Provide option to import STEP file as multi-body part instead of assembly

dcokin · ‎May 06, 2020

Oftentimes when importing a model from a vendor, it will come across as an assembly with numerous parts that do not match our standard naming conventions, and are not really needed to integrate their product with ours. I typically spend a lot of time "shrinkwrapping" such assemblies down to one part, without any interior detail, to avoid having to load all the original components into our PDM system individually. The shrinkwrapped part with less detail may also offer better performance. At times though, it may be desirable to retain all the original detail, but still not have to manage numerous additional part files for the subcomponents. Now that Creo 7 has introduced multi-body parts, I would like to be able to import an assembly as multiple bodies of one part, rather than multiple parts of an assembly.

RobertH · ‎May 08, 2020

According this it's added to Creo 7.0.

dcokin · ‎May 08, 2020

Thank you for this @RobertH! I was not familiar with the hidden "intf3d_in_as_part yes" option, but that is really helpful! I just tested it, and it works the same in Creo 4.0 M060 & Creo 7.0.0.0. My product idea remains though, as I would like the option to import as either an assembly, a multi-body part, or a single body part. (This setting allows the single body part import to work properly for the first time with all models; previously would only be effective if all the components in the model were initially defined in the same coordinate system; but if they'd been "assembled", this doesn't work right without that setting.)

Such a strange setting! I wonder why it's hidden, and affects both the default import pick, and how the import works if you select 'part'. (Why would anyone ever want the import to work the old way, with assembly errors?) I don't think I'll be making this part of my standard configuration, because I would like "assembly" to still be the default option, but I will keep this in mind for times when I'm going to shrinkwrap the assembly down to one part anyway. This may make that not necessary, or may speed it up. (May still be necessary to do further processing to remove internal voids, etc.) Very strange that the default behavior is for models to not to come up assembled properly when you select to import as a part. They've had a solution to the issue this whole time and hid it from us??!!! This has been an issue for more than 20 years! (I remember early in my career, I was helping to plan one of the Hubble Telescope servicing missions for the Space Shuttle using CATIA v4, and we had lots of trouble importing the payload models from Goddard, who were using Pro/E, because they weren't assembled properly. In that case, it was an export problem on the ProE side, but was otherwise the very same issue, where every component in the assembly reverted to default position, without respect to their assembly constraints.)

RobertH · ‎May 11, 2020

Welcome to the world of PTC where logical is not always locigal..

As I don't import very often for us it's not a huge problem and if I have trouble I blame it on an incorrect export 🙂 but probably that is not always true. I didn't test the setting as I also wasn't aware of it. I read your question and then a few minutes later I ran into the article so I thought I share it with you.

lhoogeveen · ‎Feb 09, 2021

In Creo 7, is there a way save a Creo assembly to a multibody part? I don't see an obvious way to do this either.

amansfield · ‎Apr 30, 2021

We need multibody support to allow us to:

import vendor component assemblies as a single model with watertight bodies for each component part. This will make it easier to manage in Windchill without having to assign a compatible number scheme to each part and sub-assembly.
define different materials, etc within the multi-body part file
show boundaries between bodies
show different crosshatching on a drawing between bodies..

After I posted this I tried setting the "intf3d_in_as_part yes" option and imported a complex assembly STEP file as a part. I redefined the import geometry as "Add Bodies" instead of "Add Material" and it separated all the independent bodies and added them to the model tree.

Fantastic! Works just like I wanted it to..

Now all we need is an option to "Save As" an assembly into a multibody part file without having to STEP it our first.

VMcD · ‎Sep 03, 2021

Does the inseparable assembly method meet this need?

https://support.ptc.com/help/creo/creo_pma/r8.0/usascii/index.html#page/whats_new_pma%2Fmulti_body-n...

dcokin · ‎Sep 03, 2021

@VMcD

> Does the inseparable assembly method meet this need?

Hey yeah, I think it might! I'll let you know in a couple years, after we upgrade to Creo 8 or beyond... (We're still at Creo 4.0 at my site, although other sites in our company recently went to Creo 7.0, and we are expected to follow suite by years end.)

Although this technique will take care of one of my concerns (needing to create individual line items in our database for all the vendor's subcomponents), it doesn't sound like it'll actually help with performance, the way shrinkwrapping to one part with all the internal details removed would. Good to have both options, for use as needed. But this definitely seems like an even better solution than my initial suggestion of representing vendor assemblies as multi-body parts!