Smartets way to distribute space between 2 retangular assemblys?

[cahoe]

Dear folks... yet again.

Now how do I smartest align two assemblys to same center point or distribute even space on 2 sides of the attached par example?

[tsreagan]

If you Constructed your parts centered about the origin and origin planes.   Then

In the assembly,  use the constrain tool and constrain the origins. (procedure below)

expand part1 folder

expand part1 origin folder

hit constrain button

pick "Center Point" of part1

expand part2

expand part2 origin folder

pick "Center Point" of part2

then ground them

If the individual parts share an origin, they they will be properly aligned.

If they do not share origin, it is more involved.  You will have to create planes in each part and align them.

or constrain with an offset to one edge,  though if the part dimensions change later your symetry will be affected.

2014 has a new symetry tool,  that should be used if in 2014.

(I havnt tried it yet, look into it)

If they share center planes but not center points  (not at same elevation)

then use the same procedure,  and instead of center point,  constrain the center planes in the same manner

you will have to consider the planes direction in this case however

T.S.

[cahoe]

Whoaa.. your monster and snappy as h*ll!

100 thanks!

Edit:  I'll need to make the origin points vissilbe.. right?

[tsreagan]

100 welcomes

T.S.

[jddickson]

There is several ways to do this:

1. You can put a plane on each assembly using overall length in the parameters /2 to set your plane to always be centered. When you do this to both assembles you just have to constrain your center planes together.
2. When you make the length and width pieces you could extrude both ways making your planes centered on your part. Do this on both assemble. You can then turn on the planes to constrain them together.
3. You can just use parameters if you want. Use the long assembly length and minus the short assembly length and divide by 2. Use that to drive the constraints.

There are a lot of other ways to do this these are just a few.

Hope this helps.

[cahoe]

Uh.. but center planes?

I got YZ, XZ and XY planes. But not center planes... as far as I can see

[jddickson]

When you make a part you can make the YZ, XZ, and Xy planes be centered on the part (using the planes as center planes).  Or on the 3D model tab under Work features you can add a plane to make it centered.

Tsreagan way is one of the fastest but be careful doing it that way. Make sure your origin planes are centered on both assembles. Also if you change one of the assemblies off to one side of your origin planes then it will not be centered anymore. But no matter what way you do it you have to pay attention to your constraints.  

[tsreagan]

cahoe

If you are just starting out,  mastering this tip will help you through the coming years of inventor.

Under the Origin Tab for any part or assembly you will find.

Three planes

Three axis

One Center Point

These are the all important datum objects that ALL inventor files share.

These never move, and cannot be deleted.

If I am making a bolt like object:

        When thinking about placing this back into an assembly

        The most usable point is the spot where the head meets the shaft.

 

You can even add offsets just as you do when constraining "screen selected" geometry.

Remember these datum ojects are always there and can help make parts that are easy to constrain.

Not to confuse you but there are many ways to develop the assembly,

You can create the components a part at a time, placed into the assembly after they are created,.

Or model all the components together in one part, then save the pieces as seperate part files.

Or model the parts "In Place" in an assembly.

Read up on these methods now,  the approach you choose will greatly affect your process from there.

Reffered to as designing from "BOTTOM UP" or from "TOP DOWN"

This covers it in a lot of detail. 

http://en.wikipedia.org/wiki/Top-down_and_bottom-up_design

There are some recources here(the forums)  that cover it in the context of inventor.

T.S.

[cahoe]

T.S .. you are so wonderfully awsome. Thanks

(love this place)