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Creo 3, Feature Operations is missing!?

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Creo 3, Feature Operations is missing!?

I was going to show a user how to copy features between parts using the feature operations menu when I realized it's missing in Creo 3. There is nothing in the PTC update training guide about that being removed, and a search in Creo for the menu returns no hits.

 

I use feature operations, often, to copy features from one model to another. Like this:

 

Model tab, Operations, Feature Operations, Copy, FromDifVers, Done, Pick the model, Pick the features, Pick OK, Same Dims, Same, Same, Same, OK or flip-OK, Ok or flip-OK, Done. Pick the Group Copied_Group feature, and RMB Ungroup.

 

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Creo 3, Feature Operations is missing!?

David: New method is to select features to copy from source model, select Copy, activate the target window and select Paste or Paste Special depending on how you want to define the location.

6 REPLIES 6

Re: Creo 3, Feature Operations is missing!?

David: New method is to select features to copy from source model, select Copy, activate the target window and select Paste or Paste Special depending on how you want to define the location.

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Re: Creo 3, Feature Operations is missing!?

I think I perhaps understand what you are looking for. This is what I do in Creo 3 to achieve the ability to copy geometry from any component to another. With an assembly open I go to the model tree and activate a component that I want to copy something into. I then select get data, copy geometry and by default I have mine to select surfaces but within this mode I can RMB and select solid geometry if desired. You could set yours to be chains or references ect.

I hope this helps you.

Re: Creo 3, Feature Operations is missing!?

I'd use copy - paste special instead.  A dual monitor setup helps, but isn't necessary.

  1. Open the source model and select the features to be copied.
  2. Select copy or hit ctrl-C
  3. Open the target model.  (Ideally you'd have both models open on separate screens or in side by side windows on one screen.)
  4. On the model tab in the operations group, expand the Paste menu and select paste special.
  5. On the Paste Special dialog, deselect "Dependent copy and select Advanced reference configration
  6. In the Advanced Reference Configuration dialog, Creo shows all the references used to create those features.  It also highlights them in the source model when they are selected.
  7. Pick new references in the target to match those in the source.
  8. Select the check mark when done.
--
Doug Schaefer | Engineering Manager
Crow Works

Re: Creo 3, Feature Operations is missing!?

Ok after looking at the update training again I found this:

Feature Operation Enhancements
Various feature Operations commands no longer utilize the menu manager.

The following feature operations are accessed using the Operations group in the ribbon, or in the model tree:
• Copy
o All capabilities are incorporated into the Copy icon.

• Reorder
o You can still drag and drop features using the model tree.
o You can also select Reorder from the Operations group drop-down menu to access the Feature Reorder dialog box. The dialog box provides additional functionality such as including dependent features in the reorder operation.

• Insert Mode
o Drag the Insert Indicator .
o Right-click and select Insert Here.

• Read Only
o Access the read-only functions by selecting Read Only from the Operations group drop-down menu.

Two lines, that's all the time they spent on this change to the UI. This change really needs better coverage than that. 

So all those that said copy and paste special are correct.

Re: Creo 3, Feature Operations is missing!?

The actual Feature Operations menu still exists but is only accessable with a mapkey

 

Exact text to enter:

 

mapkey  >> FO #FEATURE

 

This creates a mapkey that initiates when you hit "F" then "O" this will bring up menu we know from Creo 2

Re: Creo 3, Feature Operations is missing!?

Thanks a lot for sharing this I was able to have the old menu back in Creo 4.