Can subassembly be modeled separately from Main Assembly?

[wathavy]

Hi.
I have main assembly as I attach.
They are composed of three main subassemblies. And I start building the details of each of subassembly.

Questions:
1. Can I modify the subassembly alone in new session and keep modifying and I can still maintain the assembly updated with my modified subassembly?

2.If the above is 'NO', then what else can be done to work separately?

3.Or do I have to have pseudo subassemblies instead of real ones in my main assembly? ( Just like we used to do in 2D work... perhaps )

As the matter of fact, I do not have to worry about this issue, because I supposed to finish all by myself with this case. But if the machine get bigger, I possibly need help with other hands. Then I need to share the subassebmlies. And keep updated.
For this moment, I could ease my PC load if I know how to.

Any suggestion will be welcome.
Thank you for paying attentions.
Best Regards.

P.S.
The model manager module is not bought. And I am working without any version management either.

[clausb]

Originally Posted by wathavy

1. Can I modify the subassembly alone in new session and keep modifying and I can still maintain the assembly updated with my modified subassembly?

Yes.

3.Or do I have to have pseudo subassemblies instead of real ones in my main assembly? ( Just like we used to do in 2D work... perhaps )

No.

Just save your data in *.sd* format (instead of package files), and you can load or modify each part or subassembly individually.

Claus

[wathavy]

Thank you, Claus.
I will definitely try it, first thing in the morning, tomorrow.
Thank you again.

[wathavy]

Hi, thank you Claus.
I somehow managed to save them each indivisually at separate folders. And I succesfully reloaded them back to original positions.

But one of the subassembly needed to be merged together with the other one. Because that particular subassembly were originally made at absolute origin. So when I have it saved as '3D Data' or '3D modified' or '*.sd*' and reloaded, it was placed at the original position instead of the required position.( see attached picture )

Luckly, I have other subassembly which are designed top-down and placed at exact position where I want it to be, I made a new pseudo folder to contain the predescirbed subassembly into it. Now it seems fine....

I got dozens of questions about this issue now, but I might postpone them, since I need my work to be done.
Again, thank you so much about this.

( Is this a new feature? According to my collegue, the dealer here said this isn't possible.)

# Attached picture is unsuccessful one. Then I noticed the workaround... Or is there a right procedure to memorize subassy's relative postion? Oops, this is just a part of my questions...

[clausb]

Roughly speaking, if you have an assembly structure "/foo/subassembly", and you position "subassembly" relative to "/foo", then that position information is stored in "/foo". Hence, if you load just "subassembly", you don't get that position information. If you think about it, that's the only approach that makes sense, because subassembly could be used in hundreds of other assemblies, and trying to store (and maintain) its relative position in all those assemblies within the subassembly itself would be a nightmare.

( Is this a new feature? According to my collegue, the dealer here said this isn't possible.)

Which feature exactly do you mean?

Claus

[wathavy]

Now I seem to recognize your point. The subassembly without assembly's location is useful for future use. That makes sense.

The feature which dealer mentioned not possible is this subassembly feature stored separately with position relative to other subassembly.
But the story is heard via my coleague, so it could have been distorted.
And the dealer is sales person, not an engineer. And what he said is at the end, we still need to have all subassemblies loaded into one whole main assembly. And it may exceed the CPU power if the whole assemblies are huge.
The last part is true, yet, right? If so, the sales man was partially right, not totally, though.

Besides, I checked 'version' for the file save option. Then every save the part name increases its number by itself. And I saw the directory is now full of numbered parts. Is there way I can purge the old versioned parts?

Thank you.

[clausb]

Loading large assemblies rarely exceeds the "CPU power" - the bottleneck usually is memory. Also, you can handle quite large assemblies in CoCreate Modeling. We have customers building assemblies with several 100,000 parts.

That said, many users load and work on subassemblies, and performance is much better, of course, if you only need to load 100 parts instead of 100000.
Many of those customers rely on the assistance of tools such as Model Manager because it takes care of all the menial work of storing models in the right places, versioning, locking and unlocking them, and providing ways to attach related non-model data. Also, Model Manager provides advanced options to load models in "partial" or "lightweight" mode. (In these modes, you can load data-reduced versions of the model, which saves a lot of memory.)

Which 'version' option do you mean exactly? Could you post a screenshot?

Claus

[wathavy]

Thank you, Claus.

Which 'version' option do you mean exactly? Could you post a screenshot?

Here is the open dialog box which shows 'Version' and previously automatically numbered '*.sda' data.

I also do not know the functioning details of the '*.sd*' file type saving process. I got stunned with other dialog asking me to it 'Yes' or 'No'. I seem to understand if I say 'Yes' it will version up and the number is increased. On the contrary, if I say 'No' the version number is kept and the file is overwritten.... Am I correct?

Thank you for paying attention.
Cheers.

[clausb]

OK, so you were really talking about the "LOAD as version" option in the LOAD file dialog. I was confused because you originally said "I checked 'version' for the file save option."

"Load as version" is used, for example, to load multiple versions of the same part into memory, and compare those versions. See the online help documentation (topics "Model versioning", "Integrate imported models"). Are you sure this is what you want to do?

About the multiple files issue: When a file name collision occurs and you explicitly ask Modeling to generate new filenames, it will do so. However, this is just a new name for the file, not what in Modeling lingo would be called a part version. If you don't want all those files, simply don't let Modeling generate new filenames when saving!

My interpretation is that you did not really intend to create all those extra files. That should make it straightforward (in your case) to write a little throwaway shell script to delete the old files. At least, that (or simply deleting the old files using Windows Explorer) would be what I'd try.

Claus

[wathavy]

So, I need to wait until I see the help at office, though.
Assuming that what I checked was not version for modeling but sort of renaming process alone, what I should have done was not check the box.
And save as *.sd* only.

Anyway, I need to sort out my clattered files tomorrow morning then.

Thank you.

[Mike Swartz]

When saving 3D data, you do not get a choice of the file name. The file name will be generated based on the name of the part/assembly that you are saving.

The actual question asked by the system when you resave existing 3D data is

Some of the objects in your selection will overwrite existing files. Press Options for details. Do you want new names generated instead ?

If you select no, your existing files will be overwritten.
If you select yes, a new file name will be generated, by adding a -1, -2 to the file name.
This allows you to store "versions" of the files in your file system. If you do not want these "versions" you can manually delete them from your file system, but you need to keep the latest version.

WARNING!!! NEVER rename the .sd* files.

[Mike Swartz]

For What it's Worth.

If you have very large models, and/or if you have parts and sub-assemblies that are used in multiple assemblies, and/or you need access to previous revisions of your parts or assemblies.......

You NEED Model Manager.
It will more than pay for itself.

[May Kung]

Originally Posted by Mike Swartz

For What it's Worth.

If you have very large models, and/or if you have parts and sub-assemblies that are used in multiple assemblies, and/or you need access to previous revisions of your parts or assemblies.......

You NEED Model Manager.
It will more than pay for itself.

++ Very much agree on this point. The first time we used a PDM I didn't see what the fuss was (this was WM 5.1?). But once our parts were in the system, I could see just how powerful it is having a PDM.

Alas, we're now using a PLM which isn't nearly so convenient as MM. It's so inconvenient that many are simply storing stuff on network shares instead of using the PLM; it's a nightmare trying to get assemblies to behave when they're scattered this way, especially if you're sharing things.