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gnewman1-Visitor
1-Visitor
January 20, 2016
Question

Mirror Body not feature

  • January 20, 2016
  • 3 replies
  • 13527 views

Hello All,

I am trying to mirror the body I have created but Creo keeps refusing.

Is there a separate function in Creo for mirroring bodies? And where is it please?

If Creo wont mirror bodies can someone explain why this is the case? I cant think why this would be a problem, other CAD packages do it.

As a simple demo, if you create a cuboid then add a fillet to some edges. Then try to mirror the resultant solid. Creo will let you mirror the original cuboid but not with the fillets. I realise for this very simple example you can group the features but this seems a work around and doesn't work on more complex models using surfaces.

If I wanted the cuboid mirroring without the fillet edges I would order the fillets in the tree after the mirror operation.

Thanks for any input.


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3 replies

B
BryanMorris1-Visitor
1-Visitor
January 20, 2016

You can either try and group all the operations in the construction tree, then mirror the group... but can lead to some pretty slow regeneration, and modifying/addding stuff will cause you pain down the road.

or you can copy the surfaces, paste them, and then mirror the copied surfaces... faster to regenerate (most of the time).... oh and then solidify the result....

D
dgschaefer21-Topaz II
21-Topaz II
January 20, 2016

As a general rule, I would avoid mirroring features.  When a feature is mirrored (or copied with dependency), the feature references are locked.  So, if you need to redefine the sketch and re-dimension it to new references, Creo will no allow it unless you first delete the dependent feature.

Creo also does not support multiple sold bodies in part files as do SW and perhaps other packages.  Yes, you can create separate bodies, but Creo doesn't see them as two bodies.

There are two way's you can approach this.

The methods that Corey suggested are how I'd approach this.

G
gnewman1-VisitorAuthor
1-Visitor
February 2, 2016

Thanks to everyone for the input.

All these methods seem work arounds (to me) if its a simple, solid model, why do I need to start using surfaces to mirror it? I am new to Creo from other CAD packages so still trying to learn. Is Creo more stable using surfaces to model than solids generally? Previously I have always tried to avoid using surfaces where possible as thought they were less stable than solids and usually made the model more complex than it needed to be.

I always thought Mirror, pattern functions etc were encouraged in CAD? Saving operations, reducing repertition ensuring any modifications are carried out throughly etc.

Any idea why does Creo not support multiple bodies?

W
WillyC1-Visitor
1-Visitor
February 11, 2016

It sounds like you want to create a part model by modeling just half the part and creating the other half by mirroring.

Forgive me if I'm off the mark. I haven't read all the posts in this thread and I'm not quite sure what a body is.

If this is, in fact, what you are trying to do, it is accomplished quite easily. Although Creo has once again cheated common sense,

by changing/ hiding the basic functions we in the real world daily rely on, I assume with the best of intentions and more of those

imaginary productivity gains as their impetus. /snark/

Here's what you do to mirror all geometry:

  • Select the part name at the top of the Model Tree
  • Click Model > Mirror
  • The Mirror tab appears
  • Select a Mirror Plane
  • Done.

In the plastics biz we used to use this trick all the time before product developers created their own solid models.

Yes, I'm that old. lol

I've attached your part with the second half mirrored with my possibly incorrect idea and orientation.

Forgive me for not paying attention if I'm off on a tangent and wasting everyone's time.

Anyway, hope this helps

    C
    Constantin15-Moonstone
    15-Moonstone
    January 21, 2016

    Hi Gavin,
    I am not sure what you tried initially. You can mirror the entire solid by selecting to top node in the tree and then select the mirror feature. As a result in the tree you will just see the mirror feature (no sub elements). The geometrical result is a duplication of all geometry created prior to the mirror feature, including quilts and curves.
    If this fails it might be due to intersections.

    mirror_solid.jpg

    The other two options were discussed above:
    - mirror all features - not recommended

    - mirror and solidify the solid surface (copy) - highly recommended, since it will NOT mirror datums like the above mentioned.

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