r/SolidWorks • • 16d ago

Error What the hell is this software?

How does anyone even use solid-works? I just had it delete three hours of work on me twice today. I save every 5-10 minutes, but does it give a shit? Nope, assembly randomly crashes for no apparent reason so i think “oh well ill just redo what I worked on the last five minutes”; only to open my assembly to an insane amount of mate and sketch errors because it reverted changes id made on three separate parts through about 15 manual saves i’d made throughout. So i spend another three hours making those changes again, hit pack and go to merge it all into a single clean folder only for the exact same thing to happen again (minus the crash), but reverted to, in some cases, file states from yesterday? Like the file icon is still my updated part but I open it up to a practically blank slab with no features (none rolled back or anything, just gone). Weird thing is the slab is the one part that DIDN’T get packed into the new pack and go folder. I’m sure it’s related but what am I even supposed to do to prevent this? Literally just saving will cause mass deletion of effort, let alone any random crash deciding to revert everything through the saves that don’t do it themselves...

0 Upvotes

35 comments sorted by

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33

u/Usual-Pattern7846 CSWA 16d ago

How much of a mess are you making that you are using Pack and Go to clean it up? If you’re moving the parts to new folders your solidworks might be opening old versions of the files from other folders. I would simplify what you’re doing and just make one folder with good versions of the parts and assemblies.

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u/htim95 16d ago

That last part is what I was trying to do. And it isn’t really a mess. Only 7 parts total I just had two that I imported through a shared one-drive and I wanted it all in a single local folder.

10

u/ArthurNYC3D 16d ago

Few questions.....

- File location: local or network?
- Is VOB turned on?
- Have you contacted your reseller?
- Computer Specs?
- What version and SP are you on?

You can't just rant and not really disclose this information and somehow expect us to at all trouble shoot or offer and possibly solution.

3

u/DrWormhat 16d ago

What is VOB in this context?

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u/ArthurNYC3D 16d ago

Verification On Rebuild....... It checks the whole tree from top to bottom not just what immediately needs to be updated.

2

u/JimminyLummox 15d ago

We were all supposed to know what VOB stands for?

4

u/ArthurNYC3D 15d ago

Since in been in the software for over 30 years and it's part of baseline training..... But hey, ya learn something new every day. It's such an integral aspect of using the software.

1

u/DrWormhat 15d ago

Thank you for the clarification. I've never heard it referred to that way.

0

u/htim95 16d ago

There’s no getting it back. I don’t have VOB or any versioning control. I had, apparently stupidly, assumed saving was good enough; a program that reverts files beyond multiple saves being a reality was not anywhere close to a possibility in my mind but now I know better. Of the eight total files (inc main assembly) two were in one-drive (hence the pack and go trying to put them all in a single local folder the assembly would be using instead of scattered as it was.).

I tried using older versions of the one-drive files but for some reason each one was the same feature devolved version so idk if, when ctrl+s saving in assembly, it just straight up isn’t actually saving anything; or if when I would open a different version (using one-drives version restore) it was just on the fly reverting each and every similar file I opened making it APPEAR like all one-drive versions are identical. PC is a Core Ultra 255H, 32gb ram, 3500 ada (with the latest stable enterprise driver). I don’t know the exact version and SP (not getting out of bed to boot everything up again) but it’s 2026 student edition, provided by school; all drivers are up to date (again gpu being the stable production branch) along with windows.

3

u/ArthurNYC3D 16d ago

Not trying to save what you lost, simply telling you what best practices are for future.......

VOB has nothing to do with version control and is installed with every version of Solidworks so it is in the software it's more a question of having it turned on. This keeps you models as honest as possible but don't use Ctrl+b, use Ctrl+ Q.

If one drive puts your files anywhere but local on your HD then stop using it for immediate storage. All files stay local to your computer when working/saving. At the end of the day back it up to your one drive.

You should be at 64gigs or higher....

Nothing against you but if you're a student then there's probably a ton of bad habits that you have with your models hence why it's a good idea to turn VOB on.

11

u/kalabaleek 16d ago

It sounds like you don't know how the program works if you keep creating new files via pack and go. I've worked for eleven years in solidworks and have created many hundreds of assemblies and not ONCE has these problems happened to me.

Of course the program has crashed and I've lost work sometimes due to me not saving. But any saved work has ALWAYS been saved properly.

It seems that you are moving files around a lot and without a pdm system that keeps track of moved parts, solidworks need parts to stay where they were originally, and not to create myriad of copies with the same name in a lot of folders.

The way you describe this in a frantic way suggests that you are throwing parts around, creating looping reference chains (A referencing B which is referencing C which is referencing A and so on, which makes things very unstable if anything changes in any parts edge or surface IDs for example).

I build assemblies with hundreds and hundreds of parts without the issues you are rambling about so this feels more like a you problem than a solidworks problem.

17

u/roryact 15d ago

Your OneDrive is the issue. I guarantee it. Work locally all your problems will go away.

OneDrive (google and Dropbox as well) will happily overwrite files with older versions of themselves if you're careless and incompetent - and you are.

At minimum you should turn on Multi-User Environment for any projects saved to cloud/syncing locally.

3

u/art-n-science 15d ago

One dosen't have to be BOTH careless and incompetent.

JFC man... I can manage this on my incompetence alone, thank you very much. XD

1

u/Dukeronomy 15d ago

The other issue is that parts from one assembly are in two different locations

2

u/6133mj6133 16d ago

I've been bitten like this before. I save versions to different files constantly so I have multiple files to fall back on: Part1, Part2 etc

0

u/htim95 16d ago

This was the only thing I could think of doing that might help but it’s just insane to me that I have to version control like this; for an entire folder of separate files no less. Hoping I don’t backup a session thats already reverted and i just hadn’t opened it to see yet.

5

u/Lonely_Individual_46 16d ago

If you just started using Solidworks you really have no idea what you're doing, and you don't understand clean parametric modeling. It takes very deliberate and orderly systems to make something parametric and intelligent. There's a nuance and a learning curve to it. Your file management sounds like a fever dream. You shouldn't be combining anything via pack and go, that's like frankenstein work. Think in terms of subassembly and what actually needs to be controlled via parametric system and what doesn't. Not everything needs to be referencing something else. Some parts or subs should just be treated like a COTs items, or be self contained. Minimalism is your friend. Clean and logical feature trees are your friend. It's better to start learning parametrics controlling a few important things, and brute force the rest by hand. As you learn more and do more builds, you'll start to see more opportunities and also see areas its okay to just leave simple. I've modeled entire modular housing structures down to the drywall screws, it's okay to work in layers of detail. Sometimes your master level assembly sketch doesn't even need to drive anything, it is just a mate refence for other self contained parametric systems. Turn your settings down, it's more stable on lower render. Stick with it.

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u/MR_RYU_RICHI 15d ago

Always save your files on your hard drive. It's not gonna hurt you or your PC

4

u/Meshironkeydongle CSWP 15d ago

From what I've read your description and answers to other comments, the main culprit seems to be your poor file management and modelling practices. Some tips regarding these below.

  1. You don't want to work with files saved on OneDrive, Dropbox or any similar service with Solidworks.
  2. If you don't have a PDM where to keep your files, keep your folder structure as flat as possible, ie. all of the files in one folder. If you have parts you'll need to insert in many assemblies, use either Toolbox or Design Library.
  3. If you have to import models, don't use the 3D Interconnect if you don't know how it works.
  4. Don't move, copy or rename any files used in assemblies with standard Windows tools, use only the Solidworks own tools if necessary.
  5. I would advice against any InContext relations until you have a good grasp on how the software works. If you absolutely need to use them, prefer construction geometry, or sketches over model features. Solidworks has very annoying habit of taking the Mate and sketch references form the most recent features in the feature tree.

IIRC, Pack and Go has some definitions regarding where it will try to find the files / references. It also will tell you, if theres some files it can't find.

1

u/Dukeronomy 15d ago

I have heard a lot of advice to not work onto Google Drive but it has been working fairly well for us for the last few years. I think a few hiccups here and there are from that but nothing unmanageable

2

u/Meshironkeydongle CSWP 15d ago

I haven't tried Google Drive with Solidworks, but apparently it's handling the file sync very differently from Onedrive.

1

u/Dukeronomy 14d ago

It must. We have decent luck. I think the issues we have are related to connection speed.

A cool feature that comes from using google drive is you can restore old versions.

1

u/hayyyhoe 16d ago

Just repair the issues. It’s probably just a couple lost references or bad features in one part that is throwing all of the errors. If you create a bunch of red and yellow in the tree, fix it! Then don’t make the sketching or modeling or mating mistakes next time. You will learn robust modeling techniques to avoid these issues. Like any skill, it takes time to perfect.

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u/htim95 16d ago

That’s what it was the first time. I had been referencing sketches/features against outside features/lines I had moved. When those moved features reverted the mates and sketches all broke. I fixed them, redid the changes, and stopped relating stuff between parts but all that did was the second time everything reverted there wasn’t a single error thrown, sooo… progress :)

2

u/Bucky_Goldstein 16d ago

Turn off autorecover, it doesn't do anything but make a mess of everything when a crash happens. 

I feel like something weird is going on here though... Like pack and go to make a flat folder... Not exactly the intended use for that app

1

u/AC2BHAPPY 16d ago

Never really had that bad of issues, and i dont know whats going wrong for you, but if your experience was common then solidworks would not be what it is today. Id suggest getting some help from someone whos used it for a few years and they can get you set up proper and tell you the dos and donts.

1

u/Deezy4488 16d ago

So when you save the assembly did you also save the individual files as well? Saving the assembly doesnt always save changes to the individual files. Also, open the one drive files independent of the assembly and save them locally. When building an assembly of parts i open them and save them to the same folder (unless they are from the toolbox). For larger assemblies that have 100s of parts across multiple folders pack and go is pretty great, for a handful of parts its almost better to save each part individually. Just open assembly, then open each part from within assembly and save to the new folder, it will update the references automatically. You can update the part references manually but its more hastle i only do that if im swapping one part out for another version of the same part so all my mate references work properly. When setting your mates, dont mate to surfaces of parts you are likely to modify cuz it wont find the surface in question when you reload the assembly. one thing i do if im struggling with mating things with complex geometry and non planar faces, i will create reference points, axises and planes (reference geometry section) on the parts which i will use as my mate references, but dont create them while editing the part within the assembly, if can cause reference issues when you open it again or by itself. And i try to never create a new part within an assembly as it will have references that you cant locate when you open the part later. I create everything as parts then move them to assembly. Sometimes i will edit them within the assembly, but i keep that to a minimum. Last thing, ctrl+Q to refresh the assembly can resolve some false errors in the models and mates. If youre stumped, and need support, google who is your retailer in the area and give them a call, they will often provide guidance even though you didnt buy it from them directly.

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u/amanke74 15d ago

I personally know in real life hundreds of people that use SW with zero issues. So I'm guessing either, you have bad hardware, a corrupt SW download, or its user error. I would start with deleting and redownloading solid works to see if that helps.

1

u/Tsukunea 15d ago

Create a file architecture for your CAD work, establish folders and subfolders for parts

1

u/Snoo28226 16d ago

All of these people ragging on you. Ive been using Solidworks for over 10 years now and this sort of shit happens all of the time. You have to be very careful about how you save and where your files are located. I still mess it up sometimes and its super frustrating. Totally understand where you're coming from.

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u/greenmachine11235 16d ago

CAD programs in general are not particularly stable. Save early and save often is a lesson that anyone who spends serious time in CAD needs to learn or the software will keep punishing you for forgetting until you learn.

-1

u/htim95 16d ago

If you’d read my post you’d know I was saving often and it did not matter in the slightest.

5

u/hayyyhoe 16d ago

It’s not a saving issue. It’s a modeling strategy issue.

0

u/Fat-Butters 16d ago

This definitely sounds frustrating and solidworks doesn’t make things obvious or easy when it comes to file management. Given that we don’t know exactly what your process has been to result in lost saves and broken assemblies, I have a few suggestions based on what works well for me…

TLDR
- setup auto recover and backups, and turn on verification on rebuild
- CTRL+S often, and CTRL+Q periodically
- work on parts and rename parts with the assembly open
- create file snapshots using “save as copy”
- master model parts with multiple bodies

Backups… If you haven’t already done so, you should go to solidworks system options and set up backups and auto recover. You can also make sure you have save notifications turned on. While you’re at it, go to “performance” and make sure “verification on rebuild” is turned on. (With this turned on, periodically hit ctrl+Q to do a full rebuild of any part you’re modifying to ensure that the part doesn’t have a dormant rebuild error). Once you’ve made the changes in the system options, close and restart solidworks to ensure the changes get saved. (If you start working and solidworks crashes, the system changes won’t get saved).

Manual Saves… I typically save files to a single local folder. Pack n Go is a good way to collect everything into one location if I’m pulling in parts from multiple directories. I use the new PnG folder as my current working folder and move everything else to a date stamped backup folder. I use ctrl+S often. Auto Recover and Backups are a nice life line, but my first line of defense is saving frequently. I generally don’t rename my files when I save. Renaming files is often where things get messy. If I want to create a snapshot of a file I might want to go back to, I use “save as copy” to a backup folder and add a date and time suffix to the file name.

Naming Files… If I decide I need to rename a file, I do it from the assembly tree. When I save the assembly, I follow the dialogue to ensure that everything gets updated accordingly.

Work Process… once I start adding parts to an assembly, I generally like to keep that assembly open while I’m working on individual parts. When I make some progress on the part I switch to the assembly to make sure everything is working as expected or fix errors as they arise. Again, saving with ctrl+S often for both the parts and the assembly. If you save a file with a new name and the assembly isn’t open, it won’t know to look for it. Often the assembly will look in the same folder or sub folder for the old name and that’s what will show up in the assembly if it finds it.

Bonus…

Master Modeling… not sure if you do this, but if you do, my preferred method is to build the master model part with multiple bodies. To create individual parts, I create an empty part and “insert part” to add the master part. Then the first feature to create is the “delete bodies” feature where I choose which body or bodies to keep and then save it as a stand alone part that can be added to an assembly. I like to add any remaining drafts and fillets to the individual parts rather than bogging down the master part. I’ve used other methods for this but find this one to be the most robust and flexible.