Sketch blocks constraining

[Anonymous]

Hi everyone,

I make extensive use of blocks in sketches, but I find it difficult to understand the logic of Inventor 2013 in this matter.

Example:

I open a sketch, draw a two point rectangle, give two (aligned) dimensions to its sides, assign two dimensions of a corner with respect to the origin. Everything turns blue and I'm happy.

Now I press F8 and remove the horizontal constraint which has been put automatically, next I delete the origin. I have now three degrees of freedom, as it must be for a rigid shape in a plane.

My rectangle behaves in the 2D plane of the sketch like an unconstrained part in the 3D space of an assembly. That's exactly what I want: I turn the rectangle into a block for later use in other sketches.

But when I open the block, I find that it has FIVE degrees of freedom. What does this mean?

Firstly, the three DOF for translation and rotation shouldn't be displayed, because there's no way to remove them, because in blocks you cannnot project a coordinate system. I think blocks should have a "local" coordinate systems exactly like parts do. In fact, imagine a complicated block with lots of geometry and dimensions: you miss one dimension and you press F8 to see where it is, and the screen becomes a huge mess of red arrows. You then try to move the green lines to find a clue, but often also this doesn't help because in many cases Inventor gives priority two the translation and rotation DOF.

Secondly, and more importantly, what are the other two DOF? Going back to the rectangle, I try to add constraints: I try to put horizontality to one side. But horizontality with respect to what? But anyway, the DOF are now four. I cannot put any more constraints. I try to use the "fix" constraint to everything. It works, the rectangle is blue, even if Inventor says there are 2 DOF.

Can someone explain me where I'm wrong?

[JDMather]

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@Anonymous wrote:

Hi everyone,

I make extensive use of blocks in sketches, but I find it difficult to understand the logic of Inventor 2013 in this matter.

Example:

I open a sketch, draw a two point rectangle, give two (aligned) dimensions to its sides, assign two dimensions of a corner with respect to the origin. Everything turns blue and I'm happy.

Now I press F8 and remove the horizontal constraint which has been put automatically, next I delete the origin. I have now three degrees of freedom, as it must be for a rigid shape in a plane.

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Stop right there.

Do not delete constraints.

Convert your sketch into a Sketch Block.

The constraints are now relative only to the geometry within the block.

Attach your file here at this point if you can't figure it out.

[JDMather]

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@Anonymous wrote:

.... imagine a complicated block with lots of geometry and dimensions: you miss one dimension and you press F8 to see where it is, and the screen becomes a huge mess of red arrows. 

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When creating a complex block - add one Fixed Constaint - get everything defined and then delete the one Fixed Constraint.

Do not delete any other constraints/dimensions in the block.

[Anonymous]

I tried what you said: it keeps on displaying 4 DOF.

Edit: and if I fix a point, as I said everythig turns blue but still I'm left with 2 DOF.

[JDMather]

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@Anonymous wrote:

I tried what you said: it keeps on displaying 4 DOF.

Edit: and if I fix a point, as I said everythig turns blue but still I'm left with 2 DOF.

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You forgot to attach your *.ipt file here.

[Anonymous]

Here it is. Uh it is Inventor 2014 not 2013 sorry.

[JDMather]

Have you installed all Service Packs and Updates for 2014?

[Anonymous]

Uh, I don't know, I guess the answer is no...

So theese updates remove the problem?

[JDMather]

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@Anonymous wrote:

...

So theese updates remove the problem?

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No - it is not likely that the updates address anything with your blocks.  But the first thing I would do is remove confounding variables.

I haven't had time to investigate the behavior you describe with the blocks.

[Anonymous]

Now that I think about it, the rectangle example, as simple as it is, is unnecessairly complicated.

I tried with a point - a single point. It needs 2 dimensions, but if you turn it into a block, they become three,

as if a point could rotate. I can't figure out a way to impede a single point to rotate.

[JDMather]

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@Anonymous wrote:

Now that I think about it, the rectangle example, as simple as it is, is unnecessairly complicated.

I tried with a point - a single point. It needs 2 dimensions, but if you turn it into a block, they become three,

as if a point could rotate. I can't figure out a way to impede a single point to rotate.

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I think this is all related to pushing out derived assembly.

In my class we do an engine with only simple sketch blocks (lines and a few rectangles - that's it).

But the kinematic motion works in part file as though we were in an assembly (X,Y AND Z motion).

When we push out the assembly the assembly constraints are automatically created.

It all gets pretty complicated.

I will try to post an example when I get a chance.

I do not recall anyone being interested in this functionality since they introduced it many years ago.

[Anonymous]

Maybe I figured it out.

Math sais that a 2D geometry only constrained with itself cannot have less than 3 DOF: two translations and a rotation.

To remove theese, you need to constrain the geometry with an external, fixed, reference frame, which in case of Inventor blocks it's simply not implemented.

Or maybe, let me say it, very poorly implemented. When you build a block you can specify an insertion point (if you don't specify it's automatically set by Inventor in some way, maybe the "center of mass" of the geometry or something like that), and you can also specify if it's visible or not in the same dialog box. So the "extra" DOF are simply the coordinates of this point, which I hadn't considered before simply because it was invisible and I didn't even know it was there.

Anyway, to fully constrain the geometry in edit block mode, one must:

1) Constrain the insertion point with respect to the geometry. After this the block behaves like a 2D rigid body --> 3 DOF

2) Fix a random point, like JDMather said, thus obtaining a rigid body rotating around the fixed point --> 1 DOF

3) Block rotation. Inventor doesn't let you do this by fixing another point (I wonder why) so you can do it only with horizontality or verticality --> completely constrained.

This brings an idea for the developers: isn't it MUCH more consistent to provide blocks with an internal reference frame?