Can you have multiple parts within single model file?

[pimm]

With the CAD software we are phasing out you can have numerous independant geometry part models within a part model file.

This allows the assembly of several components without adding the clutter of extra part models.

I haven't run into this yet in Creo; is this possible?

If this isn't possible this will triple the amount of part files that we are accustomed to. It will force a different way of keeping necessary files from being deleted.

If it is possible could someone give me a little primer on how to achieve this?

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[Dale_Rosema]

Paul Imm wrote:

we .... have numerous independant geometry part models within a part model file.

Just wanted to verify that you are not talking tabulated drawings or part that are within a family, but completely independent geomertries.

If they are not totally independant I could see the use of family tables, but not for completely independent parts.

[pimm]

As far as I know there is no limit to the number of objects that we can have within a part model (within the CAD software I've mentioned). They can be drawings or part models. We could do an entire job with it's many components and drawings within a single part model.

We prefer to handle this componentized as having an entire job within a part model would not only be cluttered but also take a while to open the model file.

We will try to duplicate our component style of building our dies, but what might take 5 part files with our current system might appear to require 15 part files with Creo. It will be harder to keep track of components, and get things more jumbled up within each job folder. We prefer building things componentized to keep the die history neat and not rambling on and hard to catch the creation order.

If this is possible within Creo I'd like to discover how it is accomplished before the clutter starts to build.

[dgschaefer]

Creo tends to take a more literal interpretation of the physical world into the electronic. That means it treats a part as a part, it represents only one part. You can have multiple sold bodies in a part file, if those bodies do not overlap, but Creo will still treat it as a single part.

Drawings and assemblies are separate objects with separate files.

Basically, Creo expects a 1:1 ratio between physical and electronic objects (parts, drawings, assemblies). I expect that you'll have to change your practices with Creo. A system that parallels your tracking of the physical components may work well.

[James62]

There is nothing like adding a part into a part which then shows up as a parametric feature in the model tree. Or anything like splitting a part into a parametric multibody part.

I think you could use merge feature to merge parts, but the volumes need to be touching each other, and you would actually need an assembly for that to work.

It's also possible to import other parts into a part, but that is not a parametric approach.

Splitting of a part involves copying portions of a part into another part, and that also requires an assembly, as long as you haven't got AAX.

If you want multiple models to be driven by only one model then try using a skeleton within a subassemblies.

[ptc-4606033]

I am having the same issue I need to export a multi body part file for a CFD analysis.

in SW you have the option to merge features or not merge while they are still in contact. Can Creo do this or not?

[TomD.inPDX]

No it cannot. Would be a great option in Creo 3.0 though (PTC: hint!)

All too often I want to do a composite in a part file.

Welcome to the forum, Andrew.

[ptc-4606033]

Antonius, Thank you very Much for the Reply.

[ptc-5974501]

Agree with your wish. A plastic coextrusion is also something I'd really like to do within a single part file.

[Patriot_1776]

Well, to me it doesn't really make sense, that's what assemblies are for. You could try inserting inheritance models into a part, or maybe do it as a family table. But, if you want to cross-section it in a dwg, you'll need it to be different parts to get different x-hatching.

[TomD.inPDX]

Frank, the idea of having a pseudo assembly that reports as a single level and has transparent associativity has significant productivity implications for many sectors.

But you're right, of course... this is a huge divergence of how Pro|E "thinks".

On simple terms, think of a circuit board with traces. Or a panel with silkscreen. They are dissimilar materials in an "inseparable assembly". I would love to make PEMs a separate body in my sheetmetal part models. I would love to have a modeled solid weld yet preserve the weld prep features of the base sheetmetal or tubing part. Actually, I would love to make a bicycle frame with separate tubes rather than everything joining.

[ptc-4606033]

Hey Frank,

for CFD models that have to be as simple as possible to keep Run times down I can create Multibody parts much faster and export them quicker than going through and creating every part, assemble and then export.

in Some CFD packages you can tie them to several Solidworks configurations that are made from the family table of the multi body part and run batches of analysis without having to make more assembly files.

[Patriot_1776]

Interesting. I guess I've never had a need for that. Isn't there a composites module? Could you trick it by using family tables?

[TomU]

There are certain situations where this would be very helpful. I know Catia has the ability to create multiple solid bodies inside the same part. This is really nice when you have something that really is an assembly, but you don't want to manage it as such. It's much easier to purchase, track, and duplicate a single part (both in a PDM system and outside of it), and this can make sense if it's really treated that way in real life. If it will be a single line on the BOM, and have one drawing, and is not intended to be disassembled and altered, the single model makes much more sense. Some examples:

• Demountable Pins and Bushings with toe clamps (and possibly fasteners)
• Purchased components that move - hydraulic cylinders, gas springs, etc.
• Purchased assemblies (Standard Lifters, conveyors, valves, manifolds, fittings, etc.

Unfortunately, from what I understand this is fundamentally not possible with the Creo's (Granite) kernel. Creo treats all solid geometry in each part as one set of solid geometry. It will warn you if there are separated pieces of solid geometry contained in the same part. If you do create separate pieces of geometry, as soon as they touch they instantly "merge".

I have two basic "solutions".

1. Create an assembly. Of course you will end up with dozens to hundreds of individual parts for each assembly that now need to be tracked in the PDM system, excluded from BOM's, etc.
2. Create a single part. To make this work you need to make sure that there is a small gap between separate pieces of solid geometry (ignore the warnings), and physically change the sizes of things to simulate movement. You also may need to keep the model accuracy high enough to prevent things from automatically re-combining.

We actually have automation built that will take assemblies (typically downloaded from the Internet) and merge each individual component into one new, single part. That part is then exported and re-imported creating a single file to represent that assembly.

[rohit_rajan]

does Insert/Shared Data/Merge/Inheritance...serve the purpose?

[TomD.inPDX]

Merge-inheritance is still a separate part. And you still have the section problems.

PTC could handle this with some level of intelligence in Windchill. I've seen it done in Teamcenter and I think even co-create has this in their model manager. For the rest of us, we just have to suffer along. Unless you got clever with all your repeat region BOMs to look for a flag, or file name format compliance.

For instance...

12345.asm consists of

12345-1.prt

12345-2.prt

12345-3.prt

but only 12345 conforms to part number rules. the sub-components would not populate the repeat region in either single level or multi-level BOMs.

But then you have the formable parts to deal with... such as o-rings.

O-ring 54321.prt is a generic oring. but 54321-22334 is the same oring in assembly 22334. The BOM again picks up a blanked/hidden part 54321 but has 54321-22334 in place for drawing purposes.

Once a part is in "history" or "the database", I don't like messing with them. Since 54321-22334 is new as is 22334, you have access to these without disturbing anything that might be used elsewhere.

There are so many thing to consider. I've worked with a lot of systems. I really like the freedom no PDM give me.