How to delete a pattern and keep all of it's parts

[Ronald1]

Hello everyone,

I am currently working on a part witch is a pattern of revolves with a defined angle, to fill a complete 360° part.

The number of revolves and the angle of the revolve are variable.

Now somethimes some of the angled revolves have to be diferent from the standard division angle, and therefor

i want to delete this pattern and modify the angle for some of the revolves.

Is it possible to do this? and if Yes, How do i need to do this?

kind regards

Ronald

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[dschenken]

I think changing from a dimensional pattern to a pattern table creates a table with the same valaues the patterned items had. These values can then be individually changed.

[PatrickBrulot]

you can not delete a pattern while keeping the pattern instances. As David mentioned, you can convert it to a pattern table. If there are some feature dimensions missing in the table, you can add them afterwards using the reference tab in the pattern dashboard. There is no need to recreate the pattern, at least in Creo 2.0.

[TomU]

Look up the "unpattern" command. When the proper conditions are met a pattern can be dissolved and the individual pattern instances kept as stand-alone, independent features.

[Ronald1]

I don't think using the table pattern feature is the solution for my problem, because the part that i want to pattern is

formed from a solidifyd 306° surface copy, from witch i cut 300° of material by an other revolve feature.

So the start angle, and the revolve cut angle have to be modifyd in the pattern table.

It is the part that is patterned here, and therefor i can't select the both angles as a parameter in the pattern table.

However, i do think the unpattern command can be the solution to this problem, and i will try this in my model.

[TomD.inPDX]

I just tried the unpattern command on a patterned pattern. The sketch remains shared except for the patterning dimension. And you can still echo on and off any of the instances as normal. This could really drive someone nuts

Always good to learn something new. Thanks Tom!

[dschenken · Accepted solution]

I was looking for the proper conditions, as I want to unpattern a component pattern in an assembly and unpattern is not available.

From another group:

1) just make sure that you group the feature or component prior to patterning. It is as simple as that.

2) as I remember, you can only unpattern a pattern of feature pattern. and the feature pattern must be dimension or table type. In this condition it will be at your right click menu in WF4. Please try.

For consideration one, if the user who created the pattern had the foresight to group the component, he would not have created a pattern in the first place.

[vzak]

yes, that's the only way to do it in Creo, it should be Group Pattern to enable Unpattern (and possibly later Ungroup) commands, no other ways ... Even if you need to Group single feature - do this.

[sy07]

I just wanted to add, in the case of patterning a part feature, the sketch must be internal to the feature.