Please see the attached SW2018 Part. I don't do this kind of thing very often, and wondered if anyone has a simpler method of accomplishing the same result (the transition between the two bodies). It needs to consist of all flat surfaces, so as far as I can figure out a Loft between the profiles won't work since that creates twisted surfaces.
There is a referenced part that is missing:
TxDOT F-Shape.SLDPRT [Not Found]
You need a "Guide Curve".
Now don't ask me how they are going to form it up.
Just loft from one face to the other. Use the connectors to straighten it out, and do it all at once. No guide curve needed. You can't make a planar face from the curved edges.
Could you make surfaces and knit them into a solid body instead of lofts? For example, I'd make two surfaces from these edges, instead of three lofts. This could likely be formed from solid features too, with slightly altered sources.
Edit: basically, I'd improve the loft by reducing the number of facets by making different selections to derive planar faces, whether as a surface or a solid. Note that I only selected two edges to define the Surface-Planes, and it filled in the hypotenuse.
Hello Glenn,.. I'd just make a sketch (remove the bottom notch) and loft it to the face (and don't merge faces?).. (image attached)
I think Glenn wants all the faces to be planar. No twisting allowed.
Jim,...well, turn off normal to constraint.. and most would be planar-ish.
I think the only way to do it is to facet it in some manner like Glenn has done. You can't make a planar loft between two edges that aren't parallel to each other when viewed along the loft direction. Any non-parallelism creates twist.
Jim,.. understand.. then, maybe the majority could be a straight Sweeps and the remaining would then need to be faceted transitions?
..btw,.. if they are 3-6mm thick plates... why not just twist the plates?
You don't 'need' guide curves and Matt's suggestion works great.
My personal preferences though is 'like number of entities to like number of entities' for loft profiles.
For example, lofting a circle to rectangle. It's better to do this with 4 coradial arcs that form a circle to match the 4 lines of a rectangle.
BUT you don't have to draw 4 co-radial arcs, that would be annoying. Just drawing the circle and use the 'Split Entity' command. (Sketch points are not good enough)
2019 SOLIDWORKS Help - Split Entities
Loft connectors will naturally fall on those points where the circle was split or the lines intersect on the rectangle.
Those points can be dimension-ed or have relationships added to them which some designs really need. Easier to do it up front as connectors cannot be defined as well.
That doesn't solve the limitation of 'no planar faces from curved edges' though. That sounds like one of the sketches would fundamentally have to be reconsidered. Perhaps add the fillet/bend after the loft.
Jim Sculley wrote:
I think Glenn wants all the faces to be planar. No twisting allowed.
C'mon wood twists a little bit...And there's nothing wrong with making the Contractor earn his money by having to make complex forms...
Glenn Schroeder wrote:
Please see the attached SW2018 Part. I don't do this kind of thing very often, and wondered if anyone has a simpler method of accomplishing the same result (the transition between the two bodies). It needs to consist of all flat surfaces, so as far as I can figure out a Loft between the profiles won't work since that creates twisted surfaces.
Hello,
What about the region?
You arrive at a radius, but you posted all planar.
Kevin
..
Kevin Chandler wrote:
What about the region?
You arrive at a radius, but you posted all planar.
Kevin
The part between the continuous profiles is what needs to be all flat planes. A small offset like my model has will be okay. My final result is what I need; I was just wondering if there's a better way to achieve it.
I appreciate all the replies. I've been putting out fires and haven't had a chance to investigate the suggestions, but I need to do two similar projects in a week or so and I'll get back to this then.
LOL!
Ha gonna sell that macro? with cheese?
Justin
How can it be find out that particular connector combination will give a flat surface?
Hi Glenn Schroeder,
It can be done with flat faces;
Create on both surfaces sketches with each 16 entities of straight lines, and use them as profiles for the Loft.
Drag one connector to an aligned position to prevent twisting. No guide curves needed.
The red arrows pointing at the straight lines are important.
To get that area at the radius "even more perfect", the number of entities can be increased
Since you'll need something for the mold.
Sheetmetal lofted bend:
btw,.. your point of how accurate at the fillet made me think.. why not simplify it more so?... (image)
Paul Salvador wrote:
btw,.. your point of how accurate at the fillet made me think.. why not simplify it more so?... (image)
Paul,
Thanks for working with it, but I'm not sure how that's simpler. It's still five faces on each side.
Thank You 
Glenn,
Can you add a Screen Shot so I have an idea of what you are tackling... Thanks.
Daen