This seems like a dumb question since I've already taken some training courses, but where does Solidworks look to locate components? Does everything have to be in the same folder?
This seems like a dumb question since I've already taken some training courses, but where does Solidworks look to locate components? Does everything have to be in the same folder?
Hi Kevin, it's not a dumb qeustion!
Let's check the info in the link. It's a search routine, step by step, how SW is looking for the referenced files:
2019 SOLIDWORKS Help - Search Routine for Referenced Documents
BR,
Kamil
They don't need to be in the same folder.
When you create the assembly, Solidworks remembers where all the files were stored initially.
If you open an assembly, you can use the File->Find references to see where all the parts are located on your network/folder structure.
This is why it's important not to move files around without using Solidworks Explorer. If you move parts to different folders and/or rename them, Solidworks will freak out and not know where the parts are when you open the assembly.
Then you get to have fun relocating them.
If you are in an assembly and wanting to add components t is up to you to browse to the folder where they reside to find them.
Of course I never think to look in the help! I did look, after I posted this question, and was coming back here to delete my question.
Thank you!
I see now I wasn't very specific in my question. I meant when opening an existing assembly. But I have my answer. Thank you!
Andy Sanders wrote:
They don't need to be in the same folder.
When you create the assembly, Solidworks remembers where all the files were stored initially.
If you open an assembly, you can use the File->Find references to see where all the parts are located on your network/folder structure.
This is why it's important not to move files around without using Solidworks Explorer. If you move parts to different folders and/or rename them, Solidworks will freak out and not know where the parts are when you open the assembly.
Then you get to have fun relocating them.
Actually, SW seems to look for its component in the same folder first
IF you have an assembly with its components in diff. folders. Try this: Copy some components in diff. folder to the same folder with the assembly and open the assembly and check the ref.
Don't. And it's surprising how many forget the first step from the sheet, "Uses any open document with the same name".
That means not just any assembly or drawing you have open, but all the files that the open ones reference. So if you have an assembly with a part named "FGH", and open another assembly or drawing that also has a part named "FGH", it will use the one that has already opened and not the FGH file that the second assembly originally uses. A LOT of people get tripped up on that. It's why file naming is so important.
Bingo. Solidworks file management can be tricky for a new user who doesn't understand how it manages everything.
You can REALLY mess up an assembly if you're not careful.
It does look in the same folder first but if you rename a file out in Windows, Solidworks will still not know what's going on even if it's in the same folder.
Kamil Wilkosz wrote:
Hi Kevin, it's not a dumb qeustion!
Let's check the info in the link. It's a search routine, step by step, how SW is looking for the referenced files:
2019 SOLIDWORKS Help - Search Routine for Referenced Documents
BR,
Kamil
Awesome! Mark Kamil Wilkosz as the correct answer!
When I'm creating new parts, I work in a folder that I created for the project. When I'm done, I move them to their destination folders. Assemblies are in one area, and parts are in another. Now I will have to do things differently. If I create my components in my project folder, I need to move them to the destination folder before I add them to my assembly!
I wondered if I learned this in class, since this seems important and it doesn't sound familiar. Then I looked in the book I got in class. There's a one-sentence explanation on page 1, with a note saying it will be discussed in a later section, but I can't find that later section.
Kevin Hansen wrote:
When I'm creating new parts, I work in a folder that I created for the project. When I'm done, I move them to their destination folders. Assemblies are in one area, and parts are in another. Now I will have to do things differently. If I create my components in my project folder, I need to move them to the destination folder before I add them to my assembly!
I wondered if I learned this in class, since this seems important and it doesn't sound familiar. Then I looked in the book I got in class. There's a one-sentence explanation on page 1, with a note saying it will be discussed in a later section, but I can't find that later section.
You can create the entire assembly in your project folder, then run a "pack and go" and move everything where you need it to go. It will update references as you go. This is what I do.
Why not just create and work on the files in the destination folder?
I certainly can do that. I prefer to keep everything related to a project (I'm talking about small projects that take me a couple of days) in the same folder, including supporting documents. When I'm finished, I can easily see what to keep and what to delete. When things are out on the network, we tend to lose sight of some things that should be deleted, and junk accumulates. Like the part I didn't end up completing and using, or a layout I did on the side. Maybe I made a subassembly and later decided to only use a top-level assembly with components. Things like that, that you tend to miss when they're in a folder with hundreds of other parts.
Andy Sanders wrote:
This is why it's important not to move files around without using Solidworks Explorer.
Hadn't heard of that. We're supposed to be getting PDM in a few months, but I was wondering what to do in the meantime. I'm glad I thought of this question before we got too far into it!
Kevin Hansen wrote:
I certainly can do that. I prefer to keep everything related to a project (I'm talking about small projects that take me a couple of days) in the same folder, including supporting documents. When I'm finished, I can easily see what to keep and what to delete. When things are out on the network, we tend to lose sight of some things that should be deleted, and junk accumulates. Like the part I didn't end up completing and using, or a layout I did on the side. Maybe I made a subassembly and later decided to only use a top-level assembly with components. Things like that, that you tend to miss when they're in a folder with hundreds of other parts.
There are options to avoid that situation. I typically have sub-folders in the project folder where I save all components related to the project. As the project evolves I Pack and Go to a new sub-folder. This allows me to keep previous versions, and also leaves behind any components that are no longer used. When the design is finalized I Pack and Go directly to the project folder and delete the sub-folders.
If you don't want to deal with sub-folders, then when the project is finalized open all Drawings and main Assemblies, Ctrl+A to select all files in the folder, and delete. All files that aren't open, or referenced by the open files, will be deleted.
Kevin Hansen wrote:
We're supposed to be getting PDM in a few months,
You will find that PDM makes life much simpler, once you have all the wrinkles ironed out and your workflow set the way you work.
John
If you are working with PDM and you have it set to not allow duplicates you may want to consider forgetting about Pack and Go.
It will create copies that can never be checked in.
That only banns duplicate names, right? It doesn't check file content. When you make a pack and go you can add prefix or suffix to all file names. Or tediously re-name every file if you really want to.
yep it looks in ram. then the folder where the assembly is, and then where the files were last saved. That is unless you have set search paths. Then there are endless possibilities depending on how general or specific they are, and where you have files saved.
Search paths? *runs off to look it up*
OK, that's interesting. If we weren't going to PDM in a few months, I'd be all over that. As it is, I think I'm just going to make one single folder to store all models in.
Yeaaaah... That might not work for a networked PDM. We've found that any file folder that has over 1000 files in it starts taking awhile to load. We're talking +20 seconds just to see what files are in a folder.
What's a networked PDM? When the PDM system is looking at the files on a regular network? And is there another kind?
What I mean by networked PDM is just a PDM that has information on multiple machines and even servers that are hundreds of miles apart, as opposed to a PDM that is only on one network drive, and people are re-loading from that one machine over a LAN to their own machines.
I'm pretty sure our vault is going to be on its own server.
Hi Kevin, it's not a dumb qeustion!
Let's check the info in the link. It's a search routine, step by step, how SW is looking for the referenced files:
2019 SOLIDWORKS Help - Search Routine for Referenced Documents
BR,
Kamil