How do I properly constrain this?

[shoopdawoop]

Hi.  As you can see from the screenshot, this system is comprised of three parts.  The smaller part (part a) is inserted into the main part (part b) axially, and there is a slot cut away from part b through which a cam pin (part c) is inserted through both parts b and a.  What I need is for part a to rotate, but under the constraint of the cam pin/slot relationship.  My problem is that I have no idea how to do this.

I've tried simply making all of the parts part of a contact set, but Inventor doesn't understand that when I rotate the inner part, I want the rotation to be constrained by the slot/cam pin relationship, i.e. I want the cam pin to slide along the slot, and the contact program breaks.  

I've tried creating a joint/slider relationship between the cam pin and the slot, but I can't figure out how to orient the cam pin properly for this to work.  

Even if I could create that relationship properly, I would still have another problem: I need not only a sliding relationship between the cam pin and the slot, I need a rotational constraint wherein the cam pin remains equidistant from the x axis throughout the movement.  There is actually another long part which goes through the center of all parts of the assembly, including the end of the cam pin.  That part is centered axially on the x axis, so if the cam pin does not remain equidistant from the x axis throughout its movement, there will be interference.  

Because I didn't know how to wrap the slot sketch around the cylinder, the slot was created via an extrusion from a 2d sketch, so the side wall of the slot is therefore a simple, straight plane, that may have implications here.  

Can anyone help?

[WHolzwarth]

Well, you'd be better off with easier tasks.

I've seen these issues:

- Your Sketch29 has a total of 4 lines. That's the reason for following errors. I've left only the long line

- Your Sweep2 has no rectangular profile relative to the path. Therefore you get the bad looks of Fillet8

But, as mentioned before ..

[shoopdawoop]

When I try to sweep, I get the error, "Rail does not intersect profile," etc.  But I created the work plane ON the endpoint of the rail!  It's been giving me this error message the last few times I've done this, and I've been just accepting it and going on.  What does this **$%ing program want me to do?  How should I create the on which the profile will be sketched, if not by using the parallel to plane at a point command?  

[shoopdawoop]

How do you get a rectangular profile relative to the path?  

[shoopdawoop]

You know what the most frustrating thing is about this software?  What I want to do is so simple.  All I want to do is make a keyed slot in a cylinder, and obviously, it's possible.  I have what should be the instructions right in front of me; I should be able to simply do what you did, step by step, and obtain the same results.  But I don't.  It simply does not work.  I think I hate this software.

[WHolzwarth]

Yes, some care must be taken.

As mentioned before, you need a rectangular section relative to the sweeping path for good results:

- 3D Model -> Work Features Group -> Plane -> Normal to curve at point -> Select path and one of it's endpoints

- Sketch rectangle at this plane with actual groove thickness. Project cut edges. Constrain the rectangle tangental to the cut, and constrain both midpoints of small edges appropriate.

- Sweep it (Option path and guide surface)

- Do a full round fillet at both ends

Relax ..

[shoopdawoop]

I was getting so angry at Inventor last night, but I was just doing it wrong.  I was creating the work plane parallel to the origin plane, instead of normal to the end of the rail.  In hindsight, it seems so obvious.  

I still get the 'rail not intersecting profile' error message.  Should I worry about that?  

[shoopdawoop]

...and thank you!

[WHolzwarth]

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shoopdawoop schrieb:
 

I still get the 'rail not intersecting profile' error message.  Should I worry about that?  

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That shouldn't happen. Attach your actual IPT.

[shoopdawoop]

I was able to create the slot despite the error, but now I'm having problems constraining the pin in the slot.  For some reason, when I attempt to place a tangential constraint between the pin and the slot wall, Inventor wants to put the pin on the *outside* of the slot, rather than the inside.  When I attempt the same operation in your assembly, it constrains inside the slot.  Why does it not work for my assembly, but it does for yours?  Is this related to the 'profile not intersecting guide rails' error?

[WHolzwarth]

The tangent feature menu has two possible solutions. Try the other one.

[shoopdawoop]

I swear I tried that a few times before posting, and it constrained the middle of the cam pin to the slot face so that the pin was halfway inside the bolt carrier.  This time, for some reason, it gets closer to what I want, but the cam pin is still not sitting in the middle of the slot, and is therefore interfering with the slot face.

[WHolzwarth]

Hmm. I took a closer look at the results of a slot done by sweeping. All are not ok, the error depends on the angle relative to the axis, and the ratio between slot and diameter.

Look at the screenshot. The red area is the result of a thickened surface, it's ok for pin movement. Compared to that the sweeps are too narrow near the axis. Forget what I wrote before about sweeping for pin and slot combinations, it's not ideal.

Now I'm wondering about a reliable solution for a conical pin in slot.

[shoopdawoop]

Okay!  I have the correct slot geometry created with a thicken command, and the pin is constrained to the slot and slides back and forth as it should, but when I try to mate the cam pin to the bolt hole, there is a conflict with the cam pin/slot wall tangent mate.  

I've attached the assembly with the two conflicting constraints suppressed.

So close!  So close... 

[WHolzwarth]

Here we go again. Exchange the new files. And look at the screenshot. Pin is placed now very well.

[shoopdawoop]

My goal here isn't just to end up with an assembly that has what I want.  My goal here is to learn how to do this.  

What I'm trying to figure out is why, when I tried to constrain the pin tangent to the face of the slot, did the constraints conflict with each other?

Alternatively, what did you do differently which allowed the constraints to cooperate?

[WHolzwarth]

Did you notice that I added OffsetSurface1 to Bolt Carrier Cam Pin.ipt?

[shoopdawoop]

I see that now!  

So... I never would have guessed to do that, and after looking at it and replicating it in my assembly, I still don't understand how offsetting the surface allows the constraints to play nicely with each other.

So this (hopefully) is my last question: how did that work?  

Man, I can't thank you enough for helping me through this.  Yesterday, I was literally yelling at my computer because nothing I did was working.  Today, I have a constrained, functional assembly.  Thanks for bearing with me on this.  I'd buy you a beer if I could.  🙂

[WHolzwarth]

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shoopdawoop schrieb:

So this (hopefully) is my last question: how did that work?  

..  Thanks for bearing with me on this.  I'd buy you a beer if I could.  🙂

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How did that work? Sometimes it's better, modeling exact geometries without thickness differences. That means a 10 mm pin moves in a 10 mm slot. In real life, for sure, that's too narrow, but ..

On the other hand, I've been looking at my above screenshot and I saw no reason, why a smaller pin could be placed tangential to the slot as well. Take it as it is.

Many thanks for the beer. Over here in Germany, we buy this stuff only in crates ..

[johnsonshiue]

Hi! The way to make this particular movement in Inventor is indeed unintuitive. There is room for improvement for sure. Let me explain the technique Walter uses a little bit more so you can understand why the offset surface is needed here. Transitional constraint is defined between a moving face and a transitional face. There are two conditions you will have to understand in order to obtain desirable result. 1) Transitional face has to be bigger than moving face. 2) If a face on a solid is selected as transitional face, actually, it means the moving face can transit on the entire solid. Sometimes, this behavior can be confusing because the user anticipates the transition only happens on the selected face. However, the scope is much bigger than that. The offset surface mainly helps to define the scope of transitional constraint. Also, it ensures the pin is always normal to the cylinder.

I am very sorry for the trouble you have been through to set up this case. Fortunately, we have experts on the forum ready to help out on a regular basis.

Many thanks!

[shoopdawoop]

Okay, so the pin is the moving face, the side wall of the slot is the transitional face, and an offset surface is necessary for Inventor to properly mate the two in a transitional constraint.  Why does Inventor allow the moving face to transit on the entire solid as opposed to limiting movement to the selected face?  That behavior was definitely confusing, to the point that I began yelling at my computer out of frustration.  I'm curious: what was the reasoning behind that decision?  

Also, in what way does the offset surface help to define the scope of the transitional constraint?  Is the way in which it helps define the scope dependent on the size of the offset surface?  I tried making the offset surface on the assembly much larger, and the cam pin jumped to the side of the bolt carrier, so I presume this is the case.  

Thanks for chiming in here.  You're definitely right: there are helpful (and very patient) experts here, without whom I'd be completely lost.  Without their help, I would never have thought to create an offset surface to help define the scope of the transitional constraint.