Joint Origin challenge with a parametrically tilted component

[ericjforman]

I'm making a rigid joint to place a disc tilted on an angle centered on a rod. The disc will tilt to match the face of a derived Shaft Collar component whose angle can change. There is no way to select a joint origin at the correct point because the point is unknown UNTIL it is tilted in place. I tried manually creating a joint origin with a sketch, but the projection links from the rod are not correct projections after the disc is tilted. (No error shows up but you can see they are in the wrong place despite showing as valid projections.)

Basically I need to make the Joint Origin after the joint, but I obviously can't make the joint until I have the origin.

I tried a sliding joint instead, with joint at center instead of face, with an offset of half the disc thickness, that fixes the centering issue, but still didn't work either because the offset is only actually half if the tilt is zero degrees, it needs to know the tilt first. Same Catch 22.

I could do some extra math steps I suppose with pythagorean calcs based on a driven dimension from the derived component face angle, but is there an elegant, better way to do this? 

File: https://a360.co/462eKXN

Thank you!

 

 

[ericjforman]

This is my multi-step clumsy workaround, make a sketch to do the math, change Rigid to Sliding joint, choose a custom axis derived from the Rod, then set a Maximum - but I suspect the Fusion headz here will have a smarter way...

 

 

[davebYYPCU]

Joints work with a common and known point in both components.

The centre point of the top face sketch ellipse in the clamping disc, should be joined to the centre point of the top of the rod, and dropped down by an offset - can replace the Slider Joint if you wish.

As for the centre point of the top face sketched ellipse, in the clamping disc, you have too many to choose from, and some are not coincident, because there should be 2 lines in this list.  Pick an endpoint for the correct vertical centre line.  I put a Joint Origin there for pictures, but you don't need one, at the time of assembly, a snap point is easy to find.

The same point of the top aligned face the ellipse, in the clamping disc, should be joined to the centre point of the bottom face of the big disc elliptical cut out.

Or put another way, the big Disc is flush mounted (inside faces) to the clamping plate, and then both are dropped down.

As for not knowing the inclined angle, seems to come from the clamping disc - derived into the file. 

Noted that fully defined Derived sketches arrive in destination file as not fully defined - dangerous!

Might help...

[ericjforman]

Thanks @davebYYPCU - I understand all of your points (although btw choosing the joint snap point on the shaft collar aka clamping disc is not in fact easy, in Fusion an annoyance is that the center point of those profiles appears with snaps on but cannot be selected because it's in the gap between halves, so when you mouse off of the face it disappears, see screenshot below), thus I had to make an extra sketch point in "nut-bolt plane," not a big deal but annoying).  

 

However, this part of what you said is the problem posed in my question:

...clamping disc should be joined to the centre point of the bottom face of the big disc elliptical cut out

A) The center point of the bottom face is not the correct joint origin, as detailed my post.

B) The center point of the cut-out would be correct, but the cutout can't be performed until AFTER the joint is made.

I still don't see a way other than my workaround to have the joint be centered without a manually calculated offset. Or am I misunderstanding you?

Perhaps this will help clarify:

 

And yes btw the disc, when made very small to emphasize the point, does look odd from one side but is in fact correctly centered with this method.

[davebYYPCU]

So that I am on the same page,

I have an example file, dumbed down to see if I have the four bodies the right shape and position.  Can be parametrized if the geometry in general terms is correct.

Might help....

[ericjforman]

Thank you for giving it a try. That doesn't work. If I change the angle to 45° for example, the disc is not centered correctly. (Also your thin extrude wall location should be Center not Side.) And, regardless, my question is about using a Joint.

Here's your file with corrected sketches and labels: https://a360.co/3FXez5A,  if you want to work with that instead.

[davebYYPCU]

Ok, I see you fixed the length of Extrude 1, and the thin extrude, 

The missing line from point 2 in the second sketch will fix your problem.

Now you can set up parameters and components for Joints.

Joint the midpoint of the top of Collar to position 1. Adjustment for the Rod Position may be needed.

Joint the Centre of Mass in the Disc to position 2.  The length of the line (D) at point 2 is half the Extruded disc height.

At first, I was thinking the Joints were to be at the same place, was all sorted in my file to what you do need.  

Set the angle - this line is missing in your file.

Might help...

[laughingcreek]

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@ericjforman wrote:... in Fusion an annoyance is that the center point of those profiles appears with snaps on but cannot be selected because it's in the gap between halves, so when you mouse off of the face it disappears, ...

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when you see the snap points, hold the ctrl key down and then mouse over to the point you want.

[TrippyLighting]

Before getting to "deep in the weeds" I would recommend you start fully constraining and dimensioning your sketches.

Looking at the Clap Collar Two Piece, the first sketch defining the main dimensions is already not fully defined. That sets alarm  bells off 😉
Als mirroring sketch halves is not a good practice!

[laughingcreek]

*

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[TrippyLighting]

Attached ins one way to do it.

You could also favorite and derive the parameter for the angle from the collar to the destination design and work with that.

[ericjforman]

Thank you @TrippyLighting - the unconstrained sketch was just one center point that somehow lost being snapped to origin center - I fixed that. I also got rid of the mirroring - why is mirroring bad, just because it's more computationally intensive? 

Any way, I see your approach is simpler, to model the disc from a projected angled collar face rather than let the joint tilt it to match. And then to make the rigid joint before the disc is - symmetrically - extruded. I guess I was stuck on the practice of making the component bodies first, then making the joints between them. 

How did you select the joint snap in the Disc component? When I try to re-create it in your file, it shows the snap way off to the side, and I am unable to select the center point like you did.

[ericjforman]

I don't know why the screencast looks so low-res, I uploaded it at full resolution, but hopefully you can still see the issue...

[TrippyLighting]

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@ericjforman wrote:

...

How did you select the joint snap in the Disc component? When I try to re-create it in your file, it shows the snap way off to the side, and I am unable to select the center point like you did.

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Hide the rod so that only the sketch is visible. Otherwise the joint will try to snap to the rod.