I am trying to create a sheetmetal tapered hopper. i have attached part file. Part is not showing bendlines.
i have tried to create from solids, surface but nothing working.
Please see attached file.
Manindra,,, You are not going to get bend lines with freeform bends like this. The surfaces would have to be planar and if you want the opening on top and the bottom per you sketches you are going to end up with a twist. Imagine slicing a pyramid at an angle and you will notice that in order to keep your surfaces on the sides planar your sliced section would have to taper (unlike your sketches). Difficult to explain but if you use the "Bent" option in the sheet metal loft you can get planar surfaces and have the bend lines show. This does add a couple of bends which are necessary to make planar surfaces. The problem with that is SW will relieve the end of the bends where they meet at a single point resulting in a goofy looking model. Therefore, what I did is make two configurations. One using the formed option as you have done, and another using the bent option. The formed option is for a better looking formed model and the bent option is to get the flat pattern with bend lines. You will note that on the bent option I offset my lines so I could place the material to the outside. From experience I know that SW handles that better. Also note that I added material to the flat pattern in order to fill in the reliefs. Offsetting the sketches like I have done does alter the geometry slightly since I did not do the math to get that exact. You can put two part files (one of each config) in an assembly on top of each other and notice the slight difference.
Bent option flat pattern.
Sorry your planes are not parallel.
I know they are not parallel. Is there any other way to create this part or to show bend line?
If possible, you can created the initial shape using lofted bends with parallel planes and then cut-extruding to shape. You'll just have to be careful that this doesn't affect the geometry.
Otherwise, draw the bends onto the flat pattern with a sketch on the face. 4 bends shouldn't be too time consuming!
I have tried this method but the shape and dimensions i want, are giving error while processing cut. Do you know how can i calculate bend line accurately and how can i create bend drawings while there is no bend line? Thank you.
Very interesting method. It worked fine, but its not a right way. Now i can assume solidworks has its limit. Thank you.
Retrieving data ...