Opening a file - it sounds really simple. And it is really simple when opening simple Word or Excel files that don't have any links to external files.
But in SOLIDWORKS it is not always that simple. When opening SOLIDWORKS part files, those part files usually don't have any references to any external files (unless they are derived parts). But when opening assemblies and drawings, they are normally referencing some part and sub-assembly files. Those reference files need to be found. Otherwise those assemblies or drawings are opened without those files and they are displayed as empty.
Most SOLIDWORKS users have seen these messages when opening assemblies or drawings. If you want to know more about the reasons for these messages, please continue reading...
Where SOLIDWORKS is looking for referenced documents?
There is a specific order that SOLIDWORKS uses to find referenced documents. This so called "search routine" has been described shortly in THIS HELP ARTICLE. Let's still try to give more insight about this search routine. In this article we are concentrating on the main search rules
Let's imagine that you are opening an assembly named Cylinder.SLDASM and that assembly contains part named Piston.SLDPRT.
SEARCH RULE 1 - Any file with same name opened
Let's imagine that part Piston.SLDPRT is located in the same folder with the file Cylinder.SLDASM. But there are also other variations of this cylinder with different cylinder and piston sizes. If you already have a part named Piston.SLDPRT opened from some other folder in SOLIDWORKS before opening the assembly, SOLIDWORKS will use that already opened file as a reference. It does not matter if this file is the one that you have used initially in this assembly. It can be completely a different part belonging to a whole different project. In the example picture below there is a file Piston.SLDPRT opened from folder "Cylinder L=800 - DIAM 200" before opening assembly Cylinder.SLDASM from folder "Cylinder L=300 - DIAM 100". Assembly will use the incorrect piston file from incorrect folder. It can be clearly seen that piston is too large for the cylinder pipe.
In this context it is good to remind that all SOLIDWORKS file names should always be unique to avoid the issues with references being replaced unintentionally.
Always avoid using duplicated file names!
Instead, always use unique file names! That will eliminate the possibility of unintentional change of references.
SEARCH RULE 2 - Folders defined in "File Locations > Referenced Documents"
If SOLIDWORKS does not find the reference from opened documents, it will use the next search rule: folders defined in SOLIDWORKS settings in Tools > Options > System Options > File Locations > Referenced Documents. If folder(s) defined in "Referenced Documents" contains a file with same name, SOLIDWORKS uses that file as a reference. If there are multiple folders defined and they all contain a file with same SOLIDWORKS searches for reference from top to bottom of the list of defined folders.
Let's imagine that file named Piston.SLDPRT exists in all of three folders "Folder 1", "Folder 2" and "Folder 3". All of these folders have been added to list of "Referenced Documents".
When Cylinder.SLDASM is opened, SOLIDWORKS takes the reference file Piston.SLDPRT from folder "Folder 1" because this folder is the topmost folder in the "Referenced Documents" list. Order of the folders can be rearranged by using "Move Up" and "Mode Down" buttons.
Note: Option named Tools > Options > System Options > External References > "Reference Documents specified in File Location" needs to be enabled when using "Referenced Documents" folders as a search rule.
TIP! Using of "Referenced Documents" folders is really useful when changing the location of SOLIDWORKS files, for example from one server to another server. By adding new folder location(s) to list of "Referenced Documents" it is easy to tell SOLIDWORKS to use files from new location.
Please be careful with using the option "Include sub-folders". It is recommended to use this option only temporarily because it might cause slow opening of assemblies and drawings when added "Referenced Documents" folders contain a huge amount of sub-folders and files. After you have used this option and managed to open file with correct referenced files and saved the file, please disable this option.
SEARCH RULE 3 - File with same name exists in same folder
If SOLIDWORKS does not succeed with finding reference file by search rules 1 and 2 it will use search rule 3. If reference file with same name exists in the same folder with opened assembly or drawing (or part if it's derived part), that file is used as reference.
Let's imagine that there is an assembly Cylinder.SLDASM in folder "Cylinder Project". That assembly has been saved with parts Cylinder Pipe.SLDPRT and Piston.SLDPRT" being in sub-folder called "Parts".
If, for some reason, those part files would be located in the same folder (folder "Cylinder Project") with the assembly...
...then assembly would find those parts in that folder "Cylinder Project" instead of folder "Parts" even though the parts were there when the assembly was last saved.
SEARCH RULES 4-8
If SOLIDWORKS still hasn't found the referenced documents after performing previously described search rules 1-3, then it proceeds to next rules 4, 5, 6, 7 and 8. These rules are listed HERE.
The last rule that SOLIDWORKS uses is rule 8 where SOLIDWORKS finally gives user a possibility to show where the missing component is located or suppress the component.
If missing component cannot be found anywhere, then that component remains missing and it gets suppressed from the assembly.
FINAL CONCLUSION
Hopefully the text above has given you useful information and has introduced new ways how to handle SOLIDWORKS file references. At least it has proven that the way how SOLIDWORKS handles file references is a bit complex and not something that you have been familiar with when working with simple Microsoft Word files, for example. File reference management is always much easier when there is a PDM software used together with SOLIDWORKS. PLM Group has three different PDM solutions: SOLIDWORKS PDM, Cloud PDM and HostPLM. Users who feel that they are not in need of PDM system might also benefit from CUSTOMTOOLS software. You can always contact PLM Group Support if you have any technical questions. You can also contact PLM Group sales if you are interested in any of the solutions that we provide.
For your reference
Niklas Johansson
Technical Specialist, PLM Group Finland
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