Toolbox Help

Hi

When using the toolbox drag and drop feature, once you have selected the correct size and legnth etc, a new configuration is created within the original screw part. within the properties of this configuration there is a "bill of materials option" where 'User specified name' is selected and a description is shown, for example; 'ISO 4762 M6 x 16 --- 16N'

Does anybody know where solidworks references, 'ISO 4762 M6 x 16 --- 16N' when it creates the new configuration, whether its a .txt file saved somewhere or a property within the part i can't find, or a toolbox property

Im looking to change 'ISO 4762 M6 x 16 --- 16N' , to 'CAPSCREW M6 x 16 --- 16N', so that when a table is greated ina  drawing of the screws that appears as the part number/description

Hopefully I have explained myself clearly, if not i will clarify

Cheers

SolidworksConfigurations design Tables
Answers 7
DG
DG 2009-08-25 Best Answer
  1. Tools, Options.

  2. On the System Options tab, click Hole Wizard/Toolbox

You can see the location of your Tool box.

SF
SF 2009-08-25

YES THANK YOU, i AM AWARE OF THIS AND NOW CURRENTLY ATTEMPTING TO EDIT MY BROWSER.MDB FILE

oops caps!

Cheers for the speedy response

SF
SF 2009-08-25

Just an upate to anybody else who is intersted in this, it seems to work, but will test it soon to see if it breaks old assemblies

SF
SF 2009-08-25
Got it working, so now have BOMS on drawings only callING up the screws and have a correct description in the from of ' BUTTON HEAD SCREW - M12 x 16', etc
DG
DG 2009-08-26

Thanks for the update Chris.

Can you put down some write on this as how to edit the toolbox mdb file.

SF
SF 2009-08-26

Okay as per requested: I'll basically describe what I did and why.

Reason:

To create a BOM in a drawing which only lists screws added to the assembly via toolbox.

Method:

To do this create a new configuration within the assembly suppressing everything but the screws, then on the drawning add a BOM of that configuration. Job Done!

2nd Reason:

However the screw descriptions which appear  in the table are as such 'ISO 4017 M16 x 18 --- 20N', which means nothing to our fitters who want to see; CAPSCREW M8 x 12' or 'BUTTON HEAD SCREW M6 X 14' etc

Method:

In solidoworks go to Tools>Options>HoleWizard/Toolbox a find the file path you are using, then go to this file directory usually called 'Solidworks data' then go to Solidworks data>Lang>English>SWBrowser.mdb , I recommend making an original copy first! This must be opened with Microsoft Access or similar.

Once opened search through the list of databases until you find the ones you wish to edit, for instance we use ISO standard so I have only changed these files.

Example: ISO_CFG_BS_SHSSCREW7379 , where ISO is the standard, CFG stands for configuration, BS is bolts and screws, SHS is socket head shoulder.


It is these CFG files whch need editting, open one up and you will see a table of lots of information, under the column heading Grid_item_Name go to row 'Configuration Name', now go accross to the column ValueList, this is the text to edit. Hopefully you can see where the text and values come from and know what description you want. Edit close and repeat for another part. Save this file in SoldiworksData>Lang>English>SWBrowser.mdb . now when using screws it will give them your preferred part name/description.

WARNING!!!!! : For where I work, this would have broke old assemblies and created a file path error, to over come this weve started using a new TOOLBOX directory, so that all new assemblies with screws use the new one with new configuration names, and all old assemblies still pull screws from the old directory, for instance our old one is called 'Solidworks data', and our new one is Solidworks 2009 Data'.

DISCLAIMER: Editting the .mdb file is at your own risk, this is merely a guide of what i did, not a comprehensive how to.

DG
DG 2009-08-26

Great one Chris.

And one who want to try this, do make sure you keep a copy of the files and specially the toolbox mdb file.