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Jun 30, 2023 3:13 PM UTC
Delivered

Shrinkwrap multibody generation

Related products:Creo Parametric

Please include detailed documentation such as screenshots, images or video.

1. What version of the software are you running?
Creo 10.0.0.0


2. What is the problem?
Lack of functionality

3. Are you using a workaround? If yes, please describe it.
None decent

4. What is the use case for your organization? Describe how your idea would work in context or how it would apply to a practical situation.
We would use this function to generate a fully associative multibody part from an assembly file with the aim to generate the final machined part (1 item in our BOM) derived from a welded assembly.

5. What impact does this problem currently have on your organization? (Number of users affected, hours of lost productivity, etc.)
It will help saving a lot of time spent by users in generating a shrinkwrap and obtain a better result.

14 replies

Jun 30, 2023 3:18 PM UTC

Just like this:

 

ExampleExample

Jul 3, 2023 6:51 AM UTC
Status changed to: Acknowledged

Hi @AlessandroFerri!

Thank you for your idea. Based on the information you provided, we are acknowledging it as the Community management team. This is not a commitment from the Product team. Other users may comment and vote your idea up.

Jan 9, 2024 12:00 PM UTC
Status changed to: Implementation In Progress

Hi Alessandro 

we are currently implementing such an option.

Can you elaborate a bit more in which workflows you will then use the final machined multi-body part .

E.g. can you give examples of where the biggest time savers would be for you?

thanks...Martin

Jan 9, 2024 3:21 PM UTC

Hi Martin,

before going on, let me introduce myself; I am a former PTC MCAD consultant (1997-2005) and now I am a partner of PTC itself with my own company (Ferri Engineering). We mainly use this type of methodology to obtain a machined model starting from a welded blank. This is done to avoid massive use of assembly features (which are notoriously very challenging to use and, most of all, significantly increase regeneration time when opening an assembly) .

Over the years we have developed this methodology in companies that needed to create thousands of mechanical machining on welded assemblies with a large number of components.

Certainly this situation can be solved in the future through the use of multi body techniques, even if at present we still have many problems in coherently managing the BOM of this type of objects. For example, the same rib (body) used several times in a multi body part is not correctly documented in the repeat regions because you can't have different bodies with the same name.

To solve this, you should use a body parameter instead of the body name in the repeat regions (but this would be a good solution if it were possible in the part template to specify a set of standard parameters for the newly created bodies (which is not yet possible today but it would certainly be interesting to implement to automate this process).

Another possible use of a multibody shrinkwrap could be to create a plant layout (via Envelope Simp Rep or as simple assembled parts). 

This technique enormously reduces the number of components that Windchill must add to a workspace with obvious benefits in terms of system performance.

Last but not least, the regeneration time of a drawing view of a solid shrinkwrap is several times lower than that of the same object but created via Surface Subset.

From a theoretical point of view, it should still be easier for Creo to generate a multi-body shrinkwrap rather than a single-body shrinkwrap, simply because it does not have to resolve geometric incompatibility problems resulting from having to merge geometries from distinct solids into a single solid (such as that which occurs when joining the balls of a bearing with their seat).

I hope I made myself clear, but feel free to contact me if you have any questions or if you need clarifications.

I take this opportunity to wish you an excellent 2024

 

Alessandro

 

 

Jan 29, 2024 7:54 PM UTC

I also find this very useful.

Regarding the question of using multibodies to design welded parts and the question of having a rib body (which would have the same dimensions) not recognized as the same body in a different location it has to do with the way PTC choose to implement the multibodies. All copied bodies, or patterned bodies do not work as components inside an assembly, PTC opted duplicate in-place the copied or patterned bodies and put the geometry all in the same "set" of dumb solids. This simplifies the implementation, but also restricts the usefulness of the multibodies and for which workflows they can be used.  The problem of not recognizing the same body assembled at different Coordsys locations results in each body will not be reflected correcly in a BOM.

 

When mutlbodies where first shown in Creo 7 I asked @mneumueller why not give the option of creating "instanced" bodies (Same geometry associated with a different Coordsys instead of the Default CSYS) (same principle as a Component patterened in an assembly, pointing to the same part (The geometry "Body") but assembled at different locations.) This would accelerate both regeneration times, when patterning or duplicating a high number of bodies and allow creation of correct BOMs inside a part, when we use a Multibody part to derive different components for an assembly, ie, when creating a "Skeleton Part" as a simplified assembly to create initial geometry to derive a diferent part from each body.

 

This would facilitate the automatic and parametrically associated creation of a whole assembly (or sub-assemblies) from a multibody skeleton part).

Currently this is tedious. We only have an option to righ select a Body inside a part, and select "Create Part from Body". Which we have to repeat for each body. And afterwards, we have to manually create an assembly, and tediously assemble all the created parts that we dereived from the initial multibody skeleton part, assembling one by one, and always have to click the default assembly constraint. We cannot batch select several parts on a folder and assemble all of them at the same time. And all the parts we create this way, cannot be "duplicated", and all the "duplications" of a source part will have to be reassembled using some kind of constraints or a new pattern has to be created in assembly mode that is not associated with the patterned bodies in the skeleton multibody part.

 

If the bodies could be "instanced" in any multibody part (or at least PTC could implement this in skeleton models for users with the advanced assembly license), then user could automate the creation of derived assemblies and derived parts from a multibody part, where each copied or patterened body would in the associated derived assembly, simply assemble the same part derived from the first body, and use the source pattern to pattern the derived components in the assembly at different coordys locations.

 

This alternative multibody implementation seems like it would be the same as implementing the same functionality as the assembly funcionality but inside a PRT file instead of an ASM file. Almost, but not quite. The idea would be to avoid all the problems that exist in assembly mode that lead to Circular References nightmares. The problem in assembly mode is that a component can reference components outside in the context of the assembly. This would not be allowed in this alternative multibody implementation, since the idea is to allow a single regeneration pass, where each body can only reference geometry that exists above in the regeneration tree. To further clarify, any feature added to any instanced body would be added to all the instances, the user could not add any geometry that would be specific to one of the patterned bodies, unless a feature is added to allow the user to Specify that a duplicated or instanced body would become "unique", the effect of which, would be to simply "explode" or "collapse" the original body geometry "in place" at the current body patterened instance location, which would or could convert the body geometry to the "default" coordsys location. This way, any body that is "Unique" would be assembled automatically by default, and any instanced or patterened body would be assembled at the correct location in the automated assembly creation process. This automated and parametric assembly creation process would be a feature at the bottom of a Skeleton mutlibody PRT file,similar to a "Publish" feature for intent purposes, and problably could also be used as a feature to create what @AlessandroFerri is requesting in terms of "body" solid shrinkwrap. The difference is that @AlessandroFerri is asking for the feature "Shrinkwrap" to be added to a user selected target part, and what I propose, is the ability to add the feature of body geometry transfer to be added to the source part, much like a "Publish" feature allows better design intent than an ad-hoc "External copy geometry". This would let the solid body export selection to be specified once at the source, instead of possibly in several assemblies that could have to be redefined if any source body was deleted, or a pattern count of a body changed. This would avoid errors and manual user intervention when making changes to a design, and would allow the senior designer of the original multibody skeleton part to control which bodies would be used for the creation of any sub-assembly, or several sub-assemblies.

 

In my implementation request, I am in doubt if it would be better to create a single "Export Geometry" or "Publish Bodies", inside of which the user could specify a list of one or more sub-assemblies and which bodies to include in each sub-assembly, or if it would be better for this export feature to allow the creation of a single sub-assembly, and if the user needed to export bodies to more than one sub-assembly, it would create several export features, one for each sub-assembly.

 

And I think that the feature on the receiving parts to get the bodies from the source part would better have a different name than "Shrinkwrap", since the name of the feature makes little sense, since most associate the Shrinkwrap to a collecting of simplified geometry process around the "silhouette" of a source part, ie, modified geometry, and a process whicht migh be slow and involves lots of calculations. Since we are talking about simply collecting or transferring original solid geometry bodies, with no simplification involved, I think it's better to put this funcionality in a different command, and not inside a "shrinkwrap" feature. With a name that more correctly identifies the behaviout and intent of the feature. Like "Import Bodies" (might not be the best, since the import process might be associated with STEPs or IGEs) or "Collect Bodies", or even "Copy Bodies".

Jan 29, 2024 8:17 PM UTC

Solid Edge in a recent version has implemented almost the same funcionality that I mentioned. It allows now to Create Assemblies with all the features inside an assembly instead of the tradicional method of the geometry and the feature tree to be located on the parts. This way all the geometry is created in assembly mode, a single Assembly feature tree, but the geometry is "deposited" or put inside "part containers" like in a tradicional approach. This way Solid Edge avoids the same problem of creating complex assemblies with circular references, since there are not features inside the parts, only geometry, and all the features are put sequentially in a single place, inside the assembly, so, there is no way to generate circular references, since it's impossible to reference geometry from parts that were not created yet in the model tree history. This process is not usefull for complex assemblies, or parts that need to be reused in other contexts, but is very usefull for assemblies with many interdependent relations between parts, to specify size, or interface locations, for "start" geometry, or skeleton models, to create the inital parts to be then further refined in the derived parts where then different users can then further complete the parts, like adding rounds, chamfers, etc. This same process that Solid Edge implemented allows a very efficient implementation of welded parts per @AlessandroFerri initial request. So, since we are Creo users, and want to remain so, I think PTC should try to improve the multibody funcionality to recreate something similar. Solid Edge added the geometry creation with almost all the features that exist in Part mode to be available in assembly mode to create interrelated parts complex assemblies avoinding circular references. I think to achieve the same for Creo, is to add assembly funcionality in part mode, instead of adding the creation of almost all the features that exist in assembly mode to be available in assembly mode. From a programmer and user point of view, I think the best approach is to be able to create "instanced" bodies (same geometry in new location) to the multibody funcionality. This way if the user patterns a body named "Rib" per @AlessandroFerri  example, instead of Rib, Rib_1, Rib_2, Rib_3, Rib_4, etc... (if we currently Use pattern Geomtry of a body) Creo would create a pattern of a single Rib internally "assembled" at different Coordsys. This internal Coordsys Could be extracted and patterned in the automatically created assembly. So, in the derived assembly the user would be presented with a single "Body" / Rib part to create a drawing for, and the BOM would be correct. (If we currently use the pattern command for an extrude to pattern the extrude feature, we get a single body with several extrudes, so this does not work to create separate bodies, that's why in this case we would need to pattern the geometry instead of the feature.)

Jan 29, 2024 8:34 PM UTC

Another useful benefit of adding instanced multibodies inside a part to the Creo toolset, is that it would allow better creation of "flexible" parts like springs, hoses, wires, etc, that would be animatable in real-time. For a spring, the user could create two "fixed" solid geometries associated with a default coordsys for one end of the spring, and another "floating" or "external dependent" csys at the other end of the spring. Then, between both CSYS geometry could be added that could be realtime bent, stretched, twisted, etc. (features that already exist in Wrap mode), For realtime animation purposes, this "middle" part between a static (default Csys) body and another floating body, this triangle tesselatted could be animated with an OpenGL geometry program inside the graphics card.

Jan 31, 2024 1:55 PM UTC

for Creo 11.0 we are working on providing multibody support for Shrinkwrap.

You might want to try this out during the upcoming beta test end of February.

We would be interested in understanding whether this (fully / partially)  addresses your needs.

https://www.ptc.com/en/products/creo/beta/

 

Thanks..Martin

Feb 9, 2024 11:18 AM UTC

Hi,

I've just downloaded and installed Creo 11.0.0.0 Sneak Peek.

I tried the new Shrinkwrap and I can say that it works as I expected. I hope that all the users community will exploit this new functionality. Well done. 

 

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Apr 18, 2024 1:43 PM UTC
Status changed to: Delivered

delivered in Creo 11, see Multibody Support in Shrinkwrap Feature