Need Help with Assembly Joints

[iESCadCam]

I am trying to automate a process for I/O expansion reduction tooling. I want to somehow constrain these fingers so that they will expand out to so far (when the diameters are concentric) and collapse down to their minimum state when the fingers mate with each other. Is there a joint command that will work for this?

[JDMather]

A Mate constraint with Limits should to it.

I'll be back in a while with example.

Sketch4 is not constrained in your part file?

[iESCadCam]

I updated and attached the part file. Sketch 4 is now constrained.

[iESCadCam]

I looked at your assembly. How do you collapse the fingers so there is no gap between them?

[JDMather]

Drag the Green part in the attached assembly.

I entered a Min/Max distance as well as a default position.

[JDMather]

Depending on your Design Intent, this could also be set up to Drive Constraint rather than mouse dragging.

[JDMather · Accepted solution]

Expand the constraint dialog box to see how I set the limits.

[salariua]

I would tend to do drive constrain or drive them all with ilogic. Don't know about current status but while back the limits on constrains were only recommended for small visual simulations not for medium-large assemblyes.

Here's the knowledge center:

Tip: As with contact sets, consider assembly performance when you use limits. For best performance, use limits to evaluate your design and then edit to clear the check boxes. The limit values are stored with the relationship and remain available when you reactivate the limits.

http://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2014/...

[iESCadCam]

Thanks JD that's awesome! That's exactly what I was looking for. Now is there a way to place multiple views of this assembly in a drawing? For example I want to show a view on the drawing with collapsed dimensions and expanded dimensions.

[salariua]

You need to create positional representations of each position (collapsed, expanded). Then when you go to drawing and place the view, you can choose the positional representation for that view. Or you can do overlay to show them both on same view.

[JDMather]

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@iESCadCam wrote:

... show a view on the drawing with collapsed dimensions and expanded dimensions.

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I will post example with Position Representations later today.

You might also be interested in Overlay views.

[iESCadCam]

I'm starting to see the capability of Inventor assemblies. This is neat. I am attaching a complete assembly. Here's what I would like to do and you tell me whats the best way to go about doing it. I would like to be able to stroke the mandrel in and out until the fingers reach their limits. One limit is at collapsed state and the other is when the dowel pin on the fingers max out the slot on the middle plate in the assembly. The jaws should always maintain the tubes wall thickness from the fingers. In this case 1.3mm or until the jaws dowel pin maxes out its corresponding slot on the middle plate. Then I would like to be able to create two drawing's. One for the fingers and one for the jaws. In each of the drawings I want to show the tools in their at size (round state for manufacturing), one view in the collapsed state, and one in the fully open state. Is it possible to do all this?

[t_stramr]

I just want to point out that Assembly Joints provide limits as well. So the same result you can achieve also using joints with limits. You can find them on the second tab of joint dialog box(limits are not available in joint mini toolbar).

Thanks,

Robert