Video Tip: How to model a 3D chain drive in Creo (Pro/E)?

[sm]

We were looking into a metor question about creating a true 3D representation of a chain drive this week, and I wanted to share the outcome of that investigation. Modeling a chain drive is a frequent FIRST question, but is often not addressed properly. The following YouTube video will show you how to sketch the centerline of the chain drive around the sprockets, create a datum point pattern along the curve and then assemble the chain links including a "flexible" master link to accomodate for the different in the sum of the links vs the total length of the chain.

Chain model with Pro/ENGINEER

[JoshH]

That is a great video, nice find Scott!

I do want to share my concerns in regards to chains in Pro/e (Creo), however.

I've been testing Pro/E's ability to create a chain since about release 2001 using a methodology similar to that in the YouTube video.

1. I would NEVER adjust links to a non-standard size to make it fit.

a. Adjust your sprocket locations, this will tell you the ideal value for an ideal chain

b. Chains stretch

2. What is the design intent of the chain? Usually a simple protrusion will suffice for fit.

3. Don't forget proper chain tensioning

4. It is possible to drive a chain in Pro/E (mechanism)...but the computing power required to do this is HUGE!

5. Relations can be used to adjust your models and automate your calculations.

So folks, I would advise you to watch the video, because there really are some great techniques in it.

I would also advise you to think about your models and decide for yourself if you're truly getting what you need out of them.

Again, nice find Scott!

I hope I was able to add to it and not detract from it.

Josh

[osbexg]

Wow! What a cool video highlighting some useful techniques. I really liked the ability to pattern/repeat the single chain links at the click of a button, and the use of datum points was masterfully incorporated. Nice find...I hope to see more videos like this again soon to help out our FIRST robotics team!

Evan G.

[sm]

A similar question came up on Robotalk last week and thought I would promote this old discussion and update it with a link to a detailed example from Tim McLellan on this discussion: http://communities.ptc.com/message/167554#167554

There's a lot of good references for chains out there. Search for "chain" and "udf" which stand for User Defined Feature.

[rpackham]

Scott,

I have a few members from another team that were asking about using a chain mechanism in Creo. I don't see the actual parts in the "kit of parts". Are those pieces floating around out there, or do we need to design them?

Thanks,

Ryan

[sm]

The chain segments do not come in the KOP. You can go to Tim's website to pick up the files, the video and a PDF explanation of how to create the chain. http://www.mobiusid.com/free-downloads/

[rallen-2]

Firstly, this model looks terrific. Unfortunately, patterning along a curve is not accurate to how a real chain works. In a real chain, the distance between links is measured in a straight line between centers. When you pattern points along a curve in Creo, by contrast, the distance is measured along the curve. The point-to-point distance will thus be slightly less than what you specify. If your sprocket is very large, it will be hard to notice, but with a small sprocket, it adds up quickly and produces incorrect results. I am still trying to figure out a general solution to patterning points along a curve such that the point-to-point distance is specified, and not the distance along the curve. Any ideas welcomed. I'll post back if I figure it out.

[rallen-2]

Here is what I'm talking about. Again, for most applications, you won't notice the difference, but I'd like to get 100%.