Constrain a curved surface to an edge

[Anonymous]

I want to constrain an edge to a curved surface in an inventor assembly. Namely, the parts that should "tangentially touch" are

this lens

https://www.thorlabs.de/thorproduct.cfm?partnumber=LB1437-A

and this retaining ring

https://www.thorlabs.de/thorproduct.cfm?partnumber=SM1RR

I tried the tangential constrain but all it does is a mess... Do you know the most straightforward way to accomplish this?

Thanks!

[Xun.Zhang]

Hi,

Have you tried Transitional constrain? or try to defined two relatively fixed UCS and constrain those two UCS.

Hope it helps a little bit.

[Anonymous]

Thanks Xun!

However the transitional constrain by itself does not do the job, the ring is misaligned. The solution using two UCS seems a bit cumbersome....

do you have another idea?

[TheCADWhisperer]

Can you attach your assembly here?

[Anonymous]

Sure, here you go. I cut the parts in half (View - Cuts) for better visibility.

[johnsonshiue]

Hi! You only attach iam file. Please attach all iam and ipt files.

Many thanks!

[jletcher]

Is this what you are trying to do?

[SBix26 · Accepted solution]

Here's a modification of @jletcher's model (just the assembly and revised lens).  His has the ring penetrating into the lens.

I measured the diameter of the ring, then used that to split the face of the lens at that diameter, giving a center point to use for the constraint.

Sam B

Inventor Professional 2018.2.3
Windows 7 SP1

[Anonymous]

Thanks @SBix26 that worked perfectly. Little bit more work than I was hoping for, but still.

[SBix26]

Another similar method would be to extrude a cylindrical surface from one face to the other of the lens and use that to constrain the retaining ring.  The surface can then be made invisible and won't affect either appearance or mass.

But there have been many occasions like this where constraining an edge to a face would be very useful without the need for additional features.  I haven't searched the Inventor Ideas forum, but I suspect there is already a proposal to this effect there (and I've probably voted for it, too).

Sam B

Inventor Professional 2018.2.3
Windows 7 SP1

[milkied10]

Another way to skin this cat would be a contact set:

• constrain the centerlines of the 2 parts
• then add them both to a contact set and turn on the contact solver
• carefully slide the lens toward the hole (or just ground the hole) until it contacts and stops
• then constrain the lens into place using the mate (of flush) and some other faces, but using the predict offset to gather the distance of offset the parts are sitting at.
• then turn off the contact set options.

[Lucas.dolinarVFXZU · Accepted solution]

Hello, i would like to add some more info for future users:

The Solution by @SBix26 is Definitly the easiest and quickest i could think of, however it would be better to Project the Edge into a sketch (easier workflow and adaptive). I also recommend creating a Subassembly with these to Components (for ease and to eliminate any problems with adaptivity), and setting its BOM option to Phantom.
Also, Inventor has a much easier time constraining the Parts Surface to the midpoint of the newly created Split.


Another option to constrain these wich seems to be missing here is to constrain the Ring to the Lenses center point. This has the advantage of being Transitional AND more importantly it will work no matter the shape of the ring (see attached file)