I have a few projects on my local workstation and I would like to move them
to the server. what is the best way to move the files so that I don't create
I have all the files for one project in one folder. can I just cut and past
to the directory on the server?
This is a big problem for alot of companies, especially if you have
multiple users working on the same project.
Many companies use a PDM system for this and other tasks.
There is a way to do it easier without a PDM system. You could use
SolidWorks Explorer also. I did a quick search on the SolidWorks Sub
site but could not find the reference up there. I have it all in a word
document if you or anyone else is interested.
Let me know and I can email it to you.
Nathan Feculak wrote:
Here's something that might help. I believe that the following was copied
out of the SW help files:
When you open any parent document, the other documents that are
referenced in the parent document are loaded into memory also. In the
case of assemblies, components are loaded in memory according to the
suppression state they were in when the assembly was saved. By default,
the software searches for referenced documents in the following order:
1) The paths specified in the Folders list, if the Search file locations
for external references check box is selected.
See File Locations Options (for the Folders list) and External
References Options (for the Search file locations for external
references check box.)
2) The last path you specified to open a document.
3) The last path the system used to open a document (in the case of the
system opening a referenced document last).
4) The path where the referenced document was located when the parent
document was last saved.
5) The path where the referenced document was located when the parent
document was last saved with the original disk drive designation.
6) If a referenced file still is not found, you are given the option to
browse for it.
NOTE: All updated reference paths in the parent document are saved when
you save the parent document.
Thanks to Matt, who originally posted it back in 2001. If you think about
the above for a while, you will realize that it is really easy for the
software to find the wrong stuff if you have parts and assemblies with the
Here's another post from the same year where Ed Eaton talks about what
happens before you get to the above priorities:
So, SolidWorks has a hierarchy, which it uses to evaluate which referenced
file to use.
It goes in the following order
1) named file in memory. If a part with the correct name is already open,
it will use that one, regardless of directory structure on your hard drive,
or even if it is the appropriate file. This is why it is critical that you
never name a file simply 'flange', 'bracket', 'caster', or any other generic
name that may appear in other assemblies that you work on. The way to go is
always' left flange for hyperspace coil 6-2-01 spacely sprockets ', or a
unique part number if your company is into that sort of thing.
2) the 'in use directory'. If a part of the correct name exists in the 'in
use directory' (most of the time, the directory where your assembly
resides), SW will use that one, even if you had made explicit attempts to
point the assembly to use a part in a different directory. SW doesn't care
about good intentions.. it just cares about its internal rules regarding
file locations (tip! use this to your advantage when substituting one part
3) The specified directory for the file. Only after SW has run the prior
two checks, will it even bother to find the part in the location where you
actually specified that it would be.
Tripod Data Systems
"take the garbage out, dear"
If you look the same data up in the SW04 help, the list of 6 paths where SW
looks for referenced docs has expanded to 13, and honestly, I can't make
heads nor tails of it. At least the old list you posted was
"Jerry Steiger" wrote in news:c6u9n5$getc6$1
Read the SW help re: search directories. There is a list of the
sequence SW goes through to find referenced files.
One aspect of this is that SW searches the relative path before the
absolute path. If you copied an entire directory "project" from
"C:/project" to "D:/archive/project", and opened a drawing or assembly
from the new "D:/archive/project" location, SW will search for
components before it searches "C:/project".
You may want to run some experiments to gain trust in moving and
copying entire directory structures.
I tried to get SW to explain the process of how SW looks for files because
we had trouble with SW finding same named files all over the network. The
response was that it was complicated. When I asked how to know just where
SW actually got a file from the answer was that that information was buried
deep in the code. Neither answer was very useful.
The one thing that did come out of my discussion is that search pathes that
can be pinned down should be pinned down. In particular the Referenced
Files path should be set.
Below is the current search order as described in the online help. At first
glace it looks confusing, but closer inspection and taking a little time to
see what is described in each example, the search sequence makes sense. The
only thing that appears to be incorrectly stated is when the search actually
Note the first sentence where it says "When a referenced Document cannot be
found, SolidWorks performs a search to locate the document." The way I would
understand that is that the search routine does not kick in until a document
is not found where it was last saved at the time the document that referred
to it was saved. But I see that in the current search order below,
SolidWorks searches the last saved location in step 12. Why would it do that
if it had already determined that the referred document was not there? Could
this be a doublecheck, or does this search only apply if either the referred
document or the referring document is moved as in the example below? A few
simple tests would reveal the answer, so I did that for my own understanding
of the process. I am using SW 2004 with SP03.
In Tools, Options, Referenced Documents, I added the path to a folder on
another network drive, then in External References, I selected the option to
"Search file locations for external references". I then opened an assembly
that referred to several components, looked at the properties of one of the
components, saw the folder that it was being referenced from, closed the
assembly without saving it and closed SolidWorks. I then copied the
component part file from the current folder to the folder I added to
"Referenced Documents" using Windows Explorer. When I opened the assembly
and looked at the properties, I saw that it was now referring to the file
located in the "Referenced Documents" folder.
This would indicate to me that at least if you select the option to "Search
file locations for external references", the search criteria is always used,
even if nothing has changed in either of the files, not just if a referenced
document is not found as the online help states.
In Tools, Options, External References, I unchecked the option to "Search
file locations for external references". I closed all documents and moved
the copy of the referenced document from the "Referenced Documents" folder
to the same folder as the assembly that referred to it. When I opened the
assembly, the part file that was referred to was the one in the assembly's
This indicates that step 8 in the search was performed before step 12, since
the path of the active document (the assembly) was found before the original
path. This indicates to me that, the search criteria is ALWAYS used, even if
nothing has changed in either of the files, not just if a referenced
document is not found as the online help states.
It is unclear until closer inspection that Steps 2 thru 7 are dependent on
the Tools, Options setting for "Search file locations for external
references" and are skipped entirely if not seleted.
From SolidWorks 2004 help, reformatted for text only readablity...
Searching for Referenced Documents
When a referenced document cannot be found, SolidWorks performs a search to
locate the document. For example, this search may occur when you open a
drawing and the referenced assembly cannot be found or when you resolve a
lightweight component in an assembly and the component cannot be found.
When a referenced document is found, the software updates the path to the
referenced document in the parent document. When you save the parent
document, the updated path is saved as well.
The Rules column below describes the search routine that the software uses
to locate a missing referenced document.
The Examples column shows the paths that the software checks using the
The assembly was last saved as C:\zz\a1.sldasm. You move the assembly to
The first part in the assembly was last saved as C:\qq\p1.sldprt. You do not
move this part.
The second part in the assembly was last saved as C:\zz\yy\xx\p2.sldprt.
This part is missing either through deletion, renaming, or some other file
There are two paths in the Folders list of the File Locations Options dialog
box: D:\aa\bb\ and E:\cc\dd\
You click File, Open to open a1.sldasm in its new location.
Rules and Examples
1. Uses any open document with the same name.
If p2.sldprt is in another open document, SolidWorks uses this version of
2. Searches the first path that you specify in the Folders list in the File
Locations Options dialog box.
NOTE: You must select the Search file locations for external references
check box in the External References Options dialog box or else SolidWorks
ignores the paths that you specify.
3. Searches the path in Step 2 plus the last folder in the path where the
referenced document was last saved.
4. Searches the path in Step 2 plus the last two folders in the path where
the referenced document was last saved.
5. Repeats Step 4 until the full original path has been appended to the the
path in Step 2.
NOTE: This concept of adding one folder at a time from the full path will be
called "recursive searching" in the following steps.
6. Recursively searches the first path in the Folders list, then recursively
searches the path where the referenced document was last saved.
7. Repeats Steps 2 through 6 for the other folders in the Folders list.
8. Searches the path of the active document, then recursively searches the
path where the referenced document was last saved.
9. Searches the path where you last opened a document, then recursively
searches the path where the referenced document was last saved.
NOTE: In most cases, the path of the active document and the path where you
last opened a document are the same.
The two paths are different if you click File, Open to open one document,
then drag and drop an assembly from Windows Explorer into that document. The
path of the active document is the path from Windows Explorer and the path
where you last opened a document is the path from File, Open.
same as Step 8
10. Searches the path where the software last found a referenced document.
This is the location of p1.sldprt.
11. Searches the full path where the document was last saved without a drive
This is useful if you save a part with a UNC path such as
12. Searches the full path where the document was last saved with its
original drive designation.
13. Allows you to browse for the document yourself.
End of SolidWorks Help Exerpt.