I'm looking for a radial pattern for my holes but SE 16 always selects a rectangular pattern instead. I can pick a hole on a round face but can't seem to get the RADIAL pattern option - it always selects the other. Any idea what I'm doing wrong?

I’m a new user, not had my training yet.
But I think you’re trying to do it the ‘Fast’ way and not the ‘Smart’ way.
These are two options that are available to you from the ‘Ribbon Bar’ toolbar.

BTW
I’m having a similar problem. I can’t produce a line of holes. Keep getting a rectangular pattern.

Would appreciate some help.

SB

In the features and relationships tool bar, there is a button for either circular or rectangular patterns. In V16, they could be on the same flyout (I am using V17 and they are separate buttons).

The Fast and Smart options have nothing to do with Rectangular or Radial patterns. The Smart option is used if the feature/s being patterned cross additional faces that the parent feature did not, or shanges shape on the original surfaces that the parent feature interacts with.

The rectangular Pattern has 3 options to define the occurences
Fill, Fit and Fixed
Fill will "fill" the pattern rectangle with feature based on a user defined distance until it runs out of room in the rectangle. To create a single line in the X axis, set the distance in the Y axis greater than the rectangle size. The rectangle can be constrained to the part edges so that it update with other changes to the part.
Fit will "fit" a user defined number of occurences in the rectangular area and will adjust the distance based on the rectangle size. To create a line with this method in the X axis, you would set the Y axis occurence count to 1. The rectangle can be constrained to the part edges so that it update with other changes to the part.
Fixed will put a user defined number of occurences, a user defined distance appart. To create a line in the X axis, set your Y occurence count to 1 The rectangle size cannot be defined by constraint since the user defines the size with the occurence count and distance.

Ken

Yeah, I was used to the flyout in 16 and didn't notice the new buttons staring me in the face. Now that trim and extend have their own buttons, too, it takes me a few seconds to find them every time.

The pattern command has both circular and rectangular patterns, each has its own button.

You can create a single line of holes by a number of ways. If you click the pattern rectangle you'll see 3 options in the command bar : fixed, fit and fill. With the 'fixed' option you just set a number for the X-direction and 1 for the Y-direction (or vice versa). With 'fit' or 'fill' just make sure that what you set for a patterning distance is smaller than the side of the rectangle in question.

The construction geometry for patterning (rectangle, circle, arc) can be governed by relations just like any other profile geometry. Attaching one keypont of your rectangular pattern to the first hole and then attaching the opposite side to the extent of your part will automatically adjust the pattern when your part changes.

Deleting the horizontal/vertical constraint and replacing it with an angular relation you can make the rectangular pattern go in other directions.

There are various options for making staggered patterns.

In assembly you can sketch a geometry-only pattern in a separate sketch and use it afterwards to patters assembly parts.

Alex