I'm a BST CRSA teacher, and when you make a design under a PC and you place Toolbox elements (screws, bearings, keys,...) and you open the design from another PC, the configuration of the screws becomes anything (huge screws...). I even tried to rename the screws and store them in a screws folder associated with the design, and when you reopen the CAD file, it goes back to look for the screws in Toolbox losing the names we had given to the screws and the screws become huge. I don't understand where it comes from and what can be done to fix this Pb.
If the PCs are networked, it would be better if all PCs point to the same settings files in tools > options > file location and toolbox. Thus, there is little chance that the problem will recur.
The problem is simple: each PC has its own toolbox.
When you insert a toolbox component into an assembly on a computer, automatically the configuration of the component is created, if you open the assembly from another computer it will try to fetch the part from that computer and not from the first one, the size does not exist Solidworks will choose the default one.
The solution is to have a common toolbox, for this you just have to copy/paste the solidworks data folder of one of the stations and paste it to a network location accessible by all the workstations, then all you have to do is point all the toolboxes to the same place by going to tools, option, assisting for drilling/ toolbox.
Indeed, this is one of the big flaws of ToolBox, it will look for the standard parts in a folder on the first workstation in question (in general, C:/SolidWorks Data).
But if the folders (especially their contents) are not identical from one workstation to another, he will put default elements that he finds (for example a huge screw).
It should be noted that each time a new version of SolidWorks is installed, it offers to use the old SolidWorks Data, otherwise it creates a new default SolidWorks Data folder (1) with a hint in parenthesis that will be taken automatically.
A first solution is to have the same SolidWorks Data file on all the workstations and that the ToolBox points to the same file (Options/Wizard for drilling -> you can see which file SW points to to look for the ToolBox, if the option is checked)
The 2nd solution is to network all the workstations and to have only one ToolBox managed by a single administrator.
The 3rd solution (the one I use) is to unlink the element from the ToolBox by saving it in its working folder (for example, place the screw in the assembly so that it is properly configured. Then save it by doing "Copy As" with another name in its working folder. Erase the ToolBox screw and put in the one you just saved.
How do you explain that despite the fact that once the screw is configured, we save a copy of said screw in a screw folder associated with my assembly for example, and when I open my assembly again, it goes to look for the screw again in ToolBox??? That's the Pb, I think there may be a solution to break this link.
Alain.erp offers me this:
Unlink the item from the ToolBox by saving it to its working folder (for example, place the screw in the assembly so that it is properly configured. Then save it by doing "Copy As" with another name in its working folder. Erase the ToolBox screw and put in the one you just saved.
That's what I do, but yet it will look for the screw in toolbox again when I reopen despite the fact that I have implanted the renamed screw stored in a specific folder associated with the assembly.
As Franck points out, if you don't use the same toolbox folder and the configuration that was used doesn't exist in the second PC, then SolidWorks takes the default size.
The ideal solution is for all users to use the same SolidWorks Data folder... But this is possible if you are on the same network.
The other solution is to have all the sizes of the toolbox components usually used, so that solidworks can use the right part configuration...
To generate all the configurations, you have to go to the toolbox configuration tool... See screenshot.
This tool can be started through the start menu or from the solidworks options. The problem is that it can take a long time...
I do the same to be quiet (dragged from the toolbox to an ASM, then sldsetdocprop.exe) and good idea because it has already caused us modification problems if Solid is connected to Smarteam (modification not taken into account)
I still make the toolbox available in the same way to everyone and locally on each workstation because sharing it on a server has already caused me access problems if several users go to it at the same time
See my screenshot in my previous answer.
Otherwise we also have libraries, we rarely work with the toolbox:
- because Pro license = €
- More convenient to use
- avoid all of the above problems
- used only for specific component needs without being able to wait for a library administrator to do the Job