How we can effectively use toolbox?

I would read this thread:

Using Toolbox: Do or Don't?

Personally, we used the toolbox for a while here, but since we use such a large variety of bolts, our bolts became massive (file size) with the amount of information that was in them.  Which bogged down even the smallest of assemblies.

Then we switched the setting to "create separate part" rather than configuration, but it still didn't work very well.

There are people here at my facility that use the toolbox, but I personally don't.  I just created models for the ones we use the most, labeled them with the part numbers we needed and done.

I am a strong advocate for using Toolbox.  it has made our life much, much easier.  File size is not a problem and the information that is already available with a TB part is superb.  We customize our Toolbox by only including the fasteners in our inventory and adding our part numbers and descriptions.  Everything shows up properly in the BOMs.

Please search this forum for more information on using Toolbox.  You will see arguments for and against.

Nikhii, my vote is NOT to use toolbox.  It's caused me endless pain in the past and I have come to the same conclusion that many here have:  DON'T use it.

First, the toolbox is incomplete.  If your protocol is to use toolbox parts, when you encounter a part that isn't in the toolbox, you now have to decide how to approach it.  This can happen quite often.

The toolbox can be volatile.  It can change.  It needs to be carefully managed, especially if on a network being use by many.  If you have an excellent administrator and are sure that person will always be there, then you have a better chance at keeping the toolbox working properly.  But short of that, you are taking a chance.

I've had problems where the toolbox forgot all my fasteners and then it just puts in giant fasteners or tiny fasteners, basically whatever it feels like.  Then, I have no way of knowing what size fastener was there.  At that point you are screwed.  Maybe the network was down.  Or who knows.  I just know I determined to never let that happen again and I came up with what many do here, make our own library with individual parts that have only one configuration and maybe even are dumb parts that came from a step or iges.  then there is no way for this part to change...EVER.

Creating your own parts library isn't that difficult.  The truth is that you only use a certain number of pieces of hardware, and often you reuse the ones you have used before.  To date, we only have 102 fasteners, these are nuts, bolts, and washers.  That was developed over a 4 year period, so only about 25 a year.  YMMV.  We have multiple libraries such as fasteners, hardware, hydraulic, electric, mechanical, etc.  Total is maybe 1000 parts.  We reuse parts as often as possible, and then occasionally we have to add a part or two.

But the bottom line is that I never have a problem like I did with toolbox.  If the network is down, SWX does not just substitute something different.  It doesn't load that part until the network is back up.

By the way, I even tried once using toolbox parts but converting them back to "normal" solidworks parts.  Even this caused me headaches.

Nikhii Gandhi

Here are my comments in response to the others:

A couple of releases ago SWX fixed the giant sized fastener issue.  I remember that being mentioned in a rollout.  Perhaps one of the VARs on here can chime in and say when that was and what is really the culprit for that.  I'm not sure, but I think that problem is generally related to the software looking in various locations and finding different sets of TB files, but I don't recall for sure.

We use ANSI Inch and Metric fasteners, except we use DIN for the Nyloks.  It turns out there is no inch standard for Nylocks, even though you can download those from McMaster-Carr (McM-C is very good about listing what standards/specs a parts complies with).  There are no standard fasteners that we have needed that are not in those standards.

Our TB is very stable.  The only time we have a problem is when we try to use TB parts outside of our network version, such as on a home computer doing company work.  Even that is not a big problem for us.

We are a very small company, less than 20 people.  We have just over 300 fasteners of a very wide variety.  TB has been a real blessing for us.  There are so many benefits to using TB parts that do not exist for non-TB parts such as changing a whole group of fasteners all at once (new functionality in SWX2017).

It doesn't really matter whether you setup TB to create separate part files or separate configurations.  The net result is the same.  For what it's worth ours are setup to use configurations.  SWX manages these for me and size is not an issue.

One of the issues of using non-TB files is the management of all the fastener files.  Using configurations controlled by a Design Table is the way I would go if I were to do it, but a file with only 50 configurations can be lethargic and large.  That is also a reason not to include any more detail than necessary.

Andreas Rhomberg, no we are not using TB with PDM, but when I was grilling my VAR he showed me examples of how that is done without a problem.  One of the guys at my VAR used to work at SWX in the Boston area and I think he even worked with the PDM.

We have our TB setup on the network and all of our networked licenses of SWX are pointing to it.  Any of us can change the parts in the file, usually only adding a new fastener.  We do not have copies of TB on our local drives.

Accessing the files across the network has not been any kind of stability issue.  We access all our SWX files from the network.  However, that is a key aspect of PDM that I would like to take advantage of - that PDM makes local copies of the files to your hard drive and you work on them from there.

I've got a pretty good VAR and they did not try to dissuade me from using something just because they weren't intimate with it, as it sounds like some of the other VARs have been with Toolbox for some of the people replying to this post.

At this company we've been using Toolbox for over eight years and wouldn't do without it.

Nikhii Gandhi,

In rereading your original post I realize we all jumped into using Toolbox vs. not using Toolbox and overlooked one of the things you were asking about.

In using Hole Wizard you can very easily choose which standard you want for the holes types:

Just hit the drop down list and pick the standard, ISO, IS, DIN, etc.

Ok so I know Mcmaster is the go to for all things.

I have never once seen anyone mention Fastenal or Grainger.

Our bolts have part #'s for both Mcmaster and Fastenal built in to populate the bom.

I think if given the chance to start fresh I would go with toolbox now. But being as our machinery is legacy information along with re-build updates utilizing 2 forms of hardware control would be a PITA.

My 2 pennies worth.

My vote is also for not using Toolbox components. What I do for the most part is to spec all my fasteners from McMaster Carr. Every fastener and widget on their website has both the 2D drawing and the 3D Solidworks model available right on the same page where you select it from. It is very easy and quick. The filename has the MC part number in it and it makes it very easy to re-save it as a file that you can use over and over. Their Solidworks models seam to be very reliable in quality also. Just my two cents!

Rick<><

However you decide to use Toolbox and/or configure it, it only works if you train your users effectively and they practice consistency. It usually takes me 1-2 hours to start off a large groups of users on how to use Toolbox and about 30 minutes each time I add a new user to the group. I would also consider documenting your desired Toolbox usage and configuration for reference. It's not much more effort than training users how to use a shared library of files.

If you choose to NOT use toolbox and create your own COTS (Common off the shelf folder), consider some pretty awesome productivity tools you could be missing out on.

• Smart Fasteners - 2019 SOLIDWORKS Help - Smart Fasteners Overview  - The ability to auto-populate all hole wizards holes AND create hardware stacks.
• Even if you don't use Smart Fasteners, many Toolbox components have mate references and smart components features built in them, thus allowing them to autosize during individual drag and drop. (2019 SOLIDWORKS Help - Auto Sizing Toolbox Components )
• Updating all Toolbox components in an assembly in a few clicks.
• Added in 2019 - New option to automatically lock rotation in concentric mates, only for Toolbox Components. (2019 What's New in SOLIDWORKS - Automatically Lock Rotation for Concentric Mates to Toolbox Components)
• Consider Toolbox has been and is currently driven by a database, not embedded design tables/configurations. This can have current performance implications with file size/usability.
• Consider future productivity enhancements that may only be available for Toolbox parts and not a custom built library.

I'm definitely Toolbox biased, if you can't tell. However, ask your VAR or read various articles/blogs how Toolbox is structured. It's worth the time to understand how it works and how it can be leveraged. Then consider the time it takes to train your group on how to use it vs the time savings you COULD have with current features. If it worth it, use it. If it's not worth it, don't.

This is a honest question and one in which I mean no snarkiness at all.

For those that prefer NOT to use Toolbox and download your files from vendors, how do justify the hit in performance from sheer file size/rebuild performance?

Attached is what I consider an average example, I've quite often seen much worse comparisons and am sure there are less dramatic examples.

Vendor file is 1,210 KB while Toolbox file is 206 KB. That's 6x as much in file size.

Rebuild time is 0.13s vs .03s. That's 4x as much in rebuild time.

Graphics Triangles with comparable positions on Image Quality slider bar is 14178 vs 532, against 4x.

I know some groups have small/less complex assemblies that simply do not actively feel the performance hit yet.  However, as we grow, we all know large assembly performance issues are very challenging to manage by the time you 'feel' it. . I know this doesn't affect groups who design and model their own commonly used files. I know some groups are lucky enough to have awesome hardware to delay the impact of the performance hit for a long while. I also see groups spend alot of effort actually simplyfing the models themselves OR download generic parasolid versions of the files. (Latter option can sidestep files size and rebuild time but still presents major issues with graphics and usability).

Honest question: What benefits do you gain from conscientiously NOT using the Toolbox that is worth extra resource/effort cost?   Is it strictly file management? Or more user management?

I am in the same boat as many others - we tried toolbox years ago, weren't happy (don't recall why), started our own library of fastener models, and now have 20 years of stuff done that way. However, I am now considering giving Toolbox another shot.

Some of you seem to be saying it's too late to go back and try Toolbox again now that you have gone so far in the other direction. I don't understand that logic. Fear of Toolbox blowing up is another story, and I can understand that. But if you trust that the bugs have been worked out then why not give it a shot? Saying it's too late because of 20 years of doing it the other way sounds like sunk cost fallacy. If there are benefits to using Toolbox you can reap the benefits for the next 20 years if you start today, right?

My one concern (aside from cost of upgrading licenses) is having two copies of fastener files going forward. We'll never get rid of the non-toolbox copies since there's just too many where-used to go back and replace those. So I will have to maintain the description, vendor, vendor part number, etc. in two places when/if any of that info changes. But that info is pretty stable, so I don't see that as a major drawback.

What do you guys think (those of you who are not simply fearful of bugs)? Do you see other problems with having two systems in play?

Hello,

We use it for PEMs only, for which it performs wonderfully, especially when combine with Hole Wizard.

No need to look up PEM sheet hole data, plus the PEM name is in the tree and like Hole Wizard, the name updates on changes (provided you don't edit it).

As for other hardware, such as screws and nuts, it's usually a McMaster model as they are the low volume source and we don't assign internal part numbers to these.

We use the McMaster number as the part's reference for buy and drawings.

Their models are built so the configuration name is the McMaster part number and that this becomes the BOM part number.

We just add a description.

Not a ding against Toolbox. We just don't have the need (or the will perhaps), to move the tiller towards Toolbox on items other than PEMs.

The original question is a bit old now, but since I googled my way into this just now for different reasons... If I understand the question, I believe the issue is here:

Counterbore was mentioned as an example, but each section has a similar default fastener type.

What originally led me here was when I found that the Toolbox apparently wants unique part numbers for each thread display configuration of a fastener.  For example, I have a 1/2-13 x 3" Full Thread Hex Bolt.  That one part has three thread displays: simplified, cosmetic, and schematic.  Each of those corresponds to a unique configuration name (I have toolbox set up for configurations).  However, because they are all the same part -- regardless of display, the part number for all three is "1/2-13 x 3 FT HB".  That's what we'd show in the BOM regardless of the display.  For some reason though, the Toolbox is forcing unique part numbers for each of those.  SWX thread display has nothing to do with the physical part number of the fastener.  It should only depend on Size, Length, and Thread Length fields within that group.  I'm very confused about this.

I have a few choices for dealing with it:

1.  Use only one thread type -- probably cosmetic.  Disable the other two.

2.  Pick a default thread display (such as cosmetic) and either remove the P/N for the other two or put a (N) or (S) at the end of it just to get the Toolbox to shut up about it.  That would cause problems on the BOM as it relates to our ERP, but ... it's one option.

3.  Use some other field for P/N ... though I have no idea how I'd keep that working in a standard drawing BOM.

#1 seems like the best choice.  Anyone else dealt with this?  (I'm using 2018 by the way.)

Regards,

Jay

No for 2 reasons.  1 got caught in the flap of large tool box parts showing up.  So the company uses their own parts.  Which some come from MCMaster.  But as has been noted if you insert a lot of these it will really slow down your system.  I do like the Idea of Suppressing the helix that was mentioned.

  But the biggest reason we only have one seat for tool box and have to share it.  Our Machine shop Forman uses tool box constantly and if I was to need it I have to ask him to close it so I can use it.  He never closes a drawing or toolbox till the end of the day.  So I would spend way to much time waiting. Faster to his McMaster, or use a part we already have in the system that is not from the tool box.  But open a drawing the machine shop Forman has modified and those big parts show back up and I have to change them out so the rest of us who do not have the toolbox checked out can view the part correctly. he has modified