Creating a loft feature

kartik_1

How do I create loft feature in Onshape?

I have attached a picture showing a loft feature in conventional CAD, how do I replicate it in Onshape?

andrew_troup

The reason the loft looks the way it does is that (unlike the "conventional" CAD loft) it is modelled to look that way.

There is a single guide curve on the outside of the loft to which it is accurately conforming.
If you want to control the inside of the loft, simply add a second guide curve.

Are you trying to emulate the shape at the left in your original post, and if not, please indicate what shape you do want?  
Be as specific as you can, otherwise it's a bit like going onto an auto website and asking "how do I drive a sports car?"

andrew_troup

If you want control over the result of a loft between non-parallel profiles, regardless of the CAD package, you need to use guide curves

You also need to  prevent the loft from twisting, which may be a factor in the horrible result you somehow managed to get from Onshape.

There are video and text descriptions in the "Help" documentation section which will give you a starting understanding of how to address these issues.

I would encourage you to come back to this forum to clarify anything which remains unclear or problematic once you're had a look at those basic guidelines.

bill_23

The trick to getting good lofts is to have an equal number of segments in each profile.  The segments can be mixed.  For example you can have a square. (4 segments)  The next can be round, but you need 4 arcs to make up the circle.  Each profile needs it's own plane. The way I found out how it works was to start drawing lofts until I could predict the out come before I did the drawing.  Start by making a series of planes a few inches apart and start drawing different shapes in each one alway having the same number of segments in each one.

andrew_troup

@kartik_1 : please share your Onshape model as "public", so we can see what the specific problem is.
I cannot manage to duplicate your result.

kartik_1

Our engineer just made the model public (file name "assem"), there should be a link in my account. Please check if you can access it. 

andrew_troup

The reason the loft looks the way it does is that (unlike the "conventional" CAD loft) it is modelled to look that way.

There is a single guide curve on the outside of the loft to which it is accurately conforming.
If you want to control the inside of the loft, simply add a second guide curve.

Are you trying to emulate the shape at the left in your original post, and if not, please indicate what shape you do want?  
Be as specific as you can, otherwise it's a bit like going onto an auto website and asking "how do I drive a sports car?"

kartik_1

Hello All,

I have attached a picture showing sections of a loft where 4 points are located on the circumference of the loft section. Is it possible to make 4 guide curves through the points so that we can control the loft profile better.

andrew_troup

At present, it is a little laborious, because there is no 3D sketch capability. However the individual steps are simple, and it's a more robust workflow than most 3D spline creation in other packages, so it's worth mastering.

What you need to do is to create two splines, one on the "Front" construction plane, and one on a "Side" plane, with the spline points "coincident" with the points, on one side of each profile in sequence. (Each spline is effectively an orthogonal projection, onto a construction plane, of the desired 3D guide curve)

Now extrude one of these splines as a surface to span the whole zone, and extrude the other spline "Up to" the first surface. You should now be able to pick the intersection edge to use as a guide curve.

andrew_troup

If all the sections are ellipses, you will probably get a better result by defining two guide curves, one through - say - the innermost points of the profiles, and the other through the points on one side - ie adjacent points, one-quarter of the way around the profile )

And then by creating a third curve on the midplane (construction plane) through the centres of all the ellipses,

and then using this third curve as the path for a "sweep with guide curves".

This will require just a single elliptical profile, at one end of the path.

christopher_owens

Hello! I am trying on of these, recreating the lower rear frame member of my bicycle, for fun. It sweeps from a ellipse to a circle and is a bit of an elongated S. Creating "Point-Curve" planes along the spline and then drawing ellipses on the planes. Of course I have to draw a line in the ellipse from the center to a Quadrant vertex and then add the constraint to that line of 'Vertical' (hoping that vertical is what I think it is!). A "Nice to Have" would be the major and minor axis lines show up while sketching the ellipse.

christopher_owens

I am trying to figure out the Guide Curves. In this image you can see the "Tools" (A part transformed-copied-scaled) and a sketched path (whose points I used as locations to copy the first part to.) And a Curve Point Plane to figure out the angle to rotate the last tool.
Now I create the Loft using the surfaces of the "Tools". (This way I don't have to redraw the sketch of the shape) 
But when I try to use the sketched path as Guide Curves, the Loft fails.

Obviously I have never used a 'Loft' for anything production and am trying to figure it out!! Basically I am looking at hoods and fenders of cars for inspiration! Do I need to sketch the guide curve last? Could I "Use Edge" to recreate the sketched path so the new sketch pierces the profiles? 

_Ðave_

@christopher_owens I was experimenting with lofts also with issues getting a good guide curve. when all else failed I recreated the guide curve as a single spline and all worked fine. I'm not sure if a single spline is required (need more experimenting) but it appears to be a fail safe procedure. hth

christopher_owens

@dave_petit Well, I am getting closer! I sketched two guide splines on planes created at the vertices of the two 'tools'. Of course now both 'tools' are the same size, no scaling. I see the guide curves guide the vertices along it's path. I created one guide path as a 'Use' of the other. I was wanting to guide the whole profile (like a sweep), but yet have it get smaller along the curved path. Hmmm...seems like more construction entities are needed to do what I am thinking...

I was able to create this using a loft passing through sketches and matching vertices... so I'll keep trying!

christopher_owens

Of course that first image is kinda a "Sweep"...but not exactly! The 'other-side' surface has some variations from a "Sweep" I did to check!

andrew_troup

christopher_owens said:

I am trying to figure out the Guide Curves. In this image you can see the "Tools" (A part transformed-copied-scaled) and a sketched path (whose points I used as locations to copy the first part to.) And a Curve Point Plane to figure out the angle to rotate the last tool.
Now I create the Loft using the surfaces of the "Tools". (This way I don't have to redraw the sketch of the shape) 
But when I try to use the sketched path as Guide Curves, the Loft fails.

Obviously I have never used a 'Loft' for anything production and am trying to figure it out!! Basically I am looking at hoods and fenders of cars for inspiration! Do I need to sketch the guide curve last? Could I "Use Edge" to recreate the sketched path so the new sketch pierces the profiles? 

This is not strictly a "guide curve", it's more of a "Path", but (at least, in Solidworks) it tends to be called a "Center Line".
Onshape uses the terminology "guide line" rather than guide curve, and stipulates (among other things, listed in Help, which anyone proposing to master lofting needs to read carefully)

• "they must touch the profile (use Coincident or Pierce constraints)."

A "center line loft" is a different beast from a conventional loft with guide curves, and a beast which Onshape does not currently offer.

kartik_1

Here are two of our attempts at creating lofts 1) using circles and 2) using circles and ellipses. Please let us know any feedbacks. 

imagineered

andrew_troup, per your comment "If you want control over the result of a loft between non-parallel profiles, regardless of the CAD package, you need to use guide curves" sorry I disagree.
Trying to create a loft from 2 x 8 sided polygons to 3 circles failed miserably on Onshape, (had to create the circles from 8 radii), however tried the same in Solid Edge with no guide curve (or sectioning the circles)- No Problem

imagineered

andrew_troup; still not fail-safe in SE but   

andrew_troup

@imagineered: I wasn't pretending it couldn't work, I just said you would not have control over it.
The software will make up its own mind what "path" to use for the loft between sections: if you happen to like that path, no problemo; if no like, that's just too bad..