When to use Bodies at the part level

[jchance]

Looking for some helpful tips on when to use bodies and not to use bodies.  We moved to Creo 10 recently(from 7 i believe?).  Creo 7 had bodies but it wasn't something i was really interested in learning then.  Seems that Bodies have come along way in the 3 generations(and even more in 11). Looking to get feedback on how you use bodies in your daily part modeling/assembly work?

Things i've started to do now at the part level instead of the assembly level:

• Dowel Pins
  
  • I'll model the pin at the part level now and assign it as a body(can xhatch it differnetly at the drawing level).  I no longer need to have an assembly created for these.  This also makes GDT much easier at the part level instead of the assembly level
• Threaded Inserts
  • I'll either model a helicoil myself or do Get Data -> Import and import a threaded insert as a body into my model(assembly via csys).  
  • Much easier to handle the drawing this way
• I think i might do some plug welds for cross drilled holes(steam passages). 

Do all of these examples make sense?  how have you guys been incorporating Bodies into your modeling practices?

[KenFarley]

To be honest, and perhaps this is because I've been doing this stuff for decades, I really don't have any use for the bodies functionality. My major concern is that it is already bad enough dealing with poorly constructed, poorly thought out models at a part level, but adding a pile of features and bodies is just going to make things worse.

Modeling dowel pins, screws or other hardware wouldn't work for me at all. We have assemblies that need hundreds of threaded inserts, dowels, cap screws, etc. When these are called out on drawings they need to be specified with what their part number is (to order them) as well as making clear what material they are made of, etc. I am not going to trust my memory, let alone someone else's, to specify the correct McMaster catalog number for a spring or dowel or whatever. Hardware such as this is specified in "library" models that are used for thousands of assemblies.

I don't like using downloaded models such as screws, springs, etc. Many times they don't have properly defined surfaces and thus are not a manifold solid. Additionally, people will download and populate their assemblies with screws that have threads on them. They look cool, if you only have a few of them, but if you're using hundreds of them in an assembly you will suffer with massive slowdowns when handling the assembly because the software has to slog through all those models that have all those thread surfaces when doing hidden line views, etc. Springs are troublesome because when downloaded they are at a set length, which is never the length I want them to be in the assembly. I have taken the time to define mathematically determined springs that can be set to an appropriate length for the assembly. These are "library" parts, too. Took the time to make them robust, don't have to worry the next 20 or 30 times I use them in other designs.

When designing things that need to use common data to guarantee fitup, assure that changes to the design get reflected in all the components, etc. I use a top level master assembly. I define the driving sketches of the design in this assembly and use them to create the components. For those whose company has spent the money for the modules necessary, this is comparable to the skeleton model design methodology.

[jchance]

Our workflow is different for pins and the like that get pressed in.  They have always been detailed as  Furnish and Install and almost never end up in a BOM.  The Pin gets carried forward with the part and isn't ever disassembled.  Same with a threaded insert.  Its funcitonally one single part.  I wouldn't ever put a threaded insert on a BOM.  

I've also done the same with sheet gaskets that are adhered to parts.  Its not really a replaceable item.  Its always been detailed as a Furnish and Install item on the detail drawing.

[Dale_Rosema]

Just curious, how do the inserts and dowels get ordered? Kan-ban? or are the driven by a manufacturing system?

[jchance]

the shop who's doing the fabrication orders the item.  If we're doing the part in house then i'll order the part for our shop and they'll do the installation/fabrication.  

something like a dowel pin is detailed as:

Furnish and Install 4x Dowel Pin

Material: Stainless Steel Type 316

Description: ISO 2338-m6, 3mm x 6mm lg, chamfer both ends

mcmaster-carr 93600a267 or equal

Same also goes with bushings that are being pressed in(nylon or oillite).  

[Dale_Rosema]

Sounds like you have a good system that works for your company.

[BenLoosli]

I agree with Ken on most of his post. I also do not like imported models, but my designers do, and managers support their decision, more than mine. Imported models slow down the system regeneration times and are, as Ken said, not always modeled the best way for your company. We also need to have items in the BOM for manufacturing without making a 'fake' BOM because the assembly is made of multi-bodies.

My one area where I did experiment with using a multi-body part file was a U-bolt clamp that was coated with rubber. A single part number when purchased but comprising multiple parts, coated U-bolt, plate and nuts. As a multi-body part, I was able to assign steel to the base U-bolt and rubber to the coated section, thus giving a better weight calculation. In this instance I do see a benefit in multi-body parts, but like most of things in Creo you need to use the tools where appropriate and beneficial to your company.

[tbraxton]

All of my examples are a variation of a theme, creating the required geometry the fastest way possible.

Multi-body parts models are a good for creating master models of parts that get split into multiple parts. These would be injection molded or die cast models for example. Depending on what is needed, multibody can be more efficient (faster to create the geometry) than building everything from surface features. Both work but one or the other can be faster in some cases. I have also used multibody to exploit Boolean operations in part mode for the same reason, to create the required geometry in less time.

It is useful for designing weldments comprised of many parts such as laser cut and formed tubing. As has been mentioned it is appropriate for multi-material parts, such as 2-shot molded parts (rubber over rigid substrate). I have also used multibody for the design of fluid handling components where design them from the inside out. The fluid domain is modeled and then this geometry is used to create the solid body making the component (valve body, manifold, etc.).

It is also useful for creating models to be used for simulation (CAE) with multiple domains or materials.