Global Variables in Assemblies

I'm trying to figure out how I can set variables in my main assembly
and then be able to select that variable value as a linked dimension
when dimensioning new parts in the assembly. So far the only way I can
get my variables to to show up is if I put them in the individual
models. Whats up?

 

What I think you mean by "variable" is called a linked value in SolidWorks.
Linked values are limited in scope to the document being edited. If you
edit a component within an assembly, linked values will be limited to that
component.

There is no way to automatically make a value in an assembly available in
all referenced documents. This would be a good enhancement request.

If you create a matching linked value a the component, you can drive that
with an equation in the assembly. You will need one equation for each
component that needs the value. A third option involves externally linked
design tables referencing each other, but that's so ugly I've never heard
of anyone actually using it. A few have tried to implement it, but I never
heard a report of success.

You can create in-context references of some kind on a per-use basis, such
as equal length constraints, etc. This would be the method implemented in
skeletal modeling techniques. I would recommend looking up skeleton models
in the best practices section of the customer service portal. Maybe they
call it tips and tricks now. At any rate, skeletal modeling seems to be the
best way to take advantage of the tools available in SolidWorks.

 

Dale,
Thanks, I'll stop pulling my hair out now.
I guess I could just create a sketch in the assembly that contains
lines that will represent all the different variables that I need and
then just create in context relations when creating the individual
models. I'll also check out the skeletal modeling.

 

It sounds like you've got the basics of the idea. Take all those different
length lines and rearrange them into a layout sketch, and you'll be almost
there. Put the layout sketch into a skeleton part so you can insert it into
subassemblies. That way you can edit your subassemblies without loading the
top level assembly.

 

That makes great sense, thanks again.

 

Hi Dale,

I use a skeleton sketch part as well but this conversation reminds me
of MDT which had a great global variable system. First, you had a
text file whose name and location was a document option in the file.
Into this text file you typed anything you wanted - one variable per
line. i.e. wall = .08. Then, as you were dimensioning a sketch the
dynamic dimension would display as "d4 =" and you could just type
"wall" and hit enter. (the 4 would be a variable number - incrementing
as you added dims). Other by-products of this great system were the
ability to easily reference other dims i.e. after entering d4 = wall
(which would evaluate to .08) you could edit it to say wall + .01 -
and it would PRESERVE that numeral as you entered it. So, months
later you could edit a part an see something like d4 = wall + .06 - .
02 or whatever.

The next usage of this system was you could reference other dims as
simply as entering d5 = d4 / 2 or any other common mathematical
functions. It's hard to convey how simple and elegant this system was
compared to solidworks method of link values and the equation editor
(although the down arrow tip helps a lot!).

Zander

 

Dont know how many parts you have in your assemblies.

If it more than a few hundreds I suggest you remove all external
references after you are done with the construction, and then fully
define them manually afterwards.

The way the above usage of skeleton parts is described it is very good
for smaller assemblies with only on person working on it.

 

The way the above usage of skeleton parts is described it is very good

Interesting. I would think that skeleton modeling would be essential for
managing a large project with several designers. Is performace the primary
limitation?

 

Yes it is related to performance.

We do use skeleton parts as well. But we use them more to have the
different sub-assemblies defined according to origo.

Basically we have a sketches on different planes on the skeleton
planes. To keep the overview. And then each sub-assembly has the
skeleton part as its first part.

In this way we use the skeleton part to keep the design overview,
basically we just use it for placement (make an external mate to place
it and then delete the external mate, and remating it to the 3
standard planes).
This also allow us to compare any sub-assemblies in a new assembly, by
simply dragging them into origo.

We have to do this to have a chance to work at all. When done with the
construction, we make as-build parts of the assemblies and collect
these in a top assembly (saving each assembly as a part). Otherwise we
cannot open it. We just made one of the biggest Flexo Printers in the
world, and are just working on being able to make some top-assemblies
that can be used for documentation.

Our sub-assemblies can be up to 10k parts, and the top assembly could
be more than 100k parts (though only 15k different parts).

For those interested, please take a peak
http://www.tresu-converting.com/

 

Our sub-assemblies can be up to 10k parts, and the top assembly could

I believe that may qualify for the "large" assembly category. Also, you
have confirmed how I expected skeleton parts would work in such a project.

 

UG also works something like this. Great feature. I sure wish
Solidworks would add this type of functionality rather than all the
eye candy.

 

Yep. I've run into this "global variable" problem. I'm new to SW so I
might be doing something wrong but I can't seem to create external
references to equations or linked values that exist in other parts.
So there doesn't seem to be any way of creating true "global"
variables
in SW.

I'm resorting to "solving" the problem by creating a
"variables.SLDPRT"
that has sketches with construction lines or circles with dimensions
attached and then externally referencing these dimensions through
equal length constraints. The problem with this is sometimes you don't
want "equal" instead you may want D1+.001 to account for an
interference fit or something. Then you have to either add a secondary
equation to a construction item that is equal in order to add +.001 or
you have to make a really complicated tangential construction
configuration with a "distance between" dimension to .001. The
tangent/
construction is necessary to constrain the solution to be on the
desired
side of the line or circle. A total pain! (The secondary equation is
easier.)

What SW needs is the concept of a "project" and any part or
assembly created as a member of the project would have a scope
of equations, design table elements and variables that reference
the project. FOr instance, "D1@Sketch1"=Diameter@Project
would reference the equation or design table element named
"Diameter" that was designed for the project.

my frustrated $0.02.