Add functionality: Multi Body part

[mwa]

Add Multi Body part functionality within part-mode, so within one part several sub-parts can we indentified for example a weld-part consisting several tubes in 1 part. Due to the Multi model part the assembly is not needed and external references are avoided. Also  copying of bodys within a part is more easy when using Multi bodies. Multi body parts are also very helpfull for creating shell meshes when doing analyses with FEM- software like Ansys Workbench

[applieddesign]

Agreed! This is the #1 functional advantage SW has over Creo.

[BenLoosli]

Don't hold your breath for this change. It goes down to the core of the PTC design principle and the coding of Granite One.

SolidWorks was initially using Parasolid as their core modeling kernel and it has always allowed multiple bodies in a file. When they switched to the CATIA kernel, it too must have allowed multiple bodies in a file. Not sure if CATIA does, but since the kernel does, I would guess it does, too.

PTC's design philosophy has always been individual files for all components and then bring them together in an assembly.

[dgschaefer]

As Ben said, Creo (Proe at the time) was built around the idea that the database should reflect reality.  So, there are no multi body parts in the real world (that would be multiple parts), so not in Creo.  You may remove material at the assembly level (drilling holes at assy, etc.) but you don't add material (welds being an exception), so no assembly protrusions, only assy cuts.

So, I agree doubt that PTC will be adding this, even though it would be handy in many scenarios aside from simulating actual parts.

BTW - Ben, where did you read that SW switched kernels?  It's been rumored for some time, but I can't find any documentation that it's actually happened.

[TomU]

Work is under way.  There was a public call for working group members some time back.  Here is a screenshot from the list of active working groups:

[BenLoosli]

Doug - I did more research into the SW kernel. Dassault has said they want all of their products on the V6 kernel, however that is for new products only, like SolidWorks Experience. The original SolidWorks will stay, for now, on Parasolid. Dassault owns their own V6 kernel of CATIA and the ASICS kernel they bought plus they license the Parasolid kernel from Siemans(UG).

[KQD]

I am a new subscriber to Creo+ISDX. We have a couple of licenses of SolidWorks here, alongside Rhino and Fusion 360. I have used SolidWorks for 20 years. Back in the day, I was one of the early promoters of multi bodies in parts for SolidWorks, as this is the way we modelled in systems like Ashlar Vellum Cobalt and Think Design. CATIA, NX, SolidEdge, Inventor, SolidWorks all handle multi body parts.

When we looked at Creo, our focus was on Freestyle and ISDX. This was the main reason for us to expand our software base. We had very specific issues to deal with in the workflow using SubD methods - we use Power Surfacing in SolidWorks and Tsplines with Rhino and Fusion 360. Freestyle is an excellent product, but it needs the multi body approach to really work effectively.

So why multi body parts? In my (20 year) experience modelling in this way I can put it down to a few things:

1. Top Down master model approach - we can model in context in a part then save out bodies as parts - associatively. Update the part model, the saved out parts update, and any assemblies that use them as well. This approach is particularly important with assemblies that are made up of fixed parts - like enclosures, plastic toys, etc. You can model top down in assemblies in SolidWorks as well but for these "simple" static assemblies (often made up of complex bodies) multi body parts make things much simpler.

2. Modelling specific features - such as complex patterns than change relationship to a surface. As an example, think of a dimple feature on a double curvature surface - very common. In designing these featues I want to vary the depth or height of the dimple relative to the surface. I SolidWorks I would create a dimple body and position it above the surface or tie it to a control surface used to vary the feature depth. I then pattern the body across the surface. I then boolean cut the bodies from the base surface. Update the control surface , the relative depth of the dimple changes. very controllable, very quick, very easy. Try doing that with features alone.

3. Design exploration - sometimes when designing you need to move bodies around, see how they interact, try different approaches. With a feature only approach this is much more complex. It needs to be planned.

That last one is I think the issue here. We use CAD to DESIGN. We do not use it to DOCUMENT. If I know what I am going to model I can use any CAD system on the market. If I am using CAD to explore form, edit and tweak I need specific workflows and tools. Creo has a fantastic tool in Freestyle. I want to continue to use it, but if we cannot resolve how to create parts as efficiently as we do now in other systems, I will not be renewing the subscription - which is sad. I have a lot of other SolidWorks using designers looking at our little Creo experiment with interest.

I would be very happy for anyone at PTC to visit me to see how we actually do things, so they really understand the benefits this modelling approach brings. Right now, from what I can see and read, I'm not convinced PTC "get" the issue. I don't see how it is related to the kernel. All a solid is is a stitched up surface, and you have multiple "surface" bodies in a part. In any case you do have multi bodies in parts as long as they don't intersect.

[mneumueller]

KQD (et al),

as a member of the Creo Product Management Team I can tell you that multi-body support is currently an active project within Creo R&D.

I would be very much interested in talking to you to discuss your use cases and will contact you via e-mail.

Best regards,

Martin Neumueller

[khimani_mohiki]

Coming from NX and Catia background it was strange for me to find that I cannot make multiple bodies in Creo and boolean them together, this was key for collaborative modelling particularly in complex injection mouldings. I would be interested in how this develops, currently I don't think the workflow is as efficient as Catia and NX.

[mneumueller]

All,

if you are interested to join the working group, we would be happy to have you join.

Note that the above mentioned previous working group "embedded components" has moved to a more general "multi-body working group".

I would be very interested discussing all of the above mentioned use cases, in particular also including the collaborative modeling, and master model design aspects.

Thanks and best regards,

Martin Neumueller

[dnordin]

khimani_mohiki,

What advantage does multi body parts give you over the existing Boolean functionality in Creo Parametric?  (In assembly mode, search for "Component Operations" if you're not familiar with the functionality.)

Regards,

Dan N.

[KQD]

Multi body is used at part level not assembly level. As far as I am aware there is no Boolean functionality at part level. The issues affect (primarily) people (like me) coming from other systems that have multi body functionality (which to be honest, these days, is everyone else). I have seen what Martin and his team are working on and if we can get that in 6 there will be a lot of happy people.

[khimani_mohiki]

Multibody part would not increase the number of files to manage and would not create issues with external references in the Windchill release process. The current assembly Boolean functionality is limited, I can remove material or I can add material, I cannot intersect or union trim.

Yes, we can do these type of operations with surfacing but still with surfacing I cannot select regions to keep or remove when Merging. I will give yu an example, when designing plastic parts we use dog houses & clip towers on the B-surface, these are common features, I should be able to Boolean to the base solid of the plastic part and selectively remove the areas I don't want. I can dot his with surfacing but its much more long winded.

In terms of the product development for complex plastic mouldings the most flexible workflow I have found and used in various other systems is as follows: Define A-surface & B-surface geometry separately using surfacing > close into separate solid bodies > Boolean solid bodies together.

[dnordin]

khimani_mohiki 

The three boolean operations available in Creo Parametric assembly mode are Merge, Cut, and Intersect.  You'd have to explain why you believe intersect is not an option and how the three operations are limited in functionality.  During the creation of the assembly boolean operations, you have the option of defining the updated control (dependency control).  You can create the operation with no dependency if required.

In Creo Parametric part mode & models containing intersecting solid geometry:

1. a boolean merge option is not necessary because Creo Parametric merges intersecting geometry by default.
2. boolean cuts are not necessary because most feature include "remove geometry" as an option.
3. Intersecting the geometry of individual features isn't possible because the geometry has already been merged; use the assembly intersect in this case or use the merge feature to bring in external geometry to merge, cut, or intersect.

In your dog house & clip tower example, you should investigate the use of UDFs since you stated they are common features.  UDF's can offer flexibility during feature placement.  Another option for common features is the use of what we call "coupon" parts which are simply parts that contain already defined geometry, feature relations, parameters, etc.  When a user needs to use those features in their model, they simply open the coupon part (via a mapkey or menu pick), and use copy/paste to add the features (usually groups of features) into their model.

There are many methods of creating geometry in Creo Parametric, not all of them exist in part mode alone.

Regards,

Dan N.

[khimani_mohiki]

dnordin

Appreciate your input, I will look further into Assembly operations but what about selective Boolean, its possible in NX as Unite and with Catia as Trim to selectively remove and keep some geometry during the Boolean, how can I do that with current functionality of Assembly operations in Creo? At present we have to do this in surfacing by trimming surfaces then merging, this creates extra steps and makes updating the A-surface less robust.

On a complex part I might have several designers just working on dog houses & B-surface features (in real world most are not just copy-paste, each one must be finessed for tool feasibility & sink thinning etc) and some designers just working on A-surface, then we import their solid into the final part and Boolean trim them together, this way we can maximise the Designer resource and minimise the delivery time to the customer. I could do this with surfacing alone, and have seen it done this way in Catia, but it create many extra features to integrate the B-surface detail.

[DougZ1]

I realize this is an old post, but found this post in search for how to do multi body parts in Creo.

I switched from Solidworks to Creo this year with my new job earlier this year.  I work in the valve industry and one thing that multi body parts were used for at my old job in Solidworks was weld overlays.  It's common for valves to have weld overlays that are put on a casting.  The casting is machined before welding, weld overlayed, then the overlayed weld material is machined to size.  In Solidworks, this was easier to handle with multi body parts. I could easily do a revolve, extrude or surface offset & thicken that would end up as a separate body in the part.  Then cut the material down to show final machining. With the use of configurations it was easy to show a view for how much weld overlay to add, and then what it look liked after machining.

In Creo, this is more challenging as you can't make a multi-body part to my knowledge.  The long time ProE/Creo users here have found workarounds, by importing the machined casting model into another model, adding the material and then deleting the material that was imported/merged from the casting model. Then, putting the weld part model and machined casting model in an assembly.  I've also seen ProE drawings where they just sketched the weld overlay in the 2D drawing in a detail view instead of trying to make the weld overlay an actual part/model.

Perhaps there is a way already in Creo to do this, but the multi-body approach made the most sense in Solidworks.  The weld overlay is obviously not a separate part in reality.  The functionality of Solidworks allowed you to assign different materials/colors to the separate body as well so it was easy to show what was the overlayed material, and what was the casting.

[mneumueller]

Hi Doug,

we are working on multibody support for the next Creo version including the ability to assign different colors/materials to part.

If you are interested you can join the respective working group https://community.ptc.com/t5/Multi-Body-Working-Group/gp-p/multibody 

Did you have any PDM requirements as it relates to this? Could you / did you have the need to propagate the different bodies (or their masses and materials) individually to the PDM system?

Martin

[DougZ1]

Martin,

Thank you for the info. I would be interested in joining that working group.

My current company does not use a PDM and my old company that used Solidworks just used their Solidworks PDM for version control and basic search functionality using parameters like part name, model #..etc.  We seldom ever used multi-body parts other than for the the weld overlay process so we never had the need to show/propagate properties like mass/material in the PDM.

I could potentially see the need for those things showing up the PDM, but with the way the valve industry (my industry) is a lot of the times, we don't show materials on drawings since there are a lot of special material request, so our drawings just say "See Part #" and the material information is in the ERP/MRP system that the company uses.

[KQD]

Nice to see this topic being pushed up again. It is, I believe, the single most important feature that the developers at Creo need to sort ASAP. For all the reasons above and more. Doug explains a great example of SolidWorks configurations in conjunction with multi body parts. This is exactly the workflow we use as well, except we use it as a fundamental building block for the parts. Going a bit off piste here I have to say that the moving to Creo from SolidWorks is not easy. Multi Body is a fundamental design process in SolidWorks, Inventor, NX, SolidEdge, CATIA in fact pretty much every other system. Users EXPECT it. Yes, you can create geometry using surfaces and copy and paste etc but that in itself leads to other potential issues with workflows. For example, recently, we have been told that we have to build in context parts using Publish Geometry from a "master part". Currently we do it from an in context part in an assembly and use copy and paste geometry (and it works very very well for our processes). Of course Publish Geometry is only in AAX, which of course has just been hiked in price (nearly DOUBLED). So it is a non starter for us. If we had Multi body parts we do not need to use AAX workflows as we can do it all in one part. Further more, the AAX situation looks even dafter by the fact that SolidWorks 2020 now as AAX like assembly geometyr publishing capabilities. So guys at PTC, please get Multi Body into Creo 7. If it is not there, it is unlikely to be in before 9 (given that only big new features go into odd releases). And that, to be frank, will kill off your competitive use market. One final point Martin, I requested to join that group weeks (months?) ago but I cannot get access. It says "you have already requested to join the group" but there is no access. As I have seen the multi Body work already about a year or so ago (and it looked good then), I can certainly add to the discussion. So let me in please 🙂

[S_Edgenear]

Hi Martin,

Any chance we can expect enhanced funtcionality for Creo 10 (or later) regarding multibodies?

1. Enhanced and time saving boolean operations as Catia, NX and TopSolid 7 have. namely NX Unite Trim that lets the user seleect the "islands" of an union to add to the final boolean result, instead of adding the full volume of both bodies? Or selective trim, that allows trimming to intersecting bodies, but not including from the first body any "dangling" excess material.

2. Ability to use body Boolean operations in the context of an assembly with direct references, as we can make with quilts, namely, adding or removing material with a quilt, with the solidfy command, withhouth having to copy first the quilt to the target part, as currently we have to do with the bodies. This would speed up tremendously certain workflows where we could finally use a construction solid body in a part (or a component of an assebly) to make "cutouts" for the assembly of the part (or subassembly). Currently we still have to use quilts for these cutouts, since tu use solid bodies, we waste much more time to first copy the bodies first into the target part.

3. The ability for the multibody boolean operations to transfer colors from the source body into the target body. Using component Boolean operations with whole components in an assmmbly also transfers color, but currently, using multibodies, does not.

4. The ability for the multibody boolean operations to (optionally) transfer axis and/or hole threads (as allowed by NX), and as allowed in the old Creo assembly muti-Component Boolean operations, but adding more inteligent behaviour. Namely, only transferring axis or threads that are associated with non-disappearing solig geometry in the final target body. 

5.  The ability to define a body (or several bodies) inside a part (or an embedded copnent inside an assembly) as special "CUTOUT" construction solid geometry. This would allow automatic boolean operations whenever we add such part to an assembly (or a sub-assembly to a higher level assembly). The idea is that when we assembly a part that needs an hollowed out space on other parts in an assembly, that the "hollow geometry" is automatically subtracted when we assemble the part. Currently Catia can do this, NX also, Top Solid 7, also. If the part as a pre-defined body with a user specified name (or with the attribute "cutout" (currently there's also the attribute "Construction"), if there is a single body with the attribute, when assemblying the component, Creo should ask the user which parts of the assembly (and which bodies inside those parts) to make boolean subtractions to cutout the space for the component. If there are more than one bodie with such attribute, automatically let the user pick from those 2 or more bodie names, which one the user wants to use for the boolean subtraction on the target bodies of the target parts.

6. Inside a single part to be used as a skeleton, it would be nice to expand the hole command to make with a single feature, standard holes with both the clearance part (one one or more bodies with optional counterbore or countersink), and also the tappig or thread part on a target body at the bottom of the stack. Currently, the hole command can make holes on several bodies, which is nice, but does not allow to have the tapping part, which needs to be done as another feature, which is not associative with the first. It would be nice to have this in the future, to avoid having to do it non-parametrically, or have to resort to create UDFs for such a common operation.

7. Still concerned with the multibody improvement capability, namely with points 3. 4 and 5, to prepare the "cutouts" bodies, it would be desirable to extend the hole command to generate a "negative" solid and thread to be subtracted on a target part.  This means, if we are creating a cutout body for a hole, (in which the thread is created inside the nominal diameter) in the cutout, the thread has to be created outside.

Thank you,

Sérgio

[mneumueller]

 Thanks for this summary. They  include some good points and re-iterate earlier working group discussions.

To answer in short:   Yes, there are multibody enhancements  being planned for Creo 10.0  (including ongoing work for sheetmetal and some items from this list) as well as captured as backlog items for future releases. I plan to review/discuss them in working groups as we progress.

[S_Edgenear]

@mneumueller 

Thank you, I appreciate the feedback. Looking forward to seeing the future enhancements to one of the key aspects that we consider for the increased productivity in Creo.