Adding features to existing patterns.

[MikeMortimer]

Hi All,

Does anyone have any idea how to add features to an exising pattern, (in this case, a pattern by dimension)?

Obviously, deleting the pattern, grouping relevant features and repatterning is an obvious way to get the job done in most cases.

But what if I have a connector, and I have a couple levels deep family table which uses the number of pattern instances as a variable? If I delete the pattern then it deletes the column (for pattern instances) in the family table for good, forcing me to fix the family table (possible a lengthy one) and possibly destroying all family table instances below that which relied upon the original patterned feature.

So, in order to keep everything in tact, I'd want to add the additional feature to the original pattern, leaving the family table unaffected.

I've attached an image which crudely represents what I'm trying to do.

Can this be done?

Cheers in advance!

Mike.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[JonathanHodgson]

Without knowing in detail what you're trying to do, I can't be sure this will help, but I'm a big fan of reference patterns.

If you can add a new feature / component outside the existing pattern, but defined in such a way that all its 'moving' references are taken from the original pattern leader, then you can simply pattern it using the Reference pattern type and it will follow the original pattern.

Very, very useful for putting nuts, bolts and washers on circles of holes, as well as when modelling features within a part. You can unpattern, add or delete downstream features without affecting the original pattern.

In general, Pro/E will automatically select Reference if it's available for the entity you're patterning.

[TomD.inPDX]

I agree with Jonathan on this one. Patterning multiple features in one go is a Creo/WF/ProE weakness. I think the reference pattern was the way around this and it stuck.

In testing, I patterned the CS and then tied the extrude sketch to the CS with a dimension. Then I patterned the extrude and it gave me the "reference" option.