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What is the best way to create a flexible component?

jla9A94K
Enthusiast

What is the best way to create a flexible component?

jla9A94K
Enthusiast
Enthusiast

I very commonly have a lift or some rotational motion as part of a loading or unloading feature for the machinery that I design.

 

In most applications there is a flexible component such as a cable carrier or duct that is externally visible and moves in such a way that its shape changes as a function of the motion.

 

Recently we have started using the rendering from Inventor studio in the HMI controls of our machinery... so I am in the midst of a very painful workflow and I think that there has to be a way to create a part that is flexible so that I can render an animation instead of rendering a series of images.

 

Attached is a model which highlights the issue that I am having. You will see that with the applied constraints PLATFORM-AQ.ipt moves up and down, but DUCT-ZD.ipt only looks correct when the platform is all the way up.

 

Thanks,

 

Jesse

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Accepted solutions (3)
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Replies (8)

Anonymous
Not applicable
Accepted solution

There are a few ways to achieve the goal as you've described it.

 

One is to make the part adaptive and to project in a plane off of the upper bracket and use that to drive the resulting shape of the duct. Then when that driven constraint is manipulated in Inv Studio, the adaptive duct should change as the bracket moves with each frame.

 

The second, and my preferred method, is to have a sketch within the duct that serves to animate the model. I personally find more stability and reliability in using sketches within part files to drive all of my animations rather than constraints or adaptivity or flexibility or so on. To do this, you'd have a sketch in the duct in which you have a construction line representing the top bracket and another representing the bottom bracket and a dimension (let's call it "HEIGHT" for reference) between the two (mimicking the constraint you have in your assembly). Then, change the duct part such that this sketch is what drives the shape of the sweep. In your assembly, you'd constrain your components to the duct itself and in studio, you'd set that HEIGHT dimension as a favorite and drive it between your extents.

 

Both of these methods should work. I just personally prefer the latter after having animated a few dozen models over the years. And honestly, the sketch method can be extremely useful when you start animating several things at once. Part sketches seem to have a much easier time retaining their constraints when there are several things changing.

 

Let me know if this needs any clarification or if you'd like an example.

 

Thank you,

jla9A94K
Enthusiast
Enthusiast

I'll try to lay out both solutions. I'm not sure if I will be able to get to it today, but I'll post here when I do, or if I have questions... though the explanation seems pretty clear. 

 

Thanks for the reply.

 

 

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Anonymous
Not applicable

Sure thing!

 

I'll keep an eye out for your reply. Good luck!

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JDMather
Consultant
Consultant
Accepted solution

@jla9A94K 

Unzip and open the Attached assembly.

Go to Environments>Inventor Studio.

Open the Animation Timeline.

Click Play...

Animation Timeline.PNG


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Autodesk Inventor 2019 Certified Professional
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Certified SolidWorks Professional


jla9A94K
Enthusiast
Enthusiast

Perfect, thank you both!

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jordan.aerts
Explorer
Explorer

How do you get the duct to simultaneously shrink from one end and grow from the other end?  It is a single body with only one mating and I am perplexed.

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johnsonshiue
Community Manager
Community Manager

Hi Jordan,

 

It was a very clever technique leveraged by @JDMather. The deforming part, DUCT-ZD.ipt has a sweep feature from a circular profile and an U-shape path. The path is dimensioned in a way that when one side increases the length, the other side decreases the length.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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JDMather
Consultant
Consultant
Accepted solution

JDMather_0-1701352144949.png

JDMather_1-1701352372853.png

 

Set dimensions as a function of a User Parameter and then Animate Parameter in Studio.

Attach your assembly here if you can't figure it out.

 

JDMather_0-1701352308768.png

 


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Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional