Flip Mate (concentric) constraint

[0x3FA5]

Hi,

When trying to constrain 2 cylindrical items to be concentric, is there a way to "flip" the alignment?

For some magical reason, it is never the correct orientation on the first attempt.

The solution is to apply other mates first, but it is extremely annoying and sometimes really awkward within a big assembly, the useless clicks are driving me nuts!

The Solidworks equivalent would be clicking on "Concentric" then, if required, on "Flip Mates", done:

When doing so in Inventor, the orientation does not change:

Is there some feature in Inventor that I am not aware of?

Thank you!

[SBix26]

What version of Inventor are you using, and what are you actually trying to mate?  Axis-to-axis of two cylindrical faces?  In the last few releases of Inventor you should have a choice of directional mates as well as undirected; in previous versions it was only undirected.  But I don't see those in your screenshot, so I assume you're using an older Inventor, or selecting something different.

Can you give more detail?

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Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn

[johnsonshiue]

Hi! I believe you want to use Insert Constraint (4th button).

Many thanks!

[0x3FA5]

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@SBix26 wrote:

What version of Inventor are you using, and what are you actually trying to mate?  Axis-to-axis of two cylindrical faces?  In the last few releases of Inventor you should have a choice of directional mates as well as undirected; in previous versions it was only undirected.  But I don't see those in your screenshot, so I assume you're using an older Inventor, or selecting something different.

Can you give more detail?

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Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn

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I am trying to mate two cylindrical faces. I am not sure about the internal Inventor's mechanics of this constraint, nor should I care, maybe the actual constraint is translated to axis-to-axis, but 99% of the time I select the cylindrical faces.

I am using Inventor Professional, Build 284.

Strangely, the search has not revealed to me that the idea has already been accepted:

https://forums.autodesk.com/t5/inventor-ideas/flip-command-on-mate-axis/idi-p/4692917

[0x3FA5]

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@johnsonshiue wrote:

Hi! I believe you want to use Insert Constraint (4th button).

Many thanks!

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Insert constraint is actually two constraints: axis collinearity and set offset. I find very limited use to this option, maybe used it couple of times only.

I want to use exactly what I described: easily flip orientation when mating concentrically of the cylindrical faces.

If the next constraint is not offset, but tangent to face, the "Insert Constraint" is useless.

I see this idea was accepted, was it implemented in the recent versions?

https://forums.autodesk.com/t5/inventor-ideas/flip-command-on-mate-axis/idi-p/4692917 

[SBix26]

What year version of Inventor are you using?  This particular constraint type was changed in the last couple of versions, so it matters especially in this case what version you're using.

In general, if you are mating two cylindrical surfaces to be concentric, you will be mating the axis of one to the axis of the other.  Axis is the default selection when picking cylindrical surfaces, and you can see it because the axis highlights along with the face.  Note that you can also use Select Other to select the actual face for a Mate constraint instead of the axis, but this is not useful in the case that you're asking about.

But after that it depends which version of Inventor you're using, so that's the next piece of information needed.

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Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn

[JDMather]

Attach your assembly here.

I make extensive use of Insert constraint (sure wish SolidWorks had this one), but I understand it might not be what you need in this case.

What I don't understand is, what do you really need?
I think your actual assembly will answer that question.

[0x3FA5]

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@JDMather wrote:

Attach your assembly here.

I make extensive use of Insert constraint (sure wish SolidWorks had this one), but I understand it might not be what you need in this case.

What I don't understand is, what do you really need?
I think your actual assembly will answer that question.

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@JDMatherit becomes interesting...

While preparing an assembly to send here, I tried the "Joint - Cylindrical" again, and it worked! It did exactly what I wanted. Why it was working incorrectly with exactly the same assembly but under different name - mystery..

I needed to align cylindrical items concentrically, and flip the alignment as required.

The "Constraint -> Assembly -> Mate" always aligns incorrectly.

I need to investigate more, why the "Joint" didn't work earlier..

[SBix26]

Way back in your first post you asked if there was some feature of Inventor that you aren't aware of.  The answer is that Inventor 2020 and 2021 (maybe 2019, too?) have explicit vector solutions for mating of axes-- Aligned, Opposed, and Undirected.  You can select the one you want in the Constraint dialog before accepting.  This addresses your complaint, but requires updating to a more recent version.

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Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn

[0x3FA5]

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@SBix26 wrote:

Way back in your first post you asked if there was some feature of Inventor that you aren't aware of.  The answer is that Inventor 2020 and 2021 (maybe 2019, too?) have explicit vector solutions for mating of axes-- Aligned, Opposed, and Undirected.  You can select the one you want in the Constraint dialog before accepting.  This addresses your complaint, but requires updating to a more recent version.

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Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn

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Thank you, looks like what I was looking for!

I am just curious, how can you align vectors, with "Undirected" option?? Why not to call it "Align to Closest"?

Have Autodesk invented undirected vectors?

[SBix26]

I believe you're using Inventor 2018, right?  Undirected is the only choice you have, and that's the way it was from the beginning.  It's not that the vectors aren't directed, it's just that the solution works either direction, and, as you suggested, seems to use the solution that involves the least rotation.  It just means you have to place other constraints first, if possible, forcing Inventor to choose the solution you want.  Or, use the Free Rotate tool to get it close before using the Mate constraint.

In any case, I recommend upgrading to 2020 or 2021; we're a third of the way through the update cycle to 2022...

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Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn