Linear pattern direction

As you know, when you want to define a linear pattern, you give it a
distance, tell it how many, and define a direction. I discovered by
accident that you don't necessarily have to select an edge - you can use a
sketch line or even a dimension for the direction. So, the opportunity
exists to define a pattern direction by some weird dimension that is already
there, if it more accurately does what you want.

WT

 

selecting a dimension is the only way to get the VARY SKETCH option to be
active. This allows the user to change the size of the parent sketch
feature while it is patterned. An example of a drain cover is in the
essentials training manuals.

Hope that gives more info on selecting dimensions
Steve Tietz

 

It's interesting how a person can use a product all this time and not
remember every haveing seen something. I suppose I knew about the vary
sketch at one time, but I certainly didn't remember it.

It's odd that you have to select the dimension that locates the feature from
the edge - you can't use the dimension that is parallel to it defining the
bottom of the part. I wonder why.

WT

 

That is because only the locating dimension can cause the sketch to change
size. Think about a V shape - if you constrain a circle to the sides of the
V The V will control the diameter of the circle, right? Well if you then
dimension from the bottom vertex of the V to the center of the circle,
wouldn't changing that linear dimension cause the sketch to change shape
(diameter) -- or vary sketch.

I hope that makes sense
Steve Tietz

 

Starting with a triangle model with a circle cut dimensioned to a point
and tangent to offset edges of the model.

Doing a linear pattern off of the dimension to the point and got an
error message, but it worked.

Doing a linear pattern off of a dimension from the cicle to a
construction line coincident to the point worked with no error message.

Thanks for sharing about vary sketch. I wasn't familiar.

Patterning items that extrude to surface (as opposed to blind) can
produce similar results of varying features consistent with design
intent.

-Blair

 

At my company we do a lot of symmetrical parts where holes are
symmetric about the center of pads. Typically in my sketch for the
pattern seed feature, I put in centerlines and use the centerlines to
define my hole locations with the doubled dimension tool (just like
dimensioning diameters on round parts). I've known that you can select
the dimensions for the pattern direction, but why can't you select the
dimension to use in the pattern dimension? Seems like you should be
able to select the dimension and it would create an equal relation
between the sketch dimension and the pattern feature dimension. Right
now I go into the sketch and set up linked dimension names to use with
the pattern. It's more extra steps, but at least then my dimensions are
only driven in ONE place instead of 2.