Constraint / Assemble

[jimmy760]

I'm clueless as to which constrains or assemblely properties to assign in order to make a rectangle slide only up and down through a plate.

I've attached the assembly file.

So my question is how do you do this?

[SBix26]

For this particular assembly, it is very simple-- correct your two parts so they are constrained to be completely symmetric around the origin. For the Vertical Part, edit the sketch and remove the constraints to the origin point from the lower left corner, then place a construction line between opposite corners and constrain the mid-point of that line to the origin point; edit the extrusion feature and change it to extrude symmetrically.  For the Base Plate, edit the sketch and in the same way constrain the center of the cutout to the origin point.

Then you simply constrain two of the origin planes of the Vertical Part to be flush or mated to the corresponding origin planes of the Base Plate.  For other cases where your parts aren't neatly symmetric, you might need to create some work geometry to accomplish the same thing.

One other way of doing this in your particular case would be to mate constrain two faces of the Vertical Part to two faces of the rectangular slot, but that only works because they are exactly the same size, which you would never do in real life-- there has to be some clearance for movement and for manufacturing tolerances.

I can't post files for you, because I don't have Inventor 2012 installed on my home computer.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[jimmy760]

Hi Sam.

Thanks for replying.

Great instructions, I'm just not fully getting it though.

For instance "Vertical Part.. remove the constraints to the origin point from the lower left corner"

How exactly do you do that?

I'm thinking you mean to remove the dimensions.. width and height? I just redrew it away from the center > +

Gave up half through though.

I don't get this, I know cylinders align via assemble constraints for up and down motion only without much hassle but a rectangle is very difficult.

[SBix26]

Easiest is just to delete the four lines (but not the projected origin point) and place a new rectangle roughly centered on the origin point, then place a diagonal construction line on the rectangle and constrain its midpoint to the origin. (Note: in 2013 there is a 2-Point Center Rectangle tool that does this for you).

But if you want to save the rectangle, another method is to delete just the origin point, move your rectangle a bit, then use Project Geometry to project the origin point into the sketch again, and follow instructions from there.  Or, if you're really **** about keeping everything (as I sometimes am), hit F8 to show constraints, then delete the coincident constraint from the lower left corner and re-constrain the sketch as I suggested above.

A shaft in a hole is easier because only one constraint is needed: mate the two axes.  But a polygonal shaft requires two constraints, and there is not a naturally occuring axis (as far as Inventor is concerned).  It just means a little bit more work, but it's work we all enjoy, right?

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[jimmy760]

Have a look at this image.

Do I got it or am I sadly mistaken?

[jimmy760]

It works though.

[SBix26 · Accepted solution]

If it works, then I think you got it.  Don't forget, though, what I wrote earlier about clearances: in the real world of designing stuff that has to be manufactured and used, you can't make moving parts like that the exact same size.  There has to be a little bit of clearance for easy movement, and there has to be allowance for manufacturing tolerances.  That's why we designers and engineers get paid the big bucks...

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager