Any way to create a "driven constraint" that behaves like a driven dimension?

[LSKELLY]

Please don't confuse my question with the "drive constraint" function.

I wonder if anybody knows how (or knows a workaround) to create a "driven constraint". In part sketches, you can set dimensions as driven, after which they behave more like a measuring tape than a constraining device. I think it would be very useful if assembly constraints could be set in the same way that they do not fix objects in place but rather provide a "readout" in a parameter.

I have looked around the internet/forums and found nothing. However, it makes no sense to me that such a feature does not exist as I think it would be very useful for a number of applications and I can't imagine that programming this functionality would be too much more complicated than including regular constraints in the software.

[BDCollett]

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@LSKELLY wrote:

Sorry @JDMather.

The cylinder-and-linkage mechanism I mentioned was just an example. I was saying I would like to drag the rolling skip freely in a normal assembly, in the same way that one might drag a cylinder and linkage assembly. An unintentional red-herring.

To further illustrate my goal, it seems it is possible to achieve exactly the desired result in a sketch, but not in an assembly. I have attached a part containing a sketch. the sketch is missing one constraint which is left free to be able to drag it (best results by dragging the point at the center of the arc, I found). Give it a whirl.

Why is it possible to mathematically create rolling motion in a sketch? Because sketches allow you to create driven dimensions. What I am looking for is an assembly constraint equivalent to a driven dimension. To the best of my knowledge, no such entity exists for assembly constraints.

Also, I am asking not only for the application of the tipper skip example. The tipper skip example is only one place where this type of "driven constraint" might be useful. Theoretically, one could use such a type of constraint to make all kinds of mathematically complex motions.

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You can add limits to your constraints so they move a specific amount when dragged.

Or you can still drive a constraint dimension in an assembly with a Form and set the range there.

There are a few methods to do the things you want but I think you might be missing the complexity of the other solution you expect in an assembly.

[LSKELLY]

@BDCollett 

Yes. I guess not being a software developer I must be missing something regarding the difficulty (or perhaps instabilty) of a measuring entity that updates a parameter.

I live in hope, however, that someday such a useful feature may be added to the software.

Thanks to all that contributed here for your time.

[JDMather]

I am pretty sure that what you want to do can be done today - but until your last file - you never  indicated which two points you wanted to measure.

[LSKELLY]

@JDMather 

I will attempt another way to illustrate what I am looking for.

Take a look at the attached model sketch. Drag it about by gripping the center of the circle.

d0 is a dimension that exists not to constrain the sketch, but to provide a measurement based on the users free-dragging input. This measurement in turn drives an angle in the "eater's" jaws.

This seems easy to achieve in sketch mode, but not so easy to achieve in a free user-draggable assembly. If Inventor had a way of dynamically updating a parameter in an assembly based on the user's dragging motions (the way that d0 does in this part), making an assembly that behaves the same way as this sketch would be easy.

You could also apply such functionality to countless other applications.

[gerrardhickson]

Hi All, I haven't read through this thoroughly, but it seems related to my post in the ideas forum. In my case, I wanted to be able to "derive" a parameter based on some measurement taken from the model - this could be the distance between two planes or points or an angle - and make that measurement accessible as a parameter. That would allow it to be shown in a drawing text box or used in an equation for a derived part - the list goes on.

If it sounds relevant, check out the link below - otherwise, please disregard.

https://forums.autodesk.com/t5/inventor-ideas/annotation-values-to-parameters/idi-p/10475741

[gerrardhickson]

In the post linked in my previous message, I mentioned a work around - create a sketch, project in geometry and use driven constraints.

In the image below, I took your the sketch from your example part, created an assembly then created a sketch which derives in some geometry that finally drives some dimension constraints which are also accessible in the parameters.

You can (and probably should) turn off the sketch, so what you're left with is a few parameters that are driven by the position of your assembly geometry. I think that's more or less what you're looking to achieve....?