Hello, I am using ST6 and I am trying to make a cone that overlaps itself (pictures will explain better). I used the Loft command because I couldn't find any other easy way. The loft command works if I want to make one edge overlap, as shown in the first picture (3D). At this point, the sketches are as shown in the second picture (2D sketch). But as soon as BOTH edges are overlapping, the loft command doesn't work (as shown in the 3rd picture).
I've tried to make two lofts, one for the left side (large radius), another for the right side (small radius) but I can only make one loft work, not both together. Any ideas ?
Solved! Go to Solution.
My first thought would be to create using the surfacing environment, using bluesurf to make it, then after it's made switch to the part environment and thicken to whatever thickness you need, switch back to sheetmetal and use thin part to sheet metal to convert it to a sheet metal part.
I just saw that you're on ST6 so won't be able to open the file I sent. Here's a video showing how i made it.
I believe I used the outside face, and then I usually pick the bottom round edge and the bottom of the cone on stuff like this.
Although I have the part in the sheet metal environment, I can't flatten it correctly like you did. See pictures attached. I also attached the part (ST6). I can only choose this face or the one on the other side.
Then I have to choose the orientation. I have the choice between the selected edge on the picture or the circumference edges.
Whatever point, edge of face I choose, I always end up with this :
It seems like my part would need a planar face other than the thickness to be flatten so I tried to add a flat part (on the overlap) but it won't recognise this as a flat.
I think it's because it recognises the flat as a spline instead of a flat, planar, unbent, sheet metal face.
Go into your material table. Take a look at what your material thickness is actually set to as opposed to what it is set at. You have the sheet metal gage as 0.051, but the material thickness is showing to be 15.27304inches. Something is weird here, as I can't think of any material gages which are that thick.
I think what you did was pick the wrong face when you transformed. Delete your transform feature, then do another transform, this time don't pick that bottom edge, pick the large inside face of the the part. After that, then flatten as we talked about.
I tried making that sketch, im not sure how you made the sketch with only one diameter dimension?
I'm not sure if you were talking to me. But if you were and were referring to what you saw in the video, I will now assist. In the video I only went inside of the second sketch. If I had gone into the first sketch, you would have seen what I'll put below. There are two arcs in the first sketch. The large one is the one mostly driving this. It's diameter is 12". At the bottom is where that arc ends. Then another arc begins, which is tangent to the Ø12" at the bottom. Other than that tangency, what is driving the diameter of that second arc is the 10ga thickness which i added between the quadrants of both arcs at the top. That, accompanied with the horizontal relationships between the end points of the construction V at top, and with the 5° angular dimension between those lines, fully defines that first sketch. Then in the second sketch i simply made two more arcs both concentric with the two in my first sketch, and then had the Ø10" dimension on the large arc, and used include of the construction V from the first sketch and trimmed the remainder, and viola. Done.