Screwy Screws

[SoledWorker]

I opened a file today (that was fine yesterday) and got a message that the screws can't be found, it's substituted "the last known configuration", which are huge screws, far bigger than some of the parts they go thru. Any ideas on what this is and how to fix it?

 

[SnowCrash]

You have just been screwed. hehehehe

Or not.

Anyway, get to the properties for each of your components. I think you will find that the selected configuration option is "last used". Change that to the specific instance you want.

Crashj 'unscrewed now?' Johnson

 

[SoledWorker]

For every fastener in every model? "Smartfasteners" is quite the misnomer.

It seems like the program doesn't know where to find the screws - it has substituted inch screws in some cases (we do metric), in other places what should be M4 has been replaced with M20! There has to be an easier way...

 

[drawoh]

SoiledWorker,

Are you using the SolidWorks toolbox?

My experince with this is that the intelligence it attaches to each fastener only works on the machine that was used to attach the fastener. If you switch computers, it behaves very much the way you are describing.

I prefer to create my own fastener models, which have all the configurations I want, and BOM entries that conform to company policies.

JHG

 

[SoledWorker]

I used "smartfasteners", which pulls from the toolbox. I think that this is housed on our server.

 

[SBaugh]

Toolbox uses a Database file located in your SW directory. It is possible that file got corrupted. I'll bet you don't have a back up of it anywhere, do you?

The file is Default.mdb located under data which is under the solidworks directory. As far as I know there isn't away of getting it back because all configs are stored in that. So if you upgrade it is wise to back that file up for future reference.

If you don't use a lot of screws in your models you may want to consider making your own. You can use the bolts for toolbox but when you save them, save to a or the same file directory as your assembly. (via JHG suggestion) Scott Baugh, CSWP
3DVision Technologies
credence69@REMOVEhotmail.com

http://www.3dvisiontech.com

http://www.3dmca.com

*When in doubt always check the help*

 

[manxJim]

If you go to The Toolbox Menu select Browser Configuration then select Document Properties. Select always create copy then go to the browser button and find the Toolbox in the toolbox there is a folder Copied Parts select this folder
Now when you get a part from the Toolbox it will create a copy in this folder so next time you open you assembly it will look in the copied part directory and open the right part. If your files are on a sever the put a copy of the Toolbox on the sever and have the browser point to that Toolbox Then you will be able to open the assembly on any machine
Hope this helps