restrictions. At the moment there are now way to trim split and knit surfaces together which are useful when doing product design. Why don´t extend split part to also be able to split surfaces.

 

andrew_troup

You are correct, and I had overlooked this lack when I made my recommendation to model only one side, but this is not going to be solved by the simple addition of "normal to profile" tangency:

It needs either something like "boundary" in Solidworks, which (when used to create a "surface") is like a loft sideways as well as longways, with control of tangency on all boundaries, or at the very least the ability in loft to add tangency conditions along the edge boundaries (outermost guide curves, in the case of a "surface" loft).