How do toolbox parts determine by solidworks ?

[SWscience]

You know that toolbox parts have internal flag and then determined by solidworks or other its modules such as pdmworks. Its enough to check in a toolbox part to check this action and you will see a toolbox icon near the part you have checked in.
Now I need to know what's that flag and if it's possible to convert a toolbox part to a usuall part and vice versa.
And the second questin is :
If you open a toolbox part directly from toolbox folder you won't see any configuratons , but if you open that part from toolbox panel in an assembly and select a configurtion from dialog box that config will add to part and next time you open that toolbox part, you will see the configuration you used before.
How does it work ?
I need to know this function to use on non-toolbox parts
Best regards.

 

[SWscience]

How do toolbox parts *determined by solidworks ?
Sorry , I don't know if it's possible to edit a post !

 

[DesignSmith]

Toolbox parts in 2004 and 2005 are read-only, and the library toggles the flag just long enough to dynamically create the configuration you select and resave the file. This is done to better allow for multiple users working in different assemblies with the same fasteners, without the need for duplicate items everywhere.

It also creates new configurations on the fly, from size and type information contained in a large multi-relational database. That is how it can provide over 10 million possible items from just 1000 actual part files. (Socket Head Cap Screw alone, offers 32,000 possible combinations) Your installation of the library only contains the standard, size, length, and feature options that you have selected to use so far. Thus you can create any subset of the 10 million hardware items, without tying up the system and network resources to store that many.

You can approximate some of the Toolbox behavior with Design Table driven configurations and part equations, but you will not be able to get the same depth of choices.

You can customize Toolbox hardware to a fair extent by going to Tools-Options-Data Options-[Edit Standards Data] and start making standards or dimensional changes in the database. You can put copies of some of the items in your Design Library (Feature Palette) and then edit them to make something new, but editing the source files directly will likely prevent multi-user access and could possibly result in size configurations that will not rebuild correctly.

To really customize the Toolbox library itself get help from a VAR AE or independent CSWP.

FYI,

DesignSmith

http://www.DesignSmith-Services.com

 

[cninneman]

I do not know of any way to duplicate how solidworks creates the configurations of toolbox parts. As DesignSmith said, there are tables, for the toolbox parts, that can be edited, however there are quite a few quirky bugs in the software at this time. I have had my VAR submit the bugs that I have found, and hope to see them fixed in SP1.

So, depending on how heavily you decide to modify the standards database, don't be suprised if some things don't work they way you think they should.

The big one for me was adding parts to the tables. It does not create a configuration name specific for each new part, it gives them all the same name, and there is no way to change it.

Chris

 

[SBaugh]

No offense cninneman, but I doubt you will see your problems fixed in SP1.0, unless they are total show stoppers, not workaround, total meltdown issues. Even some of those types of issues might not make it until SP2 or 3. So bank on SW fixing your bugs by SP1

As for your big one - you can't go to the part itself and manully change it?

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[SBaugh]

Forgot a word:

"So DON'T bank on SW fixing your bugs by SP1.0"

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[cninneman]

Believe me, I know it's wishfull thinking, but it's not like I have anything else to loose by being optomistic about it.

As for your suggestion, it doesn't work. The configuration name does not populate back to the standards table. I've tried everything I can think of to make it work. There are just a lot of little annoying bugs in the toolbox software. It's just fine and dandy if you use it as packaged, but if you start customizing...beware.

 

[DesignSmith]

cninneman,

You can create a derivative part in a new Toolbox standard; (such as Low Head Socket Cap Screw in MyOwnANSI) but otherwise, the customize data process is not designed to allow addition of totally new items (like wave springs) that the relational database has not been previously set up for.
You can set up alternate file names under Toolbox-Browser Configuration... - [Browser] Document Properties - File Names, and turn Countersunk Elevator Bolt.sldprt into Locking Head Bolt.sldprt for instance. But the default configuration names of the individual sizes are controlled by hidden tables in the relational database. You may manually type over them at the time of drag & drop and it will keep that name, but it must be absolutely unique. (you may need to scroll down in the size selection dialog to see the configuation name and its edit box)
Putting your own default configuration names in requires editing the database outside of the SolidWorks interface, which is non-supported. (sorry, but I charge real money for this level of library customization)

If you are intent on this level of library manipulation, it might be best to take it off-line or open a new thread. We are straying far from the original question of Toolbox part file attributes or determination.

FYI,


DesignSmith

http://www.DesignSmith-Services.com

 

[cninneman]

DS

Yes I know exactly what you are refering to. I have created my own standard, and within that standard I have disabled the parts that I do not need, as well as setup custom properties in the browser configuration, so that I can create "duplicate part numbers for geometrically equal components".

I am working with 2005, it sounds more like you are refering to 2004. 2005 allows many more options with customizing the toolbox part tables, but as I said, there are a lot of bugs that keep them from working as expected. Trust me, I've been working very hard with this, to make it work for our company. I have pretty well used up all the recources of my VAR and have taught them a couple of things in the process. If you know how to make it work, as it should (read: I'm not paying anything more for this), I'm all ears. I think the new 2005 Toolbox is a huge and awesome tool, it's just too bad it's so buggy.

If you would like to open a new thread to discuss this more, that would be just fine with me. More people than just me, need to know about these bugs, so that they'll get fixed. According to my VAR I'm the only one so far, in thier group, that has tried to work the toolbox this hard.

Later
Chris

 

[DesignSmith]

cninneman,

In 2005, extra functionality was added to the [Edit Standards Data] utility that allows you generate tables of all the configurations for a particular fastener, and manually prepopulate the Part Number and Descriptions with your company values. (this prevents errors by not getting the values right during the initial drag & drop of a specific fastener)
However, I don't expect that it will allow you to replace the default configuration names when you import the edited tables back in. The SW interface does not let you do anything (such as over-ride configuration names) that might cause the library or its database to stop operating at the next SW session.
Hidden tables within the database have special variable strings that generate the default configuration names, and insure uniqueness of all 10 million + file and configuration name combinations.

Rather than opening up the database and risking damage to the control tables, you might look to see if using the Feature Tree Display options will give you the effect that you want. You can change the Tree Display to show Configuration Descriptions rather than the Configuration Names and manually set the configuration descriptions to whatever you want without fear of conflict with any of the Toolbox library defaults.

The basic question would be: What are trying to accomplish by substituting your own configuration names? If you are trying to simplify the Feature Tree listings of assemblies, the above suggestion could work. If you are tying to get a specific display for BOM or other types of reporting, there may be a better option than configuration names. If there is a specific application reason for your own configuration names it can be done, but only by directly editing the database itself. At which point you are on own for support, and thus you need to consider if it is worth it.

FYI,

DesignSmith

http://www.DesignSmith-Services.com

 

[cninneman]

DS

I have no desire to replace or rename the default configurations, and yes I've already tried the "export - change the config. names - import" and you're correct, that does not work. All I want to do, is simply add parts to the tables that are there, which is something I'm supposed to be able to do.

Once a derived standard has been created, you have the option to manipulate the sizes and such, in the part tables provided. If you look closely, at the bottom of the "Size" tab/table, you can add a new "size/configuration". This is where things get buggy, in the Size column, if you type in something other than what seem to be in a hidden list of predetermined sizes, your new fastener will be created with some sort of default configuration name. Now if you happen to type in a value that is one of the predetermined sizes (which, best I can tell, seem to be in incriments of 1/16"), your new fastener will be given a configuration name that is unique and usable. Go into one of the washer files and play with it for a while, you'll see what I mean. We use a lot of washers that are in 1/32" increments and this is where I'm having a problem. Yes I could probably just fake it, and give a part number to a wrong size washer, but I shouldn't have to.

This, like I said, is just one of the few bugs I have found in the toolbox software. The deeper I get, the more I find.

Later
Chris

 

[DesignSmith]

Chris,

OK, it took a little while but I verified that you are right with configuration name problem. You might check with your VAR if they can get it listed as a Regression SPR. (worked in 2004, now broken in 2005) That will raise the priority a bit.
I suspect that the database structure has changed with Part Number and Description output function being added and one of the internal linking tables is damaged or missing.
Unfortunately, the machine I am running 2005 with is not the same that I have database editing tools on, and thus I can't yet determine if manually editing the database could get around the problem until the SPR fix comes out in the next service pack or 2.

If you have 3-5 similar problems with the customization, let me know off-line, and I will look at the set to determine if anything can be done to manually fix them inside the database. (it may take several days for me to get the time to test it out)

Regards,

DesignSmith

http://www.DesignSmith-Services.com

 

[cninneman]

I don't see anyway of sending you a personal message, how do I contact you off-line?

 

[SBaugh]

Click on his website below his name and send him and email.

regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users