Looking for a constraint hack

[johnEE7T4]

Hello,

Would the Inventor User Team know if there is an app add in where I can easily automatically center a constraint about an object? Currently I use planes as construction to do this but I am hoping that when I want to constrain two items that I have a pop that asks to "select the face you want the item constrained to" and the item would automatically be placed centered on the face of the mating part. 

Like if I had a flange and wanted to constrain it to a plate in a central location.

I guess most would constrain to an edge and then offset. 

Thanks for reading.  

[CGBenner]

@johnEE7T4 

Hi.  A picture of what you are trying to assemble would really help the group to understand your need.  From your description this sounds like maybe something you could do with iLogic?

[mcgyvr]

Your description got a little confusing as you seem to initially be talking about centering 2 objects about each other then talk about centering one on the face of another so as stated an image or even better would be to post the iam (and ipt files) showing an actual example and we can tell you how it should be done..

But in general when a part is modeled centered on its origin planes you can simply use its origin planes to center it about "something" be it the face of an object or the center of another. 

See here.. https://blogs.rand.com/files/the-born-technique.pdf

[CGBenner]

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@mcgyvr wrote:

See here.. https://blogs.rand.com/files/the-born-technique.pdf

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Every time I see a post that mentions the born technique, my brain goes to "This must be the latest in the saga of Jason Bourne.  The Bourne Identity,... the Bourne Technique... " My brain is a strange and sometimes frightening place.  😂

[JDMather · Accepted solution]

If not modeled using the BORN Technique, then Workpoint  - Center of Edge Loop.

Attach assembly here if you can’t figure it out.

[johnsonshiue · Accepted solution]

Hi! I believe the OP is looking for the equivalent workflow of SWX's Width Mate in Inventor. Such constraint does not exist in Inventor. You will need to create a mid plane in the target part. Then you may constrain the other component to the mid plane.

Many thanks!

[James_Willo]

Depending on your geometry, you may also want to look at using the joints command for centring something. 

Joints quite often have a node right in the centre that you can 'mate' to. 

It's particularly good for slots. 

[johnEE7T4]

All,

Thanks for taking the time.  I apologize for the vagueness of my post but lets say you had a 3 x 5 inch rectangle and you wanted it centered on a 11 x 14 rectangle.   

I was looking for a way where the app would ask me to touch of the 4 faces (x and y) of the part that I am trying to center and the 4 faces (x and y) of the part it is to be centrally located on. 

After doing a quick investigation on the net I discovered there is really no such thing and there are actually rants by some migrators from Solid Works Users that the tool johnsonshiue referred to doesn't exist in Inventor.

If it were a round flange to be centrally located on a rectangle....I would think you can just touch off or click on the flange and it would find the center point automatically. 

[James_Willo]

Hi, please look at joints, in most cases it will do what you want. 

[James_Willo]

See this screencast for a quick demonstration. 

Obviously with more complicated geometry there may not be a node right in the centre where you want it:

https://autode.sk/3LC1lsF