Is it possible to keep the original orientation of a patterned feature during a Circular Pattern?

StephenG

I have a linear slot feature that I want to pattern around a hole and maintain the orientation of patterned feature.

Here is what OS allows me to do....

But what this is what I desire...

I do not see an option within Circular Pattern feature control panel to effect it.

konstantin_shiriazdanov

it's not possible with circular pattern but, you can use curve pattern by circle

konstantin_shiriazdanov

it's not possible with circular pattern but, you can use curve pattern by circle

StephenG

Yep, the Curve Pattern feature w/Keep Orientation option did the trick. 


Now if I could only suppress individual occurrences of the pattern I would be one happy clam.

Thanks!

mahir

StephenG said:

Now if I could only suppress individual occurrences of the pattern I would be one happy clam.

Thanks!

You can also use the Point Pattern featurescript. It would let you place points wherever you want. And if you want to skip an instance, just don't place a point there.

Point Pattern FS

StephenG

The "Point Pattern" Feature Script I found (Cody Armstrong's) appears to be a work-in-progress; it is only capable of patterning part entities. It should be capable of patterning feature, surface, plane, and mate connector entities.

Yes, I could have used it by...

•  Creating the slot feature as a cutting tool part volume
•  Creating a circular pattern of 8 points
•  Use "Point Pattern" selecting just the desired points (locations)
•  Use Boolean "Subtract" to create the slot features in the target part  

but this a lot more work than just "suppressing" specific instances of a patterned entity (part, feature, surface, etc) within a "Circular Pattern" feature. Instance suppression within a pattern is something I have seen/used in other CAD products.

Thanks for making me aware of this Feature Script. 

MBartlett21

You can use delete face or delete part to get rid of the instances you don't want

StephenG

Yes, using "Delete faces" is also a good suggestion to accomplish the result. I like this approach because it makes it easier to interpret/see design intent in the Feature list. I can rename the "Delete face N" feature name to "Remove unwanted pattern instances".  

(Use "Create selection" w/"Tangent Connected" to speed the face section process for the slots to be removed.)