I need to model an elastic (rubber) band and don't know where to begin. Can anyone offer suggestions to get me started?
If you have SW2014 check out my example assembly and see if it is sort of what you want. I ended up making the rubber band with extrudes and a loft for the twisted part. If you have any questions about it I can explain my method in more detail.
Do you need it for an assembly where it will be stretching? I'd suggest modeling it in context of the assembly using the geometry that it will be binding. That way if things move the band geometry will update accordingly.
Yes it will be used in an assembly where it will be stretching. I would love to model it in the context of the assembly, but I don't know how to begin.
The most basic method is when you are in the assembly, go to Insert > Component > New Part. Then you need to pick a surface in the assembly that you want to start sketching your part onto. If the whole band will lie on a single plane then you'd want to pick a plane that is parallel to that, so you can sketch the path of the band. Once you select a face it will automatically go into part edit mode, and you will be in a sketch on the Front Plane of the new part. So now just sketch the path of the rubber band, creating relations to the assembly parts as needed. You can even convert entities from assembly parts to pull those edges into your rubber band sketch.
As a very basic example lets say you have the band wrapping around two dowel pins that will spread apart. You could sketch the rubber band patch by drawing a slot shape and making the ends of the slot coradial to the dowel pin diameters. Once you have the patch sketched it will probably be easiest to do the rest by editing the part by itself, so you can exit the sketch and leave part editing mode (by clicking the icon in the top right). Then find the new part in the tree (it will probably be named something like [Part1^AssemblyName]) and open it up. With the part open by itself you can do a Save As to give it a name and make it's own file. Now in the part draw the cross-section of your rubber band and do a sweep to pull it around the path.
Back in the assembly the part you drew will be fixed, kind of. If you look at it's mates it will have a InPlace mate, which fixes it to the part that you started the sketch on. If the band is positioned properly you can just leave the InPlace mate, but if you need to move it then delete the mate and add new mates to position it properly. Now if the dowel pins move in the assembly the size of the rubber band will update automatically.
Excellent! This gets me started. To further complicate the matter, however, I now need to twist the rubber band.
Imagine those two dowel posts protruding from a board at 90 degree angles, one at each end of the board. The rubber band needs to wrap around the first dowel, travel under the board with the same face that mates to the dowel now mating with the bottom surface of the board (thus the twist). It travels the length of the board up to the top side again, and wraps around the second dowel (another twist). Can SolidWorks handle this?
It is doable. You can add a twist in a sweep feature, but you might need to break your sweep up into multiple sections so you can control. the twist in each portion separately.
I'm just now getting back to this. Sorry for the delay. When I open your example I think I understand what you are doing to create the rubber band, however I am curious as to why you chose 6061 aluminum alloy as the material instead of something like natural rubber. Was this merely convenience, or is there more to it than that?
My part template is set to 6061 by default and I just didn't change it. You could make the material whatever you want.
I modeled the rubber band using a slot sketch with no dimensions. extruded it thin, the width of the rubber band. in the assembly I clicked show sketch and I mated the radii on the sketch to round bars they went around using cordial mate. with the sketch not being constrained with dimensions it was allow it to stretch.
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