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## Inventor General

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Posts: 131
Registered: ‎01-03-2013
Message 1 of 4 (336 Views)

# Inferred "constraint" or measurement in Inventor

336 Views, 3 Replies
03-05-2013 11:14 AM

This is a very elementary question, but I'm wondering if I can create an inferred constraint or measurement or parameter (or something) within an assembly which Inventor can use to calculate other parameters. This very simple within a sketch using driven dimensions, but I don't know of anything similar when working with asssemblies.

Basically, here's my situation. I've got two plates placed where I want them, constrained one inch from the edge the baseplate they're sitting on, and I want to place two more plates equally spaced between them. I want to be able to change the size of the baseplate (therefore changing the distance between the outside plates) and for the inside plates to automatically adjust so all four plates remain equally spaced.

If I could create some sort of "inferred parameter" which measures the distance between the two outside plates (call it d0), then I could just constrain the two inside plates at a distance of d0/3 from the outside plates. But if I try and create a constraint between the two plates, and call the offset of the constraint d0, then if I change the size of the baseplate, the two outside plates will have a conflict between the constraint that keeps them one inch from the edge of the baseplate (which I actually want) and the constraint that keeps them d0 apart (which I only used for parametric purposes).

Does anyone know how I can create such "inferred measurements" for parametric purposes? Thanks in advance for any ideas!

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Message 2 of 4 (331 Views)

# Re: Inferred "constraint" or measurement in Inventor

03-05-2013 11:27 AM in reply to: DRoam

In your parameters in your base part note which paramter is its length or width, whichever you want to use as your overall. In your assembly go to parameters and select link at the bottom. Find your base part and select it and choose which parameter you want. Then when you apply the mates use that parameter which is now linked to the assembly and in its parameters by selecting the little arrow where you type in the measurement and choose list parameters and choose the one you linked to. Then any appropriate math to alter that length (ex: d0 /2).

It will help if you can name that parameter in the base part a unique name or create a new one with a unique name and type in the paramet wanted. If d1 is the one you want make one called Overall and type d1 for its result. Then use Overall as the one to link to. This way no matter what size the base part ends up being your mates will always be constrained at equal distances.

Steven White
Lee C. Moore, Inc.
www.lcm-wci.com
Inventor 2011
Intel Dual Xeon E31225 @ 3.1 GHz CPU
16 GB RAM
Windows 7 - 64 Bit
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Posts: 2,497
Registered: ‎03-08-2006
Message 3 of 4 (328 Views)

# Re: Inferred "constraint" or measurement in Inventor

03-05-2013 11:34 AM in reply to: DRoam

Hi DRoam,

In addition to swhite's suggestion you can try these:

You can name a parameter in the Constraint dialog box for the first constraint and then just type that name into the other constraints. For instance when you constrain the first plate from the edge, rather than entering just a value of 30mm, you would enter Offset_Distance = 30mm (recall that you can't use spaces in parameter names) then you can type or paste that parameter name, Offset_Distance, into all of the other constraint values inputs.

Or you can go to the Manage tab and click the Parameters button, and then create a User Parameter for the common value, such as Offset_Distance, then you can just enter that parameter name, Offset_Distance, into all of the constraint values inputs.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

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Message 4 of 4 (315 Views)

# Re: Inferred "constraint" or measurement in Inventor

03-05-2013 12:14 PM in reply to: DRoam

Another technique is to create a master "skeleton" ipt file that has sketches for position in the file.

Then you constrain your parts using the skeleton for reference.

Any time you need to move a reference simply double click on the dimension in the skeleton.

or

Multibody solids.....   pushed out to assembly.

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