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Four Users Referencing the Same File 1
- Thread starter ryno23
- Start date
Tools->Options->System Options->Collaboration
Jeff Mirisola, CSWP
Certified DriveWorks AE
Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M
Jeff Mirisola, CSWP
Certified DriveWorks AE
Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M
- Thread starter
- #4
-
1
- #5
Tools --> Options --> System Options --> External references --> Open referenced documents with read-only access
Use File --> Reload to gain write access to files on an as-needed basis.
You can also make files and folders read-only using Windows security settings.
Use File --> Reload to gain write access to files on an as-needed basis.
You can also make files and folders read-only using Windows security settings.
Enable multi-user environment. Select 'Check if files...'
Jeff Mirisola, CSWP
Certified DriveWorks AE
Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M
Jeff Mirisola, CSWP
Certified DriveWorks AE
Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M
- Thread starter
- #7
Thanks for all the help. Im still not sure if I am getting what I am looking for. The 4 of us all need to use the part in our designs and reference the Master part. Will Tools->Options->System Options->Collaboration fix this for me. Sorry guys for the ignorance, I am new to Solidworks.
CorBlimeyLimey
Mechanical
The Collaboration options just helps control who has current write access.
If the four of you will not be editing the part, the document can be set to Read Only and all of you can simultaneously use the part as a Master part by inserting it into a part or assy.
Another method is to use a skeleton or layout which has been derived from the part, and insert that (as the Master for reference) into another part or assy. Using this method the actual master part cannot be accidentally changed.
![[cheers]](/data/assets/smilies/cheers.gif "[cheers] [cheers]")
If the four of you will not be editing the part, the document can be set to Read Only and all of you can simultaneously use the part as a Master part by inserting it into a part or assy.
Another method is to use a skeleton or layout which has been derived from the part, and insert that (as the Master for reference) into another part or assy. Using this method the actual master part cannot be accidentally changed.
There are two main ways of sharing files in SolidWorks.
The first is having the files in a network share and inserting them from their network location. The collaboration options are there to help manage files in this sort of setting.
The second way is through file management systems like PDMWorks Workgroup and PDMWorks Enterprise. With the file management system the master copy of the files reside in a central location (vault), and the software handles copying the files from the vault to your local drive. They also provide mechanisms for revision control, where you can access older versions of the file.
It is possible to have a mixture of the two methods. We have it set up where our library / toolbox files (screws, nuts, etc.) are on a network share, and our product files are in the vault.
Using a common network location is essentially free, and requires little setup. However, it requires discipline on the part of the users and fairly good communication between the users. Historically working with files over the network has been considered a potential source of crashes.
Depending on the flavor of SolidWorks that you purchased, you may already have PDMWorks, otherwise there will be added software costs. PDMWorks requires more setup, but it enforces some of the rules like only one person can have a file checked out for changes at a time. It also can maintain a history of files, making it particularly useful for a product with long development and or life, where revision tracking becomes important.
What will work best depends a lot on your users, the product you make and your company’s culture and practices. Your VAR should be a good source for advice about which method to use and help in getting it set up.
Eric
The first is having the files in a network share and inserting them from their network location. The collaboration options are there to help manage files in this sort of setting.
The second way is through file management systems like PDMWorks Workgroup and PDMWorks Enterprise. With the file management system the master copy of the files reside in a central location (vault), and the software handles copying the files from the vault to your local drive. They also provide mechanisms for revision control, where you can access older versions of the file.
It is possible to have a mixture of the two methods. We have it set up where our library / toolbox files (screws, nuts, etc.) are on a network share, and our product files are in the vault.
Using a common network location is essentially free, and requires little setup. However, it requires discipline on the part of the users and fairly good communication between the users. Historically working with files over the network has been considered a potential source of crashes.
Depending on the flavor of SolidWorks that you purchased, you may already have PDMWorks, otherwise there will be added software costs. PDMWorks requires more setup, but it enforces some of the rules like only one person can have a file checked out for changes at a time. It also can maintain a history of files, making it particularly useful for a product with long development and or life, where revision tracking becomes important.
What will work best depends a lot on your users, the product you make and your company’s culture and practices. Your VAR should be a good source for advice about which method to use and help in getting it set up.
Eric
- Thread starter
- #11
Well, we are just getting ready to kick these jobs off, and I would like to have some idea what the best way to share this one Master file. I know in other softwares,(UG and V5) it is pretty easy to do this. I'm sure Solidworks is relatively easy as well, I just got to find it. Thanks
The bottom line is that write access needs to be controlled. That's what the collaboration options do.
My previous tip about opening references read-only is a project-saver. You want users to be deliberate about which files they change, and not save "accidental" changes.
Also, learn about search paths and how SW looks for components. Get in the habit of checking where compponents are loaded from ("File --> Find references"). Too many users are oblivious as to how SW selects a particular file or folder from which to load a component.
Team discipline is essential, whether you have PDM or not. Don't waste time or money employing team members who aren't team players.
My previous tip about opening references read-only is a project-saver. You want users to be deliberate about which files they change, and not save "accidental" changes.
Also, learn about search paths and how SW looks for components. Get in the habit of checking where compponents are loaded from ("File --> Find references"). Too many users are oblivious as to how SW selects a particular file or folder from which to load a component.
Team discipline is essential, whether you have PDM or not. Don't waste time or money employing team members who aren't team players.
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