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
SteveT wrote:
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.
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