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Creo 5.0 Mirror Multiple Components With One Command in Assembly

Greg_H
11-Garnet

Creo 5.0 Mirror Multiple Components With One Command in Assembly

I'm using Creo 5 and can't figure out how to mirror multiple components either.  I can't believe this isn't available!?  Does no one using creo make symmetric assemblies?  Is it available in Creo 8?

 

Well, I'm off to make my 11 individual mirror features about the same plane.  

1 ACCEPTED SOLUTION

Accepted Solutions
StephenW
23-Emerald II
(To:Greg_H)

There are multiple product enhancement requests for mirroring multiple components at the same time so i'm guessing it's not available.

The one that has the most votes is archived.

https://community.ptc.com/t5/Creo-Parametric-Ideas/Creo-4-0-Mirror-Multiple-Components-With-One-Command-in-Assembly/idi-p/495669

https://community.ptc.com/t5/Creo-Parametric-Ideas/Mirror-Multiple-Parts-in-Assembly-With-One-Command/idi-p/492027

https://community.ptc.com/t5/Creo-Parametric-Ideas/Allow-multiple-components-to-be-mirrored-at-once/idi-p/469603

 

My workaround:

I will typically use an axis pattern 180 degrees around an axis that is central (almost everything I do is around a central axis) instead of mirror. I use it so much I made a mapkey to do it. You can also use an axis pattern on an existing pattern

View solution in original post

6 REPLIES 6
Trebla
15-Moonstone
(To:Greg_H)

Hi Greg_H,

 

Did you try Intelligent Mirroring?

mirall.jpg

Greg_H
11-Garnet
(To:Trebla)

I'm trying the same mirror command shown in the example.  But in the examples shown, they are still selecting a single sub-assembly.  I want to mirror multiple components and patterns that are not in a single sub-assembly.

StephenW
23-Emerald II
(To:Greg_H)

There are multiple product enhancement requests for mirroring multiple components at the same time so i'm guessing it's not available.

The one that has the most votes is archived.

https://community.ptc.com/t5/Creo-Parametric-Ideas/Creo-4-0-Mirror-Multiple-Components-With-One-Command-in-Assembly/idi-p/495669

https://community.ptc.com/t5/Creo-Parametric-Ideas/Mirror-Multiple-Parts-in-Assembly-With-One-Command/idi-p/492027

https://community.ptc.com/t5/Creo-Parametric-Ideas/Allow-multiple-components-to-be-mirrored-at-once/idi-p/469603

 

My workaround:

I will typically use an axis pattern 180 degrees around an axis that is central (almost everything I do is around a central axis) instead of mirror. I use it so much I made a mapkey to do it. You can also use an axis pattern on an existing pattern

Greg_H
11-Garnet
(To:StephenW)

While it's not the perfect solution, doing a circular "axis" pattern isn't a bad idea as a work around.  It also solves an orientation issue I was having.  It's not without it's issues though.  A couple of notes on this approach as I tried it.

 

  • You either need to group all the components 1st then do the pattern, or do the pattern once on the 1st component and then reference (automatic) patterns on the subsequent components.  User preference I guess.  Not a big deal either way & certainly better than unlinked components.
  • This approach does work on linear/direction patterns!  However, if you have reference patterns, the software won't let you pattern those.  Here's the steps I used to get around that:
  1. Create your feature driven reference patterns 1st.  If you do the axis pattern 1st, the refence pattern will default to this instead of the feature.  Maybe there's a way to select this, but I do not know it.
  2. Mirror the 1st part in any of the reference patterns.
  3. Create reference patterns again on the mirrored parts (not sure why this works, but it does).
  4. Now do the axis pattern on all of the other components you wish to "mirror". 

 What a mess!  But I guess it still beats unlink components and having to do double work when something changes.

 

StephenW
23-Emerald II
(To:Greg_H)

Every so often, the axis pattern will have orientation issues as well. Generally, they are a sign of either a missing placement constraint or a "flaky" placement constraint.

The "gotcha" with most of these placement shortcuts (patterns, mirrors) is references after the fact. Any reference to a patterned or mirrored instance is prone to failure if the pattern is changed. The moral to the story is don't be haphazard with your references. Make certain you are working in the original placement area and not an area that is a patterned instance or mirror.

WS_10193292
4-Participant
(To:Greg_H)

+1 a year later using Creo 7

 

Really PTC, you STILL do not have this feature? Solidworks has had this capability for YEARS.

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