CAD Forum

Greeting everyone,
I have a Fastening library modelled by myself and it's made using a multi-configuration part. Every configuration is grouped in different Metric sizes and lengths.
This way, when I create an assembly and I want to know whi size of faastener fits, i can easily and very quickly change betwen configurations. When I save the assembly, if I have the same scew with different sizes, it saves them as different configurations of the same part in the assembly.
I shouldn't have any problem, but sometimes when i open the assembly after weeks, instead of loading the right configuration it loads a default and random one for all screws. So all screws are the same size and lenght even tho I saved the assembly and its components with the scpecific configurations that fit.

I don't know if anyone has had this issue but i cant seem to resolve it, I don't even know where to start tracking what possible issue could be. When i load the screw and i force reload to all configurations, they all reload fine and no issues at all, i go back to the assembly and the screws keep at ex. M5x55 mm in spots where only an M3 would fit.

I attatched a screenshot of the part with the multiple configurations displayed on the left. In case it helps understand what type of file i am using.

I hope I explained the problm accurately and it's understandable. Any further questions I'll be delighted to answer them.
Thanks.

This happens to toolbox frequently. It's not really a bug, it's kind of a feature designed into the system. It happens to toolbox when a new user who only has the default toolbox parts and hasn't built all the configurations opens an assembly and saves it. If you have multiple users and multiple versions of your library, this same thing could be happening to you.

Configurations is not a great technique for large libraries. It gets huge, and it causes a lot of crashes.

Welcome to the forum. Is that a Toolbox part? Since you said you modeled it I suspect it isn't. Assuming I'm correct, the problem may lie with the derived configurations. Configurations are extraordinarily useful, but it is possible to have them be too complex.

You might want to consider breaking that down to a distinct Part for each bolt size, with configurations for lengths. I've been doing that for around 15 years, and it's worked very well. Since they all started out as a single Part, when you do need to switch sides using the Replace Components function should work well (assigning the mates to the new Part should go smoothly).

Glenn Schroeder wrote: ↑Thu Apr 18, 2024 1:53 pm You might want to consider breaking that down to a distinct Part for each bolt size, with configurations for lengths. I've been doing that for around 15 years, and it's worked very well. Since they all started out as a single Part, when you do need to switch sides using the Replace Components function should work well (assigning the mates to the new Part should go smoothly).

That is exactly what I do as well. File for each part and configs for the lengths. If you need a different size of screw/bolt use replace part, just make sure they are all made in the same orientation.

Glenn Schroeder wrote: ↑Thu Apr 18, 2024 1:53 pm Welcome to the forum. Is that a Toolbox part? Since you said you modeled it I suspect it isn't. Assuming I'm correct, the problem may lie with the derived configurations. Configurations are extraordinarily useful, but it is possible to have them be too complex.

You might want to consider breaking that down to a distinct Part for each bolt size, with configurations for lengths. I've been doing that for around 15 years, and it's worked very well. Since they all started out as a single Part, when you do need to switch sides using the Replace Components function should work well (assigning the mates to the new Part should go smoothly).

Thank you so much for all the answers.
I'll give it a try to separate different sizes into different files and i'll update you on if it still happens. But i'd like to know how the process of changing sizes works in an assembly. When you change the size, thus changing the part file, does the changed part adopt the mate references from the previous size, or do you have to re-assign the mates?

In case anyone was having any doubts, this has nothing to do with ToolBox, in the sense that i don't use it. I don't know if maybe it's SolidWorks itself that just doesn't know how to manage these type of files but i'll give Glenn's solution a try.

Galletas wrote: ↑Fri Apr 19, 2024 5:36 am Thank you so much for all the answers.
I'll give it a try to separate different sizes into different files and i'll update you on if it still happens. But i'd like to know how the process of changing sizes works in an assembly. When you change the size, thus changing the part file, does the changed part adopt the mate references from the previous size, or do you have to re-assign the mates?

In case anyone was having any doubts, this has nothing to do with ToolBox, in the sense that i don't use it. I don't know if maybe it's SolidWorks itself that just doesn't know how to manage these type of files but i'll give Glenn's solution a try.

It shouldn't be too hard or long to do either as you already have all the configurations created, all you need is to create the files for each sizes and then in each files you remove the configurations that do not go with the size of the part.

I've never really seen this though to be honest and we use a lot of design tables to create parts with different lengths.

Galletas wrote: ↑Fri Apr 19, 2024 5:36 am Thank you so much for all the answers.
I'll give it a try to separate different sizes into different files and i'll update you on if it still happens. But i'd like to know how the process of changing sizes works in an assembly. When you change the size, thus changing the part file, does the changed part adopt the mate references from the previous size, or do you have to re-assign the mates?

In case anyone was having any doubts, this has nothing to do with ToolBox, in the sense that i don't use it. I don't know if maybe it's SolidWorks itself that just doesn't know how to manage these type of files but i'll give Glenn's solution a try.

The software will try to apply the Mates to the new component, with varying degrees of success, of course. Since your Parts will be very similar because of having once been all one Part, I expect it to work very well.

I think that with multiple configurations you should be careful to force rebuild all configurations and then save your hardware file.

if you switch to the configuration pane, a list of configurations and their graphic data status with "-" or "✓" is shown. the latter is when you properly rebuild the configuration and create its graphical representation. when you change configuration in the assy the configuration marked with "-" has no graphic data and it should compute it at that time, but probably it goes nuts and it shows some other random data in the file.
my educated guess.

I have seen this in assemblies with multiple configurations when the part is patterned. Sometimes instances will change to some random config.

Another thing that causes issues is the "Cofigure Part" dialog. Use this at your peril, I have found this to be very flakey and does not seem to work as well or in the same way as configuring parts individually. I think this may have to do with having derived configurations (which others have mentioned as a possible issue) because the times I have had issues with "Configure Part" have been in assemblies with derived configurations.

imaca101 wrote: ↑Sun Sep 22, 2024 9:24 pm
Another thing that causes issues is the "Cofigure Part" dialog. Use this at your peril.

I never had any issues with this feature prior to 2022, but in 2022 and 2023, sometimes the changes stick, and sometimes they don't.