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Rotate WITH constraint in assembly?

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Message 1 of 21
apullin
9519 Views, 20 Replies

Rotate WITH constraint in assembly?

So, after some reading through the help and the forums, it seems like that the operation that I'm trying to do isn't really available in Inventor:

 

I have an assembly wherein one part is mated to another grounded part, with a face-to-face coincident mate. The click + drag type of movement appears to move the part, while continually solving this constraint.

 

However, it seems like there is no way to do a rotation in the same manner, where the constraint is continually updated. There appears to only be the "Free Rotate" command, which ignores the constraints.

 

Is there really no way to do this in Inventor?
The application is that I am laying out a mold for many, many small parts, and I am trying to move and rotate them into position to get good packing efficiency and density. Each part will be attached to a mold base with one of the afformentioned face-to-face constraints, then slid & rotated around manually.

 

This seems like a really important piece of functionality. Solidworks can certainly do this, do a part rotation in an assembly, while solving for existin constraints.

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Message 2 of 21
spackle42
in reply to: apullin

This doesn't sound too complicated.  Use the explicit reference vector option in angle constraints, this requires three references: a normal face on the grounded part, a normal face on the moving part, and an edge or axis about which the rotation occurs.  Once you have these selected, you can use maximum and minimum values to limit the range of motion. Example attached. HTH



Justin Smith

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Message 3 of 21
JDMather
in reply to: apullin


@apullin wrote:
This seems like a really important piece of functionality. Solidworks can certainly do this, do a part rotation in an assembly, while solving for existin constraints.

Attach the SolidWorks assembly here.

It sounds like maybe you are referring to Contact Sets in Inventor (Physical Dymamics - Collision Detection in SWx), but perhaps more complex Environments>Dynamic Simulation in Inventor.  More information is needed.  The SolidWorks example you reference will give me the information I need.


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Message 4 of 21
JDMather
in reply to: apullin


@apullin wrote:

 

I have an assembly wherein one part is mated to another grounded part, with a face-to-face coincident mate. The click + drag type of movement appears to move the part, while continually solving this constraint.

 

 

...


Actually maybe your problem description is trivial.  Click and drag type movement while continually solving mate constraint existed in Inventor before it existed in SolidWorks. (it used to be in SWx that you had to use a icon tool before click and drag)  Post your assembly here.


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Message 5 of 21
mrattray
in reply to: apullin

Free rotate and free move both will always ignore constraints. As Justin and JD mentioned, the only way to get the part to rotate from a drag is to constrain it so it has to rotate. Posting your assembly here will help us give you a more specific answer.
Mike (not Matt) Rattray

Message 6 of 21
coreyparks
in reply to: apullin

A work around would be to add a work point along the axis you want to pivot around and then ground it.  pivot part and delete when done.  Tedious I know.

Please mark this response "Accept as solution" if it answers your question.
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Corey Parks
Message 7 of 21
graemev
in reply to: apullin

If you place the pointer just outside of the free rotation circle, the pointer changes type and permits rotation strictly about an axis normal to the current view.  Also, when near the rotation circle axes (radiating fro mteh quadrant points) the rotation is strictly about the selected axis.  I use this quite a lot for much the same reasons you seem to desire.

Message 8 of 21
jtylerbc
in reply to: apullin


@apullin wrote:


The application is that I am laying out a mold for many, many small parts, and I am trying to move and rotate them into position to get good packing efficiency and density. Each part will be attached to a mold base with one of the afformentioned face-to-face constraints, then slid & rotated around manually.

 


 

You might consider trying out the Grip Snap tools.  This will let you move or rotate parts around relative to selected geometry, while maintaining constraints.  If you issue a Grip Snap command that violates an existing constraint, you'll have the option to suppress or delete the constraints, or to cancel the move.

Message 9 of 21
apullin
in reply to: apullin

Thanks for all the input, folks. I've attached both a Solidworks 2010 and an Inventor 2014 example of what I'm trying to do. In the SolidWorks example, the 'arrow' part can be translated by left clicking and dragging, and it can be rotated by right clicking and dragging.

 

@spackle42 : In that example, it's a mate along an edge, whereas I am doing a face-to-face mate. A better way to describe it would be that it's a part sliding on a surface, with 3 degrees of freedom (one rotation, two translation). See my attached examples.

 

@JDMather : I don't think that contact sets should be needed here, although I have used them in other Inventor assemblies with success. The attached SW assembly shows the satisfaction of the face-to-face constraint without any extra contact solution. See the attached assemblies.

@graemev : This is an excellent suggestion. I just tried it, and it does indeed work as described. Thanks for the input! The mold is all layed out and printing right now.

Still, if any Autodesk people are reading this, this should perhaps be considered a feature request.

I am, though, open to the possibility that there is some reason that a rotate-while-constrainted function doesn't make sense in the inventor workflow, but it does largely makes sense in SW.

Message 10 of 21
mgrisoli
in reply to: apullin

It seems even tough the person with the original question posted his assemblies for analisys nobody really gave him a satisfatory answer.

What a pity, I have a similar question.

 

Trying to rephrase:

I have an assemly with 6 parts (let's say it's a cube).

Those parts are all constrained to each other but they are not constrained with the assembly's origin planes.

But, after mounting and constraining the whole cube I realized the anchored side of the cube is not aligned with the origin planes.

If I try to just create a constraint between the "base" of the cube against the three assembly original plane Inventor gives me an error saying there are conflicting constraints.

If I try to manually rotate the whole cube as one single part, it won't let me. It just allows the to free rotate, which is not what I want.

I want to rotate one of the sides of the cube and I want the constrained parts to come along with it.

Or I want to rotate all selected parts on a hipotetical dinamic axis resulting of the selection, not on their own individual axle.

 

How do you recommend to do this?

Message 11 of 21
johnsonshiue
in reply to: mgrisoli

Hi! Based on your description, it sounds like either the rotational DOF is not available or there is implicit ground. I would like to understand this issue better. Could you share your files here or send them to me directly (johnson.shiue@autodesk.com)?

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 12 of 21
0x3FA5
in reply to: johnsonshiue

Hi,

Any news on this issue?

Trying to rotate a block of inter-constrained parts within assembly, but the "Free Rotate" ignores the constraints.

Extremely annoying.

Thank you.

Message 13 of 21
JDMather
in reply to: 0x3FA5

Can you Attach an example assembly here?

I see there was a previous example attached that I can use.

Should be easy to rotate components.

I will upload a video in a few minutes when it is done compiling.


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Message 14 of 21
JDMather
in reply to: 0x3FA5

single component

https://autode.sk/3bfKcTy

 

with multiple components

https://autode.sk/2v2xiYx


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Message 15 of 21
0x3FA5
in reply to: JDMather

Thank you!

So, just combine the parts into internal assembly, move, then demote back into parts.

I was wandering if there is a solution as in SW... After all, this is such a simple task.

Message 16 of 21
JDMather
in reply to: 0x3FA5

@0x3FA5 

I just thought of a way I like better than fooling with demoting/promoting sub assembly.

 

Since the components have some existing constraints between them -

 

Move/Rotate one of the components of the group.

Now Ground that component.

Update and the other components will snap back to the moved/rotated component by constraints.

Unground if desired.

 

I think this even works better in Inventor than my SolidWorks trial.


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Message 17 of 21
0x3FA5
in reply to: JDMather

About 1/10 of the time, after the update, the items that where constrained to parallel axes are rotated 180 ("flipped" axis). So this cannot be trusted...

Message 18 of 21
JDMather
in reply to: 0x3FA5

Attach an example that illustrates this behavior.


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Message 19 of 21
0x3FA5
in reply to: JDMather

I will post it here next time I ran into it, but I like your idea with the assembly so much that probably will use this from now on.

 

Message 20 of 21
JDMather
in reply to: 0x3FA5


@0x3FA5 wrote:

I will post it here next time I ran into it, but I like your idea with the assembly so much that probably will use this from now on.

 


It is only a few extra clicks.

This one might be a good one for the Inventor Ideas.


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