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Can we design Multi Body Part../?


Can we design Multi Body Part../?


I want to design Mouse in creo, i done outer body using surface..

Now I want to divide in multi part.. Its possible in Creo..?

If yesh then how can we do it..?

Same thing can do in SolidWorks,

its work on multi body part modeling base, so...


perhaps you are asking about skeleton technique and TOP-DOWN design. The target is share driven geometry from one "main part" to all anothers?

Try to search more information about copy geometry.

For example youtube offers some tutorials:

Top Down Design using Skeleton Assemblies - Part 4 - External Copy Geom - YouTube



Thanks for this..

but this not what i want to know..


Creo is not a "multi-body" type software like NX, Catia etc.... Although what you want to do is possible with a Top Down method and can be accomplished by a few methods. You can use a Master/Merge, Publish Geom/CopyGeom or you can use an Inheritance feature. You could do it as a Bottom Up method but it is not advisable since you have an exterior, countered surface that is shared by multiple parts.

I prefer the PubGeom method. In any case, you can create all the part break outs in one file and then "share" the information to the individual parts as one or multiple features. If you need to see a simple example, let me know.


Creo does not allow for multiple solid bodies within a single part like SW does.  You can make multiple, non-overlapping solids in a single part file, but Creo treats them as one.  If they overlap, they are merged.  Each part of your mouse should be a separate part file.  It's slightly more cumbersome, but I find it to better represent the reality of the physical product.

The top down design techniques mentioned above can be used to pull the surfaces out of the master model you've created into the individual parts.  I find the skeletons & publish geom / copy geom pairs to be the most robust and flexible, but it does require the Advanced Assembly Extenion (AAX) which you may not have.

Just wanted to confirm that what Doug and Dean are talking about is the way to go in Creo. Create a master model which is like a layout of the old days and then use those surfaces and any thing critical shared between parts using one of many techniques. I prefer using Publish Geometry out from the master and copy geometry from the master to import into the individual shapes. It can seem like extra work up front, but will totally be worth it down the road especially if you create the master thinking about association between features and geometry. Make changes in the master and regenerate the master and parts and get all the changes down steam. This can be a very robust modeling technique. Good luck.

Building on Dean, Doug, and Mark...

I will also throw in my vote for the Master Model - External Copy Geom technique.   I personally use this technique every day.  There is no way I could do what I do with the quality and proper matchup between complex piece parts without this powerful tool.

Good Luck


Bernie Gruman

Owner / Designer / Builder

PTC Strategy is: one part, one material, one mass -> just like in real / physical world.

BUT - you can simulate similar things just like in SWX with little restrictions

First thing:

- you need discipline in managing features in your model tree

then you can use closed quilts instead of solids.

- manage the features for each quilt in right order in the model tree

- use annotations features (without annotations) as marks to sort your features

- use an analyze feature with the right density for each quilt to calculate the complete mass of your multi body part

- separating the visibility with layers would be very helpful - even when you use combined states

So: If you can work with this restrictions, you can create multi body like parts - IMHO - I never used multi bodies in SWX, 'cause I can't see the benefit. The PTC strategy works fine and goes 1:1 like real world.

But you can do with your system, whatever you want.

Not seen anything for multi-body. Would be useful. However I have devised a work around by using an assemby of a part and tracing the relevent geometry into the new part and then drop the references PDQ as the next time you load up the part as stand alone all the references would not be there and the whole lot will crash. Sorry PTC but Solid Edge wins here again with the syncronous technology, multi-body modelling, automomous re-referencing, again and again, time is saved in bucket loads.


What you have described is essentially a Top Down approach, normally utilized in an Assembly with one of the procedures described above. Managing all the surfaces, merges, quilts can get a bit tedious, essentially if you are referencing offset surfaces (I.E. body gaps, reveal lines, etc... with merges) With a single change it can go pear shaped quickly.

Am I reading correctly you do this in a .PRT file? IMHO, I believe you are making more work for yourself in the long run.


Multi body is really a "what one is used to doing" type thing. I have worked on both types of software and, IMHO, one does not have an advantage "technically" over the other. Each method gives the same results, with the same amount of control as the other.

It's true - this technique makes more work with some restrictions. And I can't see the benefit inside Creo. So I prefer a clear top-down-solution with skeleton, publish and copy geom with clear downstream and replace options. But not everybody have an essentials team or advanced assembly license.

And what I'm doing with Creo is always playing. I'm not paid to build up CAD data. I use it for fun.

That's fair. I forget not everyone will have all the license capability. But, even with simple Assembly Mode you can get the results without all the extra surface work and management. Both methods work....just depends how much "Fun" one wants to have, I guess.



Thanks for your views. I too have used both types. I just get on better with the direct, nudge to surface, lock to feature that SE provides, I just find it so more fluid and much quicker to use than traditional ordered, parametric modelling where topology can mean that the thing that you want to reference from is often just not there without the extra operations of setting up a special reference plain higher up in the tree along with another sketch at the top with all the references detached, so you can lock onto things, but that can most of the time get out of date rather quickly too.

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