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Mirror Solids with sketches

Mirror Solids with sketches

Mirror Solids with sketches

In Catia 5
How does one mirror a solid , along with it's associated skethes and sketch planes etc.?

You can do it in Catia 4...........easy.


RE: Mirror Solids with sketches

Because V5 uses a hierarchial database (it doesn't store the final geometry - just the steps to create it), you can't mirror everything.

I've been trying to figure out an easy way to mirror similar, but not exactly opposite parts, and the best I've come up with is to model the second part from scratch.

RE: Mirror Solids with sketches

Ditto. You can go into each sketch, one at a time, and mirror the elements in the sketch. This will work pretty well on a simple solid, but it gets tougher with larger ones.  Turning Auto-Update OFF can help while you are still in-process.

RE: Mirror Solids with sketches

This was my conclusion

I have had to mirror everything with Surface Design.
Create new Sketches from the wireframes produced.
Then Re-Create the solid tree.

My client isn't a happy bunny.

Catia 4 ---30 seconds work.
Catia 5 ---2 DAYS.!

RE: Mirror Solids with sketches

While this (and a few other things) may be tougher in V5 than they were in V4, there are so many other ways that V5 shines over V4.  I can show you where we have saved 6 weeks over V4 on specific design tasks.  

It's easy to say "I can't do this in V5 like I can in V4".  The real challenge, and the real way to get the job done, is to ask "What is the end job that I need done", and find out how to do it.  You will usually find that you can do it a different way in V5 than you did in V4, and you can save much time doing it that way.  

In your case, Do you really need the support geometry mirrored?  Or do you just need the final solid?  Can you find a way to make the appropriate changes on the "original" part so that the final, mirrored part looks correct?  Can you simply start with the original part mirrored and make some pads, pockets, holes, etc. to come up with the final part?  Is there some common, fundamental geometry that could be put into a 3rd CATPart document, and then use that to create your left and right hand parts?  

Much of the key to the power of V5 is not in simply creating the geometry.  Building solids is pretty much the same in all CAD modellers.  Some have these tools, some have those tools, but it all boils down to the same.  The real key to the power of V5 is in it's ability to modify and re-use the design intent of your original designs, so that follow-on designs can be created faster.

I'll get off of my soapbox now.

RE: Mirror Solids with sketches

I agree with you on all points, I , personally am a big fan of V5.
However, I have to work to the ability of the lowest common denominator in my client's office. The 15 years on V4 dinosaur who doesn't want the bother of new 'gadgets'.

I can produce wonderous time saving trees and links and power copies.

Would the dinosuaur understand it, ? No.
That would be my fault then.

RE: Mirror Solids with sketches

Back to the mirroring question. We design Tail lamp for trucks and we have to mirror 99% of the parts from right hand to left hand. The parts that don't mirror are the holes that the bulbs fit into. We design using one side of the vehicle and when we are ready to prototype the parts we mirror (CATIA V4) the opposite side and added the appropriate locking socket hole. If CATIA V5 can't mirror -CATIA V5 has introduced a problem. Do we model up to a level and stop - copy the file to Left hand and finishe design? Does any one have some advise. thanks texaspete

RE: Mirror Solids with sketches


I've never done tail lamps, but I think you have a good solution: model common geometry, and then mirror and add unique features. I'd put the common geometry in one CATpart, and then link it into the right and left parts with one being symmetry'd.

But, this assumes you can easily store the data in your database (do you use PLM?), and it doesn't cause problems with downstream applications, like analysis and tooling.


RE: Mirror Solids with sketches

Jack's method is exactly what I would recommend as well.  This way, if you need to make changes that effect both parts, you can make htose changes to the common part.  if the changes effect only one or the other, you can change it in one of the child parts.

PLM can help you manage these types of links, however they will work in the file system as well.  You may have to create some parts that don't belong in the BOM, but that shouldn't stop you - there are plenty of parts we end up creating in V5 that don't beong in the BOM but are necessary to get CATIA to work most efficiently (just as there are plenty of parts in the BOM that we don't model in CATIA).

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