Help with assembly constraints

[Anonymous]

Hello,

 I am trying to constrain this conical slope of roller shaft to inside edge of holder but its not going through. I tried to make the slope as tangent to inside edge of circle but it doesn't recognize it as a valid constraint. Is there any way i can constrain this such a way that, slope of roller is in contact with the inside edge of circle?

Attaching the screen shot Assembly roller and holder

Thanks

[TheCADWhisperer]

Multiple techniques to achieve this.

Contact Set would be one, but that only finds the contact and is resource intensive.

My preference would be to Split the conical face at the contact diameter and then use this with an Insert constraint (or other as appropriate).  I would probably add Constraint Limits for allowable motion in this case as well.

Attach assembly with two mating parts if you can't figure this technique out.

I probably have an existing example, but you haven't stated what version of Inventor you are using.

[Cadmanto · Accepted solution]

You could also create a plan slicing through the conical shape where you want the constraint and create a sketch there.  Then constrain that sketch point.

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[Anonymous]

Thank you for your quick response, attaching the assembly file with the pats. I tried the contact solver but its failing for some reason. I am using Inventor 2019

Appreciate the help

[TheCADWhisperer · Accepted solution]

I took a look at your files and found a number of issues.

I did not realize that you were a beginner.  I will have to make many corrections, but because of the number of errors in logic I am not sure of your true Design Intent.

[Anonymous]

That is precisely what i wanted to do, thank you so much.

[SBix26 · Accepted solution]

Another, and perhaps more realistic solution, is to give the sharp edge a slight chamfer at the same angle as the conic surface.  Then it is a simple face/face mate constraint.

Completely sharp edges are an extreme rarity in fabricated parts.  Many fabrication drawings have boilerplate text on them along the lines of "break sharp edges", which means to file them off slightly or machine a very small chamfer, depending on the tolerances and fabrication techniques involved.  We almost never model such things because it adds no value; instead it clutters up drawings.  In your particular case, though, it would make your constraint much easier.

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Sam B
Inventor Pro 2019.1.2 | Windows 7 SP1
LinkedIn

[Anonymous]

Wow that's actually way easier and you are right, we do have a standard note which says, break edges and sharp corners .005-.015. Face to face mate worked perfect and I was even able to add limits. 

Thanks a ton.