Toolbox vs. Standard Parts 9

[macduff]

All,
I would like everyone's opinion on the question I'm about to ask, so here we go.

I'm wondering what is the best way to set up standard parts/hardware for our company. We use many NAS, MIL, AN fastners and would like to standize this for the end users when building an assembly/drawing BOM's and also not having conflicts with PDMWorks when chenking in & out parts and assemblies.

1) Do I use the SW Toolbox and edit all the part no.s and descriptions?

2) Do I setup separtate part files and add configurations?

3) Do I use the SW Library feature for this?

We are currently having some issues with our PDMWorks not resolving part paths to the toolbox and takes alot of time fixing the assemblies.

Our SW Toolbox is now located on our server and everyone is mapped to that drive. So if changes to this, everyone will see the new parts, right? I made a copy of the "ANSI inch" area of toolbox and started renaming the configurations and descriptions.

Also....what do think about the BOM tables in SW2004? Do I use the new SW BOM or keep using the Excel based table?

I know whatever I do, it's going to take alot of time setting up standard hardware. I'm looking to you for the right direction.

Thanks,

macduff

 

[EdDanzer]

We gave up on Tool Box long ago for some of the same reasons and more. The parts library we developed has all families of parts based off one original model. Any bolt or cap screw is interchangeable with out loosing mates. Any ball bearing is interchangeable with out loosing mates. Any nut is interchangeable with out loosing mates. Any brass fitting, or hydraulic fitting is interchangeable with out loosing mates. Any lock ring is interchangeable with out loosing mates. Any hydraulic cartridge valve is interchangeable with out loosing mates as are most components. We even have standard mating geometry named so parts can be mated by picking from the feature manager. The setting up was time consuming and more expensive initially, but can save days when doing the next size of a large assembly where a few hundred components have to be changed. Changing components without loosing mates is essential to saving development costs.
I tried to get SolidWorks to take over this type of parts library from 1997 to 1999, but they have chosen the Tool Box way. My position is had they went this route and supplied a parts library on CD it could save every implementation $10,000 to $100,000 in startup costs, plus $1,000 to $5,000 per year in file maintenance.
All of our SolidWorks files are stored on a network attached hard drive for low cost sharing.
The Excel BOM seems to be more mature, so we have been continuing to use it. I hope that the SolidWorks BOM generator is expanded to allow greater functionality and ease of modification, then it might be worth changing. We have some crashing with Excel.

 

[TWHems62]

We recently started this process also.
We have a library of parts with our descriptions and part numbers
and use the "ADD PARTS WIZARD" from the toolbox to deposit them into the toolbox.
Basically added them to the feature toolbox, then disabled the ones we choose not to use.
This is under toolbox pull down menu.

Hope this helps.
We are just starting to use this also, will try to update as we go.

Good Luck
Tim

 

[Standing]

macduff,
Back when we started Toolbox, the task was assigned to a drafter, who at the time did not assemble parts together. He used Toolbox as is out of the box. He created each part as a separate file and saved the part in a write-protected area in PDM. We all had to start using these parts. It was not until I trained him in how to put in MateReferences did he add this information. After getting into the system to far to change, the Engineers and Designers found out that we could not replace a screw of the same size at different length that we got upset.
In my humble opinion, “I would use Toolbox to create the first and only screw”. Then copy using save as and change that screw to meet the requirements of the next size. The reason for doing this is that you could replace a screw of different size and the mates would keep. If that is to much work then I would use Toolbox to create the first screw of each size #4, #6, and etc then copy and change the length and description.
I really like EdDanzer idea, to bad that SolidWorks did not listen.


Bradley

 

[SBaugh]

Have you tried using the "Edit Standards Data" in the Tools\Options\System Options\Data Options - There you can Create your own toolbox of parts.

Or

Make yourself a bunch of Library parts - FYI - Library parts don't support Configurations like Toolbox parts do.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[Standing]

Scott,
I am using SolidWorks 2003 SP 5.1. I do not see Data Options. Does this start in 2004?


Bradley

 

[SBaugh]

Yes this is new to SW04.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[coolcad]

We are implimenting PDMWorks and having the same questions about using toolbox. Toolbox parts cannot reside in the PDMWorks vault. But that is fine since these parts are almost never revised. We are leaning towards individual part files placed in the vault. We can still use Toolbox to generate new parts but disconnect them from toolbox and put them in PDMWorks as a part.

I like Toolbox because, well it's cool. However, we have seen configurations go south before. And tool box is made of of single files with tons of configurations.

Has anyone else had trouble with configurations, especially from toolbox?

I'd love to hear others post how they deal with standard parts like fasteners, especially if you are using PDMworks.

Thanks!

 

[pdybeck]

glennwi,

We have both Toolbox and PDM/Works here. I have set up all installations so that the toolbox parts that are created are copies, and therefore separate files with just the needed configuration in them. We do check in those separate copied files. I have set up folders/projects in PDM/Works for standard parts. We locate the standard parts in those folders. If users here need to insert or use a standard part in their assembly, the first place they look is in the vault. If what they need is there, great, just drop and drag into the assembly. The BOM information is already filled out. If the part is not in the vault, then they create the copy using toolbox, fill out the appropriate custom file properties, and then check into PDM/Works for all to use it. So, toolbox for us is a parts generator, and not the part database like it can be used. There used to be limitations on geometrically equal parts having different part numbers in the toolbox library, but that has somewhat been quietly fixed by SolidWorks. I would recommend to any company to use the setup we have for Toolbox and PDM/Works. Keep it simple and straightforward so everyone can easily understand and be clear on the important issues.

Pete Yodis
Harold Beck and Sons

 

[coolcad]

Pete,

Thanks! That is the way we were leaning and I'm glad others like yourself are finding success with it.

Glenn

 

[macduff]

Guys,
Thank you so much for the very valuable input. I'm learning towards what pdybeck wrote in his last thread.

This thread seemed to be very important to others as well as myself.

Have a good weekend!

Colin Fitzpatrick

 

[JNR]

Regardless of the fact that we have Tool box and SmarTeam PDM (or had - we may have let ToolBox licence lapse), we only used Toolbox to make basic library models. We took the all SW approach from there. I don't know how good TB is now, but back then the models were crude. Sketches were totally undefined - not even fixed!! Also though it used the rotated profile thread method - no helixes (good), the pitches were all arbitrary.

We also use much almost exclusively MIL/NAS/AN. In fact on internal tooling, etc. where MIL, etc. is not required we call it out and use a general note allowing equivalent commercial hardware. That really saves on library generation and size.

We did not produce the entire library in one go. We did a start batch of most commonly used. We now add to it as we need to. This seems to be more efficient for us.

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

There are only 10 types of people in the world - those who understand binary and those who don't.

 

[tstanley]

SBaugh

Are you hinting that you can create your own toolbox of parts, using the information in the Data Options, without actually purchasing the toolbox option? In other words, use that data in a design table or something?

Tom Stanley

 

[SBaugh]

Are you hinting that you can create your own toolbox of parts, using the information in the Data Options, without actually purchasing the toolbox option?

I believe you will have to have Toolbox because you have to get the DB from somewhere.

In other words, use that data in a design table or something?

No, the files are SW files with configurations but they really use an Access Database.

I have Toolbox and I know you can Edit the data options by creating your own "New Standard name". You have to create it from the existing toolbox parts. So what that does is, it copies... lets say for example "Ansi Inch". It copies all the toolbax parts of "Ansi Inch" and you can modifiy the parts from there, by adding more sizes to the DB that are not normally there. For example - A "Narrow flat washer" only goes up to 3". You have a row below that, so you can add your own sizes that are not there or maybe you have a custom size. You have the ability to add it there. Then you can insert a TB part into your assembly using your new DB plus you get all the parts you custom made to choose from in the Drop down list when inserting.

IHTH explains it better.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[tstanley]

Thanks Scott. I thought that I would ask anyway.

Tom Stanley

 

[cmm]

Toolbox users who use a "vault" system like pdybeck describes.. When you generate a part with Toolbox do you delete the extraneous configurations before you save it to your "vault"?

Perhaps this is worth another thread but here goes.. I am about to create a "vault" for myself and my fellow ME to use. We are the only ones who will use it, possibly a 3rd person in the future but I don't forsee many more than that. Is PDMworks worthwhile for this number of people? So far my philosophy regarding Solidworks has been minimalism.. to keep it simple and work only with proven features. I don't consider toolbox to be a proven feature for anything except creating good part geometry. Is PDMworks similar in that isn't quite as useful as it's intended to be?

Chris Montgomery
Mechanical Engineer

http://www.adaptivequipment.com

 

[pdybeck]

Chris,

First - You do not have to delete the extra configurations when you have the option set in Toolbox to create a copy. The reason why is because only the configuration that is specified gets created in the copied file - so there is just one config. Make sure that the option to create copies is set in the Toolbox browser configurator. Also, as a side note... When you are specifying the size of the standard part to use in the dialogue box/table there is a row for the Configuration Name. As it turns out when you have the option set to create copies, this entry becomes the filename for the newly created file. Before I discovered this I used to open a blank dummy assembly, create my toolbox copy part, close the dummy assembly, rename the newly created part in Windows Explorer, and then drag the part into the assembly I needed it in. Now I can just insert the copied part directly into the assembly and name it via the configuration row. It saves a tedious file management step. I have actually been requesting from SolidWorks for users have the save copy option checked that when they insert a part, a Save As dialogue box pops up asking where they want the file, and what its name should be. This Save As dialogue box pop up could also be toggled on or off under the Browser Configurator for Toolbox.

Regarding the second portion of your post I wholeheartedly agree that it is wise to keep things as simple as they need to be - but not too simple that your design intent is lost. I actually implemented a policy here that we do not use configurations within parts to define more than one part number. I did not want to have part and assembly files where multiple part numbers are defined. File naming and revisioning became more complicated in that scenario. This was not because SolidWorks couldn't handle it or it couldn't be done in PDM (well at least manually), but because I wanted to keep things simple for our users. I would highly recommend that you implement PDM/Works for several reasons, including the fact that it can actually simplify your job. First of all, it is proven. It has been in existence and use for well over 5 years, probably more like 8 or so but don't quote me on that. Many companies use it and have been very successful with it. Some of the ideas may take a little while to get used to, but once you understand the basic workings, you are well on your way. You probably wnat to get training from your VAR as that will get you off the ground and running. Second of all, it makes a world of a difference when trying to tackle revisions and recording what was done, when it was done, who did it, and if disciplined - why the revision was made. The beauty of Parametric Solid Modelers is that you can make changes so much more quickly and easily, but the flip side of the coin is that it can easily become difficult to trace what changed and why and even who made the change. You also have searching capability including where used functionality, references, and through information stored on custom properties. 3rd - its cheap comparatively speaking to the overall cost of CAD and also how much time it can save you later. $500 is not a lot to ask for PDM, especially considering what else is out there. 4th, its easy to add users as your company may grow. Simply use the vault admin tool. Its also easy to port the vault from location to location - just stop the service, copy the vault folder, and go. 5th, it is a SolidWorks product, so you can be assured that they will improve it, add functionality that the users request, and roll out new versions synchronously with the solid modeling program. 6th, its very easy to implement and maintain. I am an engineer and not in IT for our company, yet I found it was very easy to understand the system thoroughly because it was designed to be used by engineers and not to burden the IT department. Also, if you want to allow non engineering staff to search for, view, and print files in the vault there is an Advanced Server for PDM/Works that contains a Web Portal. From Internet Explorer users can surf the vault looking for what they want and once they find it they can use eDrawings to view CAD files without having to copy out. I am currently planning on implementing this as the next phase for company.

Finally, what ever you do, make sure to document your policies regarding use of SolidWorks so that others that will be working with you can understand not only how to correctly do things, but the reasons why. Sometimes this gets lost in companies as people come and go and the years roll by. I found that documenting these polices also helped to really think things out and try to forsee how things may be used down the road for my company. It also allowed users here to question how we might tackle things that I hadn't thought of. Hope I was able to help. Sorry for the long post.

Pete Yodis
Harold Beck and Sons

 

[cmm]

Thank you pdybeck. One last question.. When it's time to burn a drawing package CD for a client or our archives should I just copy the files from my "vault" to a new folder on the CD and point the assemblies to the new folder? Right now we maintain self-contained project folders for this reason.. i.e. the assemblies don't call parts outside the project folder, they call local copies of "vault" parts, each of which has a project code added to the filename (we learned the hard way to never duplicate filenames).

Chris Montgomery
Mechanical Engineer

http://www.adaptivequipment.com

 

[pdybeck]

Not sure if I fully understand your questions or how you are set up there with project folders. Are you sending the SolidWorks drawing files to your clients? The first thing I thought of is do they need the SolidWorks files - or could you just create eDrawings, PDFs, or DXFs and send them? Are your projects set up in the vault? I would advocate setting your projects up in the vault. You can use the Bulk Load functionality in the Admin Tool to get all you files into the vault quickly. You could also have a project area on your network where copies of vault parts exist. This area is where you would work on the files. This could also be the area where you copy your files to a CD. I didn't really understand why you are pointing your assemblies to a folder on a CD. When its time to send files to your customer just copy the files in the work area to CD. With PDM/Works you can easily make sure the version of those files in your work area is at the same version/revision as the current vault version/revision. The visual icons in the local view in PDM/Works tell you what their status is. You can easily update/reload from the vault to get the correct revision. After that, you could just burn those files to a CD. You could even use the SolidWorks Task Scheduler to create PDFs or eDrawings overnight of the drawing files in your project area. You could burn those files to a CD so you wouldn't have to worry about sending all part, assembly, and drawing files to a customer. I have heard that SolidWorks is working to incorporate Task Scheduler functionality into PDM/Works so that you wouldn't have to copy out files to perform certain tasks. Hope I was able to help. Again, I don't know if I understand exactly what you are doing and need.

 

[JNR]

cmm, we use SmarTeam for PDM which handles configurations as separate part numbers with multiple configurations (for other purposes) for each part. So it is not an issue for us, since we only generated the inital ones with TB.

BTW: SmarTeam used a SW configuration name structure like this:

partname (sub config)

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

There are only 10 types of people in the world - those who understand binary and those who don't.