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Mirror Part

Newbie

Mirror Part

Hi,

is there any way to choose the mirror plane when I want to save a mirrored part?

I use Creo 3 M60.

If not - PTC just do it!

Many thx,

Michael

11 REPLIES 11

Re: Mirror Part

Nope.

--
Doug Schaefer | Engineering Manager
Crow Works

Re: Mirror Part

Yes there is! IF you create the mirrored part inside an assembly.

  1. In the "Component" area of the "Model" tab ... you pick "create"
  2. the Create window opens, you choose "Part" with the radio selected for "Mirror" (Give it a Name & Common name)
  3. Next window, select your mirror type... Dependency control ... the Part you are mirroring ... and most important - the Plane to mirror from
  4. Preview it with the check box option at the bottom left... then hit "okay" when you're done

I haven't yet checked the dependencies in Windchill. But this is the only way to select the mirror plane I know.

UPDATE: It worked perfectly in Windchill - as long as the mirroring plane you chose was in the part itself, there was no assembly dependency.

Highlighted

Re: Mirror Part

In my previous experience it would only mirror across that plane within that assembly for that one component.  Once you took that same component out and to another assembly or assemble it again at Default it would act as if it was mirrored across the front datum plane.

What you can do to remedy this is to:

  1. Create a new part
  2. Copy Geometry from original side
  3. Mirror Copy Geometry quilt
  4. Solidify mirrored quilt across the datum of your choosing
  5. Hide Copy Geometry

Now you have a dependent mirrored version across the plane of your choosing

Re: Mirror Part

I know I have a desire to be able to do this, but I always remember that no part file has a specific orientation by itself, and assemblies orient the parts.

Is there a specific reason this is needed?

Of course; knowing you are going to do this, you can plan ahead and build your model with the default mirror plane in mind.

Doug's answer is correct

Re: Mirror Part

Did you try my solution? Because I've used it now twice completely successfully in Creo 2.0 with Windchill 10.2.

Re: Mirror Part

This also worked by making a temp assembly, default orienting the part... making the mirror using the datum from the original part (NOT one from the assembly). Saving the Part, deleting the assembly when you're done.

This is probably one of the few times Creo does not create some secret reference to the assembly a part is made in.

Re: Mirror Part

Daniel,

This is how it had to be done prior to Wildfire 3.0 when File->Mirror Part was introduced.

However you will find upon further investigation using your method it will mirror about the Front Plane regardless of what plane you chose.

Re: Mirror Part

Corey Susie wrote:

Daniel,

This is how it had to be done prior to Wildfire 3.0 when File->Mirror Part was introduced.

However you will find upon further investigation using your method it will mirror about the Front Plane regardless of what plane you chose.

I've used Daniel's method before to control my mirror plane, however I just tested it in Creo 2 M190 and WF5 M200 and it doesn't work.  I'm not sure if that's a change in functionality or if I'm not remembering how it worked correctly.  It does mirror about the front plane regardless of what plane you choose.

This certainly feels like a bug, but I'm not sure that PTC would agree.

--
Doug Schaefer | Engineering Manager
Crow Works

Re: Mirror Part

It has worked that way in the datecodes of WF2, WF3, and Creo 2.0 I have used. 

In TDD assemblies I create, this is always an issue for me.  However as long as you have Advanced Assembly Extension you can use the work around I utilize with Copy Geom.