Add custom parts to toolbox 1

[chrissyd]

I have a top assembly that I am getting ready to check-in to PDMWorks. We are just now implementing PDM, even though we have sub-asemblies that were created six months ago. Some of the hardware was found on-line and imported into Solidworks. Other hardware parts were created as a part by engineers. I have tried a couple of test check-ins on smaller sub assemblies only to find that PDM does not recognize these as tool box parts and so they become revision controlled and roll rev's. A good amount of hardware was brought in through the Solidworks toolbox but even some of that is not recognized as being a toolbox part. (Maybe because we renamed the parts to our company part numbers?) How do I get PDM to recognize these parts as being toolbox parts? I've thought about just blowing out all the hardware and starting over. But there are 17 assemblies and I don't want to go through all the work if there is an easier way. Help!!

 

[SBaugh]

YOu don't have to make it directly a TB part... just put those parts into a folder on your server some where and put that path in the standard libraries so they are not revision controlled.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[chrissyd]

We do have a folder that we keep these hardware parts. They are broken down into a dozen or so sub-folders listed by what they are (i.e., SHCS, Nut, Washer, etc.). Up until now, whenever we need a SHCS screw let's say, we browse over to these folders to insert the component into our assemblies. I wrote the path to all these folders in stardard libraries. And it still checks the hardware in as if they are just parts that need to be revision controlled. Should these folders be somewhere else, like where Solidworks resides? Is that what you mean by putting it on the server? I just started work here not too long ago and I'm not sure how Solidworks was set up or where it resides.

 

[Standing]

My heart goes out to you. We started with mismatch of screws sources. We started SolidWorks before ToolBox was released.
One for our Engineers replaced all the ¼-20 x ¾ inch screws to ¼-20 x 1 inch, about 50 of them. He had 100 mate errors. None of our screws could be replaced with any other screw without mate errors. Something had to be done.
Our fix was to start with one screw, save as copy and change the size and description. Now every screw and bolt is built off the same root model. Washers were done the same way. At the same time mate references were inserted. We also built subassemblies of washers and screws.
Bottom line: We can now replace a 10-32 x 1 inch screw with a ½-13 x 1-1/2 screw without mate errors. A lock washer will replace a flat, lock, high collar or star washer. I have tested each reference mate by inserting every screw in an assembly. This also makes it easy to check into PDM; yes we do control revisions of hardware. How we manage the system is left for another time.


Bradley

 

[EEnd]

There is a Standard Libraries tab in the PDMWorks VaultAdmin (at least in 2006). On that tab you can specify paths that correspond to directories of library (including toolbox) parts. There are also options for disabling check in of library parts. One thing that I have noticed is that even when check in is disabled, SolidWorks will still send the fasteners over. I think that is so that the vault can maintain info about which configurations are in use and such. However, there will be no revision control on the library parts, and they will show up in their own area in the vault.

Eric

 

[chrissyd]

I have already written the paths to our hardware in the standard libraries tab. After each entry I have gotten a error message that the vault is unable to see the folders. I found a way to trick it though, but it's crazy if you have a lot of assemblies to check in. I open all the hardware that is included in my assy from their folders first, then open the assemby. When I go the check in the assemby, the hardware is not revision controlled, but still shows up in the PDM tree with a library icon as opposed to a toolbox icon. So it's still not exactly what i want but I guess it's still progress.

 

[Standing]

Thank you for the Star.

Bradley

 

[gandytable]

When I first started SolidWorks, I was the only user and did similar to Bradley. I did a save as copy and changed name and dimensions as needed.

Then I worked for a company with Pro-E and they made a generic part for each main fastener catagory and used configurations (Pro-E calls them family tables) to make the different sizes of bolts, screws, washers, etc... Many parts can be made very quickly with a design table. Then instead of replace, you can go to component properties and choose the part you want. The part is switched out and all mates are retained.

What are the advantages and disadvantages of using configurations verses the save as copy method?

 

[J-C]

Advantages of configurations:
Every size in one file thus easier to manage.
Easier to swap sizes in assy.

Disadvatages of configurations:
Large file size (though probably the same as adding up several files)

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP4.0 on WinXP SP2

 

[CorBlimeyLimey]

gandytable ...The size of a file with 100 configs is far less than the size of 100 separate files ... less clutter and much easier to manage (move, copy, etc).

For screws, it is best to use a DT to control only the lengths of one diameter & type of screw.


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