Parametric models and ST?

[pkelecy]

I recently put together a nice parametric model of a part (in SE traditional) that, through the use of a few driving dimensions and relationships, can be scaled to different sizes and have key feature changes. With this I can accommodate all the design variations we might expect for this part. I was very happy with the result.

However, my local SE rep suggested I focus on ST, as "that is the future", which made me wonder how I would do this in the ST environment. My understanding is that once you've create a part (in ST) the sketch you used is no longer active. So is there a way to set up a ST model with variable relations (to keep things in proportion) so you can easily resize and make *expected* design changes? I played around with this a little, but it wasn't obvious how to do this (assuming it can be done).

Thanks for any feedback.

Pat

 

[donyoung]

Hi,
The answer is like that from the Orcle of Delphi: Yes and No
First you are dealing with faces only, the so called 'LiveRules'
can be used to find/collect all faces in a model that share
a common constarint (planer, concentric, ...) and those found
will move/chnage as a whole.
OTH take a C-Channel and put in a circular cutout through both 'legs'.
This is one feature in both modes but in ST-Mode you will be able
the change both cutouts independend of each other including
the deletion/moving of one cutout without becoming the 'feature'
itself invalid. The feature is now only a collection of faces grouped
under a name. After creation they have in common:

- both cutouts are concentric
- both cutouts have the same diameter
- both cutouts are defined by 2 coordinates
- both cutouts share a common name
That's all.

You have to try this on your own -- it's nearly impossible
to put that into a few words.

dy

 

[jeff4136]

> However, my local SE rep suggested
> I focus on ST, as "that is the future"

Get him / her (or jon <g>) to show you how to duplicate your intent using the different modeling paradigm.

-Jeff Howard (wf2)
Sure it's true. I saw it on the internet.

 

[Kenny_G]

To answer your question, dimensional constraints are transferred from the sketch to the model when geometry is created or additional dimensions can be added. Formulas can still be applied between dimensions (they must be locked) which will drive the geometry (using Variable Table or right clicking on a dimension and choose Edit Formula).

Ken

 

[donyoung]

Hi,

sketch dimensions will be propagated to the final
model but
- only as non-locked (previously known as 'driven')
dimensions
- the dimensioning is done by using endpoints or
center points (either implicit or explicit). Other
dimensions might get propagated but can't be used
because they arn't modifiable
(midpoint to center point for example)

dy

 

[pkelecy]

What about relationship constraints, such as lines being collinear, equal, or parallel (I use all three in my profile), concentric arcs, etc - are these all carried over as well? What about construction elements and their relationships with profile elements?

Pat

 

[donyoung]

Pat,

they will not be carried over to the final model.
The final model can be changed by
- using dimensions
- using the steering wheel
in both cases the LiveRules as set will control how
the model will behave during the change. One other
method is to define explicit relationships between
faces of either the same or diferent object.

You may draw a rectangle and dimension all for sides
without the sketch becoming 'overconstraint'. Each
dimension can be used to change the model.
As already mentioned elsewhere: you have to think
different. A feature is now just a collection of
faces that have some in common - not more. A circular
cutout through both legs of a C-beam is one feature
but each of the cutouts can be modified independend
of the other, even a deletion of one cutout will
not invalidate the feature as a whole.

dy