Trouble creating a simple loft with guides
Hi, I am trying to create a simple loft between two opposite side faces of a block. The profiles are rectangles with different depths from the top surface. On the top surface I sketched a couple of guide arcs for the loft to follow. No matter what I try I can only get the top surface of the loft to follow the guides. The bottom surface always follows a straight line between the connection points of the profiles. I must be missing something simple. Any ideas? Thanks.
https://cad.onshape.com/documents/163af253ef97ba2ee4497c9e/w/3ded52a9af1074e98be1bcf4/e/b9bff13f557f2487306723f5?renderMode=0&uiState=698481993dc5a2e4a0e88d96
Answers
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That is because the guides are only at the top. How should the program guess you want it also at the bottom, but not at the outside edges? Make guides for the bottom, too. You could just copy them. Or build the whole thing out ot two extrusions. Much easier in this case.
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Set up a three point plane - start a sketch - add the two 3-point arcs and copy the radii from those above to the new ones below - and there's your four functional guides.
Unemployed Onshaper- Operating on European time - More of me here ➤➤ https://linktr.ee/Liam.G0 -
Ahh, thats what I was missing. I tried other sketches for the bottom points but I failed to make them on a plane that intersected all the bottom connection points. I had tried to make a sketch on the bottom surface of the original loft (same plane you guys created) but the loft couldnt see the sketch b/c it was after the loft.
Makes perfect sense now.
Matt, not sure I understand what you suggested. It almost seems like what I tried but couldnt get it to work. Are you projecting the original guides onto the surface created by the first loft?
Thanks
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Following up…Matt, when I try to project the curves onto Plane 1 the endpoints dont line up with the profiles. How did you do that?
I see CADnerd just reproduced the radius manually between the connection points on the new sketch.
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Use the "Use" tool to create the second set of guides.
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@martin_kopplow - tried that first and it didn't work due to the angle. Trickier than it looks - a useful little challenge.
Unemployed Onshaper- Operating on European time - More of me here ➤➤ https://linktr.ee/Liam.G0 -
The Use tool didn't quite cut it. I used Projected curves (which allows you to control the projection direction, rather than being simply normal to the sketch plane).
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Oh I see now. It looked like "Direction" only had one option…Normal to Target. You have to hilite Direction then click on the part somewhere.
Good method.
Thanks all…very useful info. Learned multiple techniques.
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There is more than one way to skin a cat. You could also just remove-extrude the face between the curves for cutout, then replace-face the bottom with an angled (3-pt.) plane. You could also face-extrude the upper curves, then split the two faces with said plane and loft between them. Always depends on what you're trying to achieve regarding design intent.
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