CAD Forum

So,

I got this part which the user created a multi body assembly in SolidWorks. Don't ask me why. The feature tree is well and full of his work.

I would like to split the parts out into an assembly, but the "save bodies" command creates basically just dumb solids.

Is there any way to save the bodies as parts with their features intact?

Thanks!

you could insert the part into another part and have it insert bodies and then suppress the undesired ones for each part. There's a few ways you could proceed about this.

I would do a "Save As" on the multi-body part for as many individual parts that I want. Then open each one and delete all of the features for other bodies. Depending on the complexity of the assembly, this could be a time consuming task. Add all of these parts into a new parent assembly with all sharing the same origin.

SPerman wrote: ↑Fri Feb 02, 2024 8:41 am I would do a "Save As" on the multi-body part for as many individual parts that I want. Then open each one and delete all of the features for other bodies. Depending on the complexity of the assembly, this could be a time consuming task. Add all of these parts into a new parent assembly with all sharing the same origin.

You could insert into another part, and then get the features. That probably stands the best chance of working.

And if there are any inter-relations, there might be a lot of repairing to do.

Or as an option, save out the bodies and use Featureworks to re-feature them.

Or save out the bodies and get a real direct modeler to deal with changes.

Alternative - re-educate the user. Have the user extract all the junk. Building assemblies with bodies is short term lazy.

Do you plan on keeping, using, maintaining, copying this assembly and or it's parts for years to come? If no, then whatever is simplest, probably what Scott and Alex said, or since you won't be maintaining them, what's wrong with dumb solids.(1) If you will need these models for years to come then, and I'm on a bit of a limb here, but if that's how they modeled it then they probably don't understand many of the other best practices that apply to your use case. I'm assuming you very well know what's best for your use case, You'll be better off long term to remodel them from scratch.

*1, dumb solids with no feature tree are usually better than solids with dumb feature tree.

doobes wrote: ↑Fri Feb 02, 2024 8:20 am So,

I got this part which the user created a multi body assembly in SolidWorks. Don't ask me why. The feature tree is well and full of his work.

I would like to split the parts out into an assembly, but the "save bodies" command creates basically just dumb solids.

Is there any way to save the bodies as parts with their features intact?

Thanks!

Just use them as dumb solids.
Depends on how the other model it, most likely all the features are related to each other.
It'll be a mess trying to figure out which feature will change what.

doobs you mean it's a muliple body part, correct, not assembly.

Maybe they were using the master modeling way that many Industrial designers use instead of top down assembly modeling where the new parts are internal and reside only in the assembly.

In the multiple body part you could do folders to group the features of each body, but some features may not go into certain folders do to how they modeled. You can also make configurations and delete the bodies, which leaves a feature at the bottom of the tree, then put each config in an assembly.

again many good suggestion by the others.

I have to deal with this all the time with student files, features are in know chronological order that make sense, there like a shotgun blast

Frederick_Law wrote: ↑Fri Feb 02, 2024 9:27 am Just use them as dumb solids.
Depends on how the other model it, most likely all the features are related to each other.
It'll be a mess trying to figure out which feature will change what.

This is very true. I have been thinking about this while I am working on a custom truck body. (Yep it's multibody)! So I have only been working in design for about 2 years and basically the only training I had was what I learned from tutorials, asking my boss how he would build a particular part, and whatever help I could find from here & other forums. I have learned a lot in the past 2 years & I still model most of our items (Mostly sheet metal) as multibody parts. Especially so if the parts are all going to be welded together into one sub assembly.

I do use save bodies once in a great while but since most of our parts are one off items or one off variations of an item we very rarely save the individual bodies as their on part. That said what is wrong with a dumb body? Is there any reason why you can't go to the original multibody part to make the changes needed to the part, then do a rebuild & if SW does what it suppose to do the change should happen to the dumb body?

With using the split feature we have found that to get the bends & sheet metal properties on the saved part we need to add the convert to sheet metal feature in on the saved part. But then since I'm new to this maybe I'm missing something?

DLZ_SWX_User wrote: ↑Fri Feb 02, 2024 10:07 am That said what is wrong with a dumb body? Is there any reason why you can't go to the original multibody part to make the changes needed to the part, then do a rebuild & if SW does what it suppose to do the change should happen to the dumb body?

No features in dumb body.
Dumb body is not the problem.
Problem is editing features in multibody.
If you're working on someone else's model, you have no idea which feature affect which part.
Some feature might affect multiple parts.
There might be 100s hole features and have fun finding the one you want.

I'd like to offer an alternative solution. You could keep this Part, with with multiple configurations and use multiple Delete Bodies functions to delete all bodies except one, of course excluding a different body for each feature, and set the suppression state for each as appropriate.

That way you'd have the original configuration with all bodies, and one configuration for each single body. You could then insert them into an Assembly if needed.

I used to model multibody parts (assemblies) in unigraphics back in the days. At that time we did not have a assy license at all and used UG for surface modelling and complex die cast and plastic part design only. then switched to full 3d and started to appreciate the benefits of using assemblies. :)
But I have to admit modelling as multibody in the same context is easier... it depends on a lot of thing and in the end what data output you need from your cad.

in UG (now nx) there was not a real distinction between drawings, assy and part design. a .prt file could be used to mate other prt, like an assy it can also contain the drafting data together with the 3d data in a sIngle file.

Also for vehicle design is dummy body galore and all parts are relative to the vehicle main assy csys so you could just import everything as a body and it would automagically be in position.
parametric design is good, but at some point (bumpers, trims, big parts) you will not dare to modify or rollback something 2000 features up in the feature tree unless it is absolutely necessary and there were no alternatives.
At another job we made mould design for third parties (many automotive) and all the parameters you need are in the mould base and the parting surface: the rest could be relinked and modified with direct modelling, also a dummy solid is lighter.
every company has its own way to do things: fewer people, no shared data between projects, data stability vs speed.

doobes wrote: ↑Fri Feb 02, 2024 8:20 am So,

I got this part which the user created a multi body assembly in SolidWorks. Don't ask me why. The feature tree is well and full of his work.

I would like to split the parts out into an assembly, but the "save bodies" command creates basically just dumb solids.

Is there any way to save the bodies as parts with their features intact?

Thanks!

Hi Doobes,
Is this perhaps a Virtual Component (Assembly)?
https://help.solidworks.com/2020/englis ... L_COMP.htm

Glenn Schroeder wrote: ↑Fri Feb 02, 2024 12:13 pm I'd like to offer an alternative solution. You could keep this Part, with with multiple configurations and use multiple Delete Bodies functions to delete all bodies except one, of course excluding a different body for each feature, and set the suppression state for each as appropriate.

That way you'd have the original configuration with all bodies, and one configuration for each single body. You could then insert them into an Assembly if needed.

Geeze. That's way too simple....
Prolly the best solution.

Thanks to all who chimed in. Appreciate the suggestions.

doobes wrote: ↑Sat Feb 03, 2024 8:31 am Geeze. That's way too simple....
Prolly the best solution.

Thanks to all who chimed in. Appreciate the suggestions.

I really wouldn't do that, I do tool design and you have no other way then doing multibody parts for the splits and inserts. Sometimes the history tree gets very long. If you are used to it it is no big deal.

Anyway if you do the configurations you will potentially run into horrible rebuilds all the time. Instead just save the bodies out or insert and delete bodies for each part. This way You will never get a rebuild unless you go into the original multibody part and edit it.

As for changing the original multi body part, if it is complex, make a copy so you can reference back to check what things are supposed to do and the final geometry (break external references on the copy). There is also compare body in evaluate to do a 100% check.

Thanks.

This is kinda a quick and dirty model of a drill press to go in my garage. I wound up splitting the thing into bodies, exporting as a parasolid and then imported them as parts into an assembly. After that, it was fairly easy for the recognize features dohicky to do it's thing.

The reason I wanted to have a real model was far smaller than the actual drillpress. I'm doing a garage layout so if it's close it's fine.

thanks to all.

I think we can call this done!

doobes wrote: ↑Sat Feb 03, 2024 8:31 am Geeze. That's way too simple....
Prolly the best solution.

Thanks to all who chimed in. Appreciate the suggestions.

I'm not an engineer, which is probably why I like simple.

Wait.... All you wanted was a model to fit in your shop? Why the heck would you go through the trouble of making an assembly?

josh wrote: ↑Mon Feb 05, 2024 11:11 am Wait.... All you wanted was a model to fit in your shop? Why the heck would you go through the trouble of making an assembly?

Looks like I was doing it wrong when laying out CNCs in plant. Should have modeled every nuts and bolts.



Just take the multibody part and save it as combined body without all the internal details.
Unless you want to 3D print and build it.

josh wrote: ↑Mon Feb 05, 2024 11:11 am Wait.... All you wanted was a model to fit in your shop? Why the heck would you go through the trouble of making an assembly?

Small(ish) garage, lot's of bits and bobs.

I will admit to being a tad OCD though....