I'm trying to roll this into a cone. (there are 2 more parts to complete the cone) I had to cut it up to fit on 6X12 metal sheets for cutting. Not sure if i'm on the right track here or not.
Levi.. maybe Dennis Bacon or someone else can help... bcuz.. I'm not quite sure what you want to do.. or reengineer?...
I'll attach what I guess you're trying to do.. creating 3 panels and taking first set of cord lengths from your sketch and placing them on the two circles??
Levi,, Apparently you want the top of the cone offset from the center of the bottom 36.625 (or the rear surfaces on the same plane). An oblique cone.. Is that correct? If so your sheet metal part in the flat is way off. I divided my sheet metal oblique cone into three sections similar to what Paul Salvador is showing.
I simply split up the top circle and bottom circle then did a Sheet Metal Lofted-Bend on each pair of corresponding arcs. Then flattened the rear (yellow color) and made measurements until I got it under 144". To do this I simply kept making adjustments on the angle of the split top and bottom circles. Note the different shape from your flat.. All pieces now fit on a 6' x 12' sheet. How would you like to lug that thing around out of .134? Hmmm,,, you may have to make this out of four pieces. Just noticed that.
You can select one body at a time and flatten it.
Edit:.. I've gone screenshot mad. Another edit:.. I noticed that I have a k-factor of .33 in my file. You may want to change that more relevant to the material you are using.
Last edit,,, I promise. To answer part of your question. No you cannot roll an existing flat piece of sheet metal into a conical shape (in SolidWorks). I suppose you could do a series of radial sketch bends but that would be a lot of effort, trial and error, and not get you the results you want. In my last screenshot (I promise), I wrapped a sketch made from the periphery of your part onto a surface loft I made from your sketch circles in order to show you how your flat part would look when formed. Probably (long shot) could have used the deform tool to accomplish this also if I made a solid boss extrude from the outline of your part. I did extend the top hole of the loft in order to give the top points of your part profile something to wrap onto.
With the file I attached you can adjust the angles of the arcs (sketches 12 & 13) and alter the lofted sections to see if you can get each of the three parts onto a 6' x 12' sheet but I don't think you will be able to. I made the angles equal on both sketches but they do not have to be.
Why not use the lofted bend feature and do a reverse engineering - create your offset sketch diameters, space apart and height? Then use the Loft Bend feature, flatten and measure the bounding box and adjust your initial sketches to get the overall size down to what you need.
Circled in red is the bounding box dimensions, change the Top plane, Floor Plan and the sketch diameters to get the bounding box dimension what you need..
Hi guys thanks alot for the help and sorry for not replying sooner. I should've been clearer. This is 1 of 3 parts that form into a cone. I flattened the original cone and divided it into three parts that i could get into 6X12 sheets but now I want to reassemble them in solidworks. I'll attach all 3 to this post.
What I usually do in a case like this, create an Assy from your Part.
Create configs for ea. Part (Sheet ) needed in your Part file and place a cut, now insert the Part file in to the Assembly to the Origin 3x in your case,may take some adjustment to get the Sheet size, but it is all within one Part and robust.
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