"geometrical sets" vs "Ordered geometrical sets" vs "Bo 1

[abeschneider]

since I am new to Catia, I'm struggling with the concept of geometrical sets, ordered geometrical sets, body, and body in set...

I'm trying to make a control structure which will have a variety of sketches and datums which will ultimately control a complex product. I had been creating all my sketches and other features in the default "PartBody", but I'm running into difficulties in reordering components in the spec tree - for instance even though an object was dependent only on a plane high up in the tree, if I tried to reorder it before the rest of the objects in the tree, I'd get errors.

Anyway, is there a recommended way to organize geometry; should I create a "geometrical set", an "ordered geometrical set", or what?

Thanks a lot, I'm new to this and I appreciate your help! I'm on V5R15, Windows XP SP1, nvidia QuadroFX 2000. I'm transitioning to Catia from UGS NX3.

 

[catiajim]

I would definitely recommend that you turn Hybrid Design OFF and do not use Ordered Geometric Sets until you get the hang of V5. These features may be very powerful, but they can really confuse the heck out of a novice user. You can disable Hybrid Design thru TOOLS --> OPTIONS --> INFRASTRUCTURE --> PART INFRASTRUCTURE --> Part Document.

Unfortunately, once you have started down the road with an Ordered Geometric Set or Hybrid Design, you cannot go back - you need to start over.

With these options turned OFF, you will find that your wireframe elements will be in the Geometric Set, and your Solid elements will be in the Part Body. Sketches can exist in either location, or in some cases even in both (when you create your sketch in the Geometric Set, and then use it to create a solid feature). Re-ordering the Geometric Set will not cause your parts to fail then. Re-ordering your solid will usually cause problems.

FYI, think of an Ordered Geometric set as Wireframe that behaves exactly like a Solid. Each Feature on the tree exists in a specific order on the tree. Features can reach above them to reference other geometry, but they cannot reach below them. Thus, when you re-order the tree, a feature may not be able to locate the support geometry any more. Think of a Hybrid Body as the combination of a PartBody and an Ordered Geometric Set. It can contain both Solid features and Wireframe Features. Position in the tree is extremely important.

 

[jackk]

Normally I would agree with Jim. And I do agree with Jim if you've been using CATIA for a long time.

But since you're new to CATIA (and your company is also new to CATIA?), I would suggest you Do use Hybrid Design and organize all your geomety into part bodies (and don't use Geometric Sets or Ordered Geometric Sets). I think this would be much easier. Once you get more familiar with CATIA and having parent geometry higher in the tree than it's children geometry; then you can start organizing your geometry into Ordered Geometric Sets that are under the Part Body.

But beware: most other users and companies use CATIA the way Jim described (they don't use Hybrid Design), so my method could cause problems if you exchange data with other companies.

 

[UGperson]

abeschneider,

I am also a former UG designer, and I do understand the pains that are ahead of you. If your company will let you use Hybrid Design Do it. This will make Catia act more like UG by will place the sketches and plains in the tree at the time of creation like UG dose. Which will allow you to reorder features like UG.

Just remember that this is not UG its CATIA (Cuss And Try It Again)!!! I tend to do this a lot...

 

[catiajim]

You can re-order your features in a Ordered Geometrical Set or in a Hybrid Body, but you need to be very careful about precidence. Each element needs to make sure that it's parents are above it in the tree, and it's children are below it. Otherwise, things will blow sky high.

 

[abeschneider]

ok, I want to thank you for your comments; though I admit it's still a bit confusing, trying to figure out the best way to proceed.

Lets say I am modelling a machine with several subcomponents. (Like a top-down assembly structure). There is a common set of datums and possibly sketch geometry, referred to by the various subcomponents. Would a decent way to proceed be (assuming Hybrid Modeling) to place the common datums in the default PartBody, and then create individual Body's for each significant subcomponent's master geometry. Then, "publish" the relevant geometry, which is then referenced by new Parts, which are then re-assembled into the final machine.

would the creation of many Body's be redundant? If not, would you put them at the same level as PartBody, or at a level within PartBody?

Thanks for your advice again; my apologies for dumb questions.

 

[jackk]

Abe...

That's a pretty advanced question for someone who is new to CATIA!

Yes, your approach is good. Use common 'master geometry' that you've published and then use it in the detail parts with links back to the publications. The linked geometry will automatically go into a geometric set called REFERENCE GEOMETRY.

The number of Part Bodies and/or Geometric Sets depends on how complex your parts are and whatever will make it easier for everyone to understand your part definition.

I've been told that UG has similar capabilities - is it called "skeletons" ?

...Jack

 

[jackk]

I suggest your company contact your CATIA dealer (or look for a consultant) to help lead you through the confusion and eliminate the pain of trial-and-error.

 

[abeschneider]

jackk - in UGS NX3, this method (or at least a similar one) is called WAVE linking; it basically allows instantaneous associative linking of objects and parameters; it's very useful when designing complex machinery, and especially useful when the parameters of the machine aren't yet final, because the associativity allows for flexible updating of the entire machine without manually re-dimensioning all the subcomponents.

So, I'm trying to figure out how to do the same type of thing with Catia...

is there a major difference between creating additional Body's within the PartBody, vs creating these new Body's at the same level as PartBody?

 

[catiajim]

Your method should work well, however I STRONGLY recommend that you DO NOT put everything in one CATPart. You need to work this methodology using an Assembly (CATProduct). You would have a Master Control CATPart (Skeleton), that would contain your master geometry. This Master Geometry would be Published (Tools --> Publication). Then create each component in it's own Part. Link the sketches back to the Master Control Part (Tools --> Options --> Infrastructure --> Part Infrastructure --> General --> Keep link with selected object).

 

[abeschneider]

catiajim - I think I understand some of the reasons why you suggest using CATParts assembled into a CATProduct for this method. I have a couple questions as a result, though:

1. I have a CATPart composed only of reference planes and parameters, which is the 1st part in my overall CATProduct. I publish the planes and params so the other CATParts can reference them. The other CATParts are created independent of the overall assembly, and are in turn assembled into their own sub CATProducts. However, when I change a parameter in the reference CATPart, the change doesn't automatically propagate through all the linked parts. I have to manually update all the linked components. Is there a way to "Update All"?

2. Lets say I created a part along the methods above. One of the things I want to do with this part is to use it to subtract out of another part, but rather than creating the solid in 2 different locations, I want to add the 1 part into an assembly with the target part, and then do a Boolean subtract. When I try to assemble the part into the other CATProduct, CATIA complains "Contextual part not inserted in its context ...". It lets me add, and then I can do a Boolean, which automatically places a new Body in the target CATPart. Is there anything wrong with this? Why the error message?

Apologies for the long-winded questions. It seems like the official help docs are a little short on the details of advanced assembly modeling...

 

[abeschneider]

Apparently now "Update All" in the assembly context is working - it propagates all the changes down thru the levels.

I still wonder about my question #2... restated, it is: If I create a part with contextual links (ie: references to Published components in an assembly) and then want to assembly it into a different assembly, is there anything wrong with the approach? Is CATIA's warning about "contextual part not inserted in its context..." just a reminder, or should I not be doing this?

(It just seems like this is a handy way to 1. create geometry in context of system-level contraints, and then 2. assembly the geometry as needed, which may imply different physical positioning than was present in the Published context.)

Thanks.

 

[catiajim]

Yes, it's just a reminder. What it is telling you is that the part cannot be edited in this context.

 

[abeschneider]

great. thanks a lot catiajim and jackk

 

[jackk]

Your welcome Abe!

Just one little clarification about contextual parts: You can edit the geometry of any part, contextual or non-contextual. The restriction is with links - you can only edit/replace/create links (external references) with contextual parts while they are in their contextual assembly.