how do you design chains on inventor?
Not sure, but in some drawings of the feild I have seen is just a pattern of the general dimentions of the chain links.
My advice on chains: Do them last. It’s not really necessary except for aesthetics and they sap up power.
Warning: The following process does take a bit of time and is a bit messy. There are most likely much better ways to do this. I was pressed for time and I did what would work for me in a hurry, but it still took a few hours. After seeing 103’s description on how to make a lead screw, I think that they’ll have a better handle on this than I do. Also, do your math beforehand so you don’t have to tension your chain, so to speak. I the fix in my description in case you don’t do it beforehand.
Here’s a method that’s much easier than below and would probably be fine. Just make the plate as I describe below and emboss a chain-like pattern on it. Decal might work for the image. I don’t know too much about this though, so I’ll leave it as an exercise for the reader to figure out 
With that said, last year I used the “ANSI chain links” on this site. The dimensions on the links didn’t quite match the iSprocket in the First CAD Library and it made a visible difference when going around a 45 tooth sprocket, so I changed the dimensions on the links very slightly (although I don’t remember exactly how). I then made a work plane that was on one face of a sprocket. Create a component on the work plane and project the geometry of the sprockets that I was connecting onto the sketch. After that, I made a circle so that it was concentric with the sprocket and the outside was coincident with the radius of the teeth of the sprocket (the points will come up if you project the geometry). After that, make lines connecting the two circles (coincident and tangent to create a solid profile). Extrude to the width of the sprockets.
Following this, place the two chain profiles that you need (I didn’t really use the master link one). Constrain them so that the axis of the chain link is centered on the piece (I used a mate with an offset). Constrain them so that their axes mate, and that they are centered correctly on the sprockets. I also lined them up so that one matched the line where the straight part starts (axis to line mate - you won’t be able to do this for all sides). I then turned the sprocket to match. After that, you can use a “pattern components” to place more links around the circle. You’ll need to know the right number of chain links to put, as well as the degrees for offset (which will involve a bit of geometry).
After doing this, place two more of the appropriate links. Constrain the axes to each other, and the appropriate axis-to-axis mate with your patterned chain. As necessary, constrain an axis to the face of the circle again (if you are already clear of it, don’t worry). Then, constrain the axis of the chain links to be mated with the straight part. After this, previous experience and patterns take over. Place more chain as necessary until two are on the straight section completely. Then pattern the components rectangularly with the correct offset so that they go until the next circle. Constrain until two links are on the circle. Then pattern around this circle as well. Repeat the same process with the straight part.
Unless you’re lucky or you do your math beforehand, the ends of the two links won’t line up. Hopefully you have your chain tensioner device built into inventor. If you need to, measure the distance between the two axes that don’t line up. Then calculate how much you need to move the tensioner with geometry, and do so. The plate you made should be adaptive by default, but you may lose some constraints when you do so. Since you’ve learned the process and know what dimensions that you need, replacing some chain shouldn’t be very difficult. After you’re all done, make your plate invisible (and assign it a weight of 0 to keep your physical properties accurate) and you’re done.
honestly, making the chains for our robot on inventor wasn’t hard. tedious, yes…but not hard.
obviously, you’ve shipped the robot, but i’ll go ahead and tell you how i did it.
first, i made the two pieces for the chain, the “outer” link and the “inner” link. the outer link has two elliptical disks with two bars between them. the inner link has two elliptical disks (closer together than the outer link of course) with two hollow cylinders between.
THIS IS THE KEY PART: The inside distance between the two disks on the Outer link, and the outside distance of the two disks on the inner link MUST BE THE SAME. ALSO: make sure the diameter of the bars of the outer link and the inside diameter of the hollow cylinders are the same.
after that, its simply a tedious job of using Insert Constraints to insert the bars of the Outer link into the hollow cylinders of the Inner link.
it wasn’t fun, what with our two chains having 56 and 96 links two-a-piece, but when i finished…i basked in the feeling of accomplishing something :]
The trick to making chain in inventor is making it go around a sprocket properly. It’s easy to make chain go in a line.
It’s easy to make chain go around a sprocket.
I don’t know how you’d make it do both.
Anybody?
If somebody is willing to look it up there is a tutorial somewhere about how to animate chain properly. Somebody might wish to look that up.
That’s exactly the one I was thinking about. That is by far the most realistic chain animation I have ever seen.
If you cant tell from the animation, all he used was halflinks and not full links. Im sure using half links would make it easier.
Also check this one for creation. Animation might be overkill by the time you back up a bit from the model.
http://www.mcadforums.com/forums/viewtopic.php?t=2196