Hello dear SW fellows,
we are currently running SW 2012 (expired maintenance). We are re-enabling our maintenance and will update to SW 2014, latest SP.
We experienced many problems in the past with the SW toolbox, such as the 'big screw' issue, and others.
Also, I have read in the past dozens of posts of people having problems with the toolbox, especially when it came to the following:
- Updating: problems when updating SW.
- Sharing assemblies: problems either when sending assemblies with toolbox parts, or opening assemblies coming from a different company with a different toolbox installation.
- Performance: large toolbox file size
These are definitely all cons, but I am wondering if in 2014 the toolbox is better than it was in the past?
At this time, we are downloading hardware 3D files from McMaster, and creating our own library. This works very well, but is extremely time consuming to build.
I would love to use the SW toolbox, if I knew for sure it would be stable and problem-free; especially considering it has much more than screws and nuts, like retaining rings, bearings, etc etc.
Also, at this time we are not using any PDM, but upon updating to SW 2014, we will also install Workgroup PDM.
I assume we could place the toolbox in the WPDM, and only have to manage one toolbox for all users, correct?
I look forward to hearing your opinions.
Are people still manually building their own libraries, or is the toolbox more reliable now?
Thank you.
And how do you handle different materials?
Right now I do one file per size bolt per material, with configurations for lengths. So a 1/2 grade8 bolt is a different file from a 1/2 18-8 bolt.
Just curious to see what people are doing...
I generally just insert a note on the drawing calling out the grade. That works okay for me, but it might not for everyone.
We use one file for each size bolt in a particular material, and use configs for lengths. So we'd have a file for 1/4-20 SHCS Steel Black Oxide, another file for 1/4-20 SHCS Stainless Steel, another file for 5/16-18 SHCS Steel Black Oxide, etc. There aren't that many length options that bolt come in, so I just create every length up to some limit I think is reasonable, for example for a 1/4-20 screw I might only make configs up to 2" long initially and add longer as needed. If you make the files for one material first then you can just copy them and all you need to change is the material property to make the other material files.
With regards to PDM, I don't think you need to bother checking them in. What works great for us is to put the files on a network location that everyone has access to and have all the users set that location as a Design Library. Then the parts will show up alongside the toolbox in the design library tab. Then in your Workgroup PDM options you can disable check-in of standard library files (because you probably don't need revision control of them).
We want to give a number to any standard part with configurations.
The number is in the Solidworks partfile name.
We make our standard parts with design tables.
But after SW2006 there is no "save last used configuration" anymore.
This has caused us hundreds of hours additional work and
design time for large projects have decreased dramatically.
We design a lot of machines consisting of standard parts.
Suppose I insert a bearing (with all configs in it) with name
for example 25#deep groove ballbearing and config=6002
This part number 25 is used for example 20 times in 10 different subassemblies.
But after the bearings have been inserted, we decide that the bearing should be bigger,
suppose it should be 6004 instead of 6002.
Till SW2006 we would have all the standard parts to set "save last used configuration"
and it was 1 mouseclick to update part 25 in every assembly.
But after SW2006 a name of a part is not unique for it's configuration anymore,
which not only needs you to search for 20 parts in different assemblies and changing
the configuration each seperately but it also causes a lot of mistakes.
The number of mouseclicks to do these simply things (before SW2006)
have easily increased 10-100 times more.
This is one of the biggest inefficiencies we have in Solidworks after SW2006
when using standard parts with configurations.
I never understood why such a time, mouseclicks and error saver simply has been removed.
Does Toolbox fix these problems?
We have many parts with configs that are not in toolbox like motors,
pneumatic cilinders all kinds of non standard bearings etc etc.
If Toolbox could fix the problems that were introduced after SW2006 with
discontinuing "last saved configuration" then it would make sense for us.
Jody has explained that you can configure toolbox to save a separate file for each configuration. Is that what you are talking about? So that if you want to change all instances of a fastener you can do a replace component instead of configuring each individual instance?
I think that is far too much work also.
We are thinking about making an external database
with the designtables that recognizes the part and allows
you to change to another standard size. A kind of VBA
application should change the dimensions of the existing part.
The problem is you can't change the current configurationname
which now is the part list info for us.
25 years ago we had a German Autodesk application called
Genius, they did it the same way in Autocad. When you edited
a standard part it recognized the part and showed the sizes
according to DIN/ANSI or your own standard.
Changing a named part to another size that has been used
several times should be easy as it happens so often.
It was so easy and logical before in SW2005.
In SW2005 I opened the part with the configurations and
changed the configuration and all instances were automatically
changed of that standard part.
In the menu (see picture) there was a checkbox
"Use component's "in use" or last saved configuration"
This is how it should be as a named (numbered) standard part is
unique, you should never have parts with the same file name and
different sizes driven by configurations.
I can't believe why they broke it and never fixed it.
Why does Solidworks remove such usefull options.
Maybe they broke it to sell us Toolbox??
Anyway, there is no way Toolbox can fix what has
been broken after removing this usefull option.
"Use component's "in use" or last saved configuration"
They probably took away that option because it led to a lot of mistakes. Let's say you used that option for all of your bearings in an assembly. Then later you want to add a new size to the bearing, suddenly that new size is the last saved configuration and all of your bearings changed to that one without you knowing about it. I don't even know what the "in-use" configuration means. What if you are using several different configurations of that part in the same assembly. Which one is the "in-use" configuration?
In use means the last saved configuration of this part.
So how it looks while you open the part.
You could have different sizes with the same partnumber in
SW2005 too like it is now but we find that very tricky.
When you want your part to behave "unique" you choose
this last saved option in the assembly where it is used.
If you don't want that you don't set this option. It was
much more flexible.
If your bearing has the same filename it should be the same size everywhere
in that machine for us.
We always have a unique filename for one size of the bearing.
A bearing starts with a number in the filename for us.
What you explain with the mistakes is what is happening for us now
without this option.
We also have parts that we don't give a name, for example a simple
washer or bolt. In that case we don't use a number for that part
and we do not use "save last configuration".
We use the numbers to have them unique. They are in stock under
a certain number and the easiest way to manage it is by starting the
part file name with a number.
Of course everybody has their own ways of managing part names,
after learning from the mistakes we did it like I explained.
This is a long post. But in evaluating Toolbox I thought sharing our company’s process and discoveries story may help future users make the decision for themselves. Please note, we are using Solidworks 2013 and are about to update to 2014 now that most of the initial patches have released. And the problems we ran into may not pertain to your situation.
We are trying to create standard operating procedures for our growing office and have been evaluating between the following methods as options for fastener addition to assembly models:
1) Toolbox
2) Design Tables in the Design Library
3) Separate Folder of individual Fastener Files
Option 3 is what our company has had for years and has worked fine, but we want to try to increase efficiency and get everyone to use the same methods? So, we continue the evaluation.
Option 1 is used by some of our engineers who have loved it, but it hasn’t historically been matched to our part numbers and they have to look up our inventory listing to ensure they are using options we have in stock if at all possible. So this process has been slow out of the box.
Option 2 is new to us and seems to be working really well, but to replace fasteners, even with the built in “replace” option, you have to dig deep into the design library source files to choose the replaceable part, if it isn't already a configuration of the part that was originally chosen from the design library. It would be great if the design library had a replace function of its own to save time by avoiding this digging function, but we haven’t seen that yet.
OUR COMPANY: When entering a fastener into our assembly models, we want our engineers to first try to find a fastener that would work from within our inventory, that we purchase on a regular bases, before creating the need to purchase a new fastener we don’t normally carry. We don't want to start purchasing a new fastener for their designs if we have something close that would work just fine. Our reasoning is that we want to purchase in bulk. However we sell and produce custom products. To increase efficiency, we are trying to avoid having to purchase one or two of any fastener for a product we will be producing once or twice a year. A whole bunch of this will get costly fast, so we limit the new designs so we can stick to some basic standard hardware. When creating designs, our engineers start with need and size then work with the BOMs later after the design is complete. So picking from our inventory, they choose size first, then list the part numbers later.
OUR EXPERIENCES: In trying to get Toolbox to work for our purposes, we have played with Toolbox a bunch and have spent many hours on the phone with our support team learning how to customize toolbox and adjust it for our needs. Never at any point did we go behind the scenes and manual manipulate any models or any tables. We only worked through the existing functionality of the Toolbox Configurator.
We have used the import export tool to enter all of our regularly purchased parts. We copied all the hardware models we could find into a single folder so we could eliminate searching for parts within the toolbox. We have created custom properties and have utilized the material choice options.
LESSON ONE: One large learning curve we went through is to find how to avoid broken toolbox links. OUR CHOICE: As a result we have chosen to create toolbox configurations instead of individual parts. WHY WE CHOSE: When saving individual parts, it actual separates the parts from Toolbox. Toolbox will recognize the separate files, but will no longer manipulate them from the Configurator. Thus if we want to add or remove a custom property in the future, it would no longer recognize the individual files, because it would not know with which of the new property options it is associated it. Or, if you removed a property, it may have previously created a separate model for each of the property options that are now null and void and it doesn’t know which model to use, so it doesn’t use any of them. This resulted in a lot of broken links and miss identified fasteners.
We even tried the “duplicate part numbers for geometrically equal components” option to try to create multiple materials, but the same problem was created where the parts were technically no longer recognizable to Toolbox if we updated property options later. This also added a few other weird side effects that I am not remembering in detail enough right now to list.
LESSON TWO: We did however find that updating properties was possible without losing all of your previously inserted data. You simply have to:
It wasn’t a fast process, but it did allow us to NOT LOSE our previously entered data.
LESSON THREE: We also went through a lot of searching to find out that Toolbox does NOT have models for several of the Imperial Standard hardware that we use regularly. I can find just about any fastener model we could want in metric, but can't find toolbox models for Nylock Nut, Nylock Nut Thin, or Toplock nuts with standard imperial measurements. We also cannot find a model for Clevis Pins that gives what we thought were standard combination options of diameter and length. All of these things we purchase regularly from the standard options listed online for sale to the public from large fastener vendors such as McMaster Carr. These are fasteners that can be found in any hardware store here in the mid-west (Kansas). It doesn't make sense to us why these options would not be available, but have had to forfeit some toolbox usage to method options 2 and 3 above, right from the start, because of these omissions in Toolbox. There are several other “Standard” fasteners that are missing, but we purchase them on a rare enough basis that having a separate file for them wasn’t that big of a deal.
Still we pushed forward to see if toolbox could possibly save us time with just the fastener models we need that ARE available in Toolbox. So we continued to set up toolbox for our use and trials.
OUR CURRENT STATE and PROBLEM:
We now have everything set up with all of our standard hardware (those we could find a model for in toolbox) and were testing through it to see if it would actually run the way we want it to. Now we are running into another problem.
BACKGROUND TO UNDERSTAND OUR CURRENT PROBLEM: Our part numbers were added to fasteners in number order of need. So as we needed a new fastener, it got the next consecutive number. So, if we ordered our fasteners by size, their part numbers would not be consecutive and vise versa; if we ordered the fasteners by part number, the fastener sizes would be all over the place and not in order. This causes toolbox efficiency problems as follows:
When we add a toolbox part, it first auto inserts according to the hole size in the model, which is great. But, if we want to add a different nut size (Nylock nuts are larger), we may need a longer bolt. We can simply choose a different size in the properties box, which is also great.
However, with all of the information and part numbers we have imported into Toolbox, it doesn't narrow the options by only that information. For example, all length options are available whether or not we have a part number associated with them or not, because it is filled into our matrix.
NOTE: Example: When narrowing down the options by unchecking them in Toolbox Configurator, if you want a single odd ball bolt length, then it must be available for ALL possible property combination of that bolt size. So if we want it to be available for only Stainless steel material, half inch diameter, then it will available for every other Half inch diameter bolt in every other active (with check mark) material listed in the materials property option. Causing an exponential number of options to choose from, every time you add a property. We have narrowed the properties options in Toolbox Configurator by un-checking as many as we could.
Toolbox will list in a window sorted by Part Number all of the parts you imported. But, even after narrowing down their options by un-checking them in Toolbox Configurator so they are not available for the picking, our engineers still have thousands of combinations available to choose from. When they choose a combination of properties form the dialog box, the only way they can tell if they have chosen one of the couple hundred fasteners that we entered data for (our inventory) is by lucking out and choosing the exact properties combination of one of them. At that time, Toolbox will highlight the fastener of choice in the Part number window. But, it won’t scroll to it, so they may not even know it is highlighted. Toolbox will also not narrow down the options in the part number window, so they can pick one of the imported options listed that may be close to a size we have in inventory. They are essentially blind to the information we entered until it has been entered and accepted. OR, they can scroll through the several hundred options we did import, which would be great if they were looking for a specific part number, but they are looking for a size. And as mentioned before our part numbers are not consecutive with size, so the sizes are listed randomly because this list is only sorted by Part Number.
IN SUMMARY: Our engineers cannot tell via toolbox which of the toolbox property combination we actually did import into Toolbox, and thus cannot tell if we carry the part in inventory or not. At best it’s a crapshoot to pick one of a few hundred out of several thousand options.
So this turned out to be quite the conundrum for us.
It would be very helpful if toolbox would narrow down the visible options in the Part Number window as properties are chosen from the dialog box. Even if it narrowed it down by diameter or length, it would be a huge time savings.
This detail of Toolbox is such a pain that we are thinking of forgoing toolbox all together. I spoke with our helpdesk and they said that Toolbox simply can't pull information in that direction to narrow down the list. It pulls information from the other direction to simply provide the list of the imported data in order of part number. We already have lists of this information, importing it into toolbox to list it, in a not so helpful sort order, did not improve things for us at all. And the list that Toolbox shows is much less user friendly than the excel sheet we started with. At least with the excel sheet they can sort the list.
Toolbox for our engineers is suppose to help them work from the design and size to the part number. Making them look through the list of part numbers to find the size that is close to the one already chosen in toolbox is counterproductive.
So we are back to the drawing board. We are probably going to start using design tables. The only problem I have found with this is in the replacement function, where we have to dig down into the design library to find the parts to replace them. And it would be nice if we could use the auto-sizing functionality that toolbox provides.
So, I hope this helped at least one person out. And, I hope Toolbox improves in the future. But in the mean time, we are still struggling with its usability and hope something better and similar comes along soon.
That was a very good and thorough explanation of you situation. A couple of your problems might be helped by moving toward a design library of standard components instead of toolbox.
It seems like a common method of setting up screw files is to have one file for each combination of thread size, material, finish, and that one file would have configurations for every length option. If you set up your library in this manner then changing lengths of a screw is as easy as changing the configuration, it would not require digging around in folders. However if you wanted to change from a button head to a socket head screw, then you would need to browse for the new file. But you can set up the folder structure of your design library in a way that makes it easy to navigate to the desired files.
As far as helping the engineers pick common sizes, that will be difficult. The best I can think of is to only create configurations on demand. So when an engineer pulls a certain screw into an assembly, it might only have a couple size options for what you have used before. If they need a new size then they would have to open the screw file, edit the design table, add a new length and assign the new part number. I don't know if you'd trust all of the engineers to do that without messing something up. You could also have one person in charge of updating the hardware and have all engineers go to them when new sizes are needed.
Thank you Jamil!
Yes, we are considering all of this. We do have a design library started and it is built exactly as you explained so far. The digging into files was specifically targeted at having to change thread sizes/diameters. And as far as trusting the engineers to not mess things up, well we don't really. We love our engineers and their brilliant minds, but also acknowledge their need for speed and efficiency and tendency to skip the insigificant details that results in messy paperwork. It's not their thing, so we have a document specialist and file manager to support them, so they can continue being exactly as they are, BRILLIANT, and nothing gets mixed up, messed up, or missed.
So excellent suggestions! We've choose all of them!
Thank you.
TJ
Just to close our story...
In the end, after much evaluation, our company has "officially" decided to go with design tables and not use toolbox at all. We feel that toolbox has too many problems, and is lacking too many basic hardware elements for it to work for us. We think it would simply slow us down instead of adding benefit. Design tables are working marvelously for us, and because it is easier to access, we can update, add, change, etc any details we feel are necessary.
Thanks everyone.
TJ
This reply is old, but I thought it would be a good information to those deciding weather to use Toolbox or not.
I have worked as cad administrator in 3 different establishments in about 10 years. In the majority of people I've set up with toolbox I think they would have been better off without it. In the past I have been a BIG supporter of it because I believe it is going to improve to the point of if we don't use it we wish we did. In 10 years I haven't seen anybody working in departments agree with that.
1. It doesn't have all fasteners. Most "pointed" screws are missing Those come in kind of handy for places that design office furniture. Pop rivets are missing, and a deluge of other fasteners we end up creating ourselves. So that means there are (2) places for hardware. If you use design tables and library parts in pdm, that problem goes away and you can have 1 central method. Oh yeah I have suggested several times adding these, that was several years ago.
2. Our dept. finds it way overcomplicated so its a struggle to enforce its use. I've been at it for 8 years and am still learning things. Many design engineers are lost, and it takes a few of us to figure out simple things like adding sizes or types. We are talking guys using Solidworks for 12 years, 3, and new people good luck with that.
3. Slow: We use pdmworkgroup, (soon to use pdm pro), and boy do our Solidworks design table fasteners work slick compared to the slow toolbox. Instead of putting everything in a centralized vault it shoots these out to a local drive (pdmworks does not recommend checking in toolbox parts). Do you see a pattern here? two different types of fasteners now we have 2 different places.
4. Bugs& bugs. We have at least 1-2 SPR's for bugs we have found in toolbox, for stuff like unable to exclude from BOM. No problems for the old configured parts.
5. Creates exponential configurations: If you add properties to your fasteners with different suffixes it is creating thousands of configurations for example separate property for material and finish, you have to have a configuration for every finish every material. We are conservative on properties. Your simple design table only creates the ones you need.
6. Confusing fastener organization such as washers. They are in categories (ANSI inch) that most never refer to including McMaster Carr & Fastenal. Plain Type B, Preferred type, even degreed engineers who have to constantly ask which category there are in or create cheat sheets.
7. Complicated to create drawings of groups of fasteners with revisions. Our plant requires drawings of all fasteners, if those drawings change a revision is necessary. Toolbox doesn't play well with revisions or grouping fasteners together on one drawing, in pdm they are not revision managed (the normal Solidworks is a no brainer). We ended up creating an assembly with different toolbox fasteners in it and revise the assembly which revised the drawing. Your single design table driven part is much simpler than this.
8 I think toolbox may have its place in more of a job shop- or mechanical only shop where "pointed screws" are never used. For administration of the thing, you will need to have 1 trained guru to keep it managed or else you will have a mess. A position not necessary for simple configured parts. All that administration and troubleshooting of another "system" costs money.
9. Toolbox is a good reference for dimensions of the parts it has, for example the hex size of a bolt or thickness of a nut.
10. If you change properties and delete others, toolbox quickly turns into a mess. It puts suffixes on the configurations that may not relate to the old ones.
11. Pack and goes with other SW establishments get messy because the toolbox parts are named the same thing.
12. If your network is slow or pokey don' use it collaboratively or else it will slow down your SW.
In conclusion I think toolbox can be used as a reference or in a small job shop(mechanical) establishment. Don't use it if you make things that use wood screws, or unusual fasteners because many are not in there & don't hold your breath if you ask them to be added. Send a person to your VAR's class on this before it is even set up and make sure that person knows it inside and out. If you have a larger engineering department over 5 people this person should set the parts up or else you'll have a mess, for example its easy to create a screw configuration and forget to select full thread vs. partial thread. Some of the tips are called out in letter codes that are difficult to know what they mean. SW has made some valiant efforts to improve this but still has a ton of work and massive simplifications.
Both Theresa Ouderkirk and Robert Bartz have listed the reasons why I don't use Toolbox any more. At best, it is confusing, and if you use a special field for your part number field, then you are SOL completely. The sorting thing that Theresa mentioned was the worst, though.
My experience with the toolbox (TB) is a based on annoyance.
Now that it's prefaced, I can be constructive.
The toolbox, in theory is great.
Counterbores aren't standard.
嗨，我可以向你请教一些关于 toolbox自定义属性的问题吗？？？
我怎么联系您？你有QQ 吗 ?? 多谢
请问，
how Add attributes of"weight" to the toolbox parts in toolbox manager?
Our company has just started thinking about testing Toolbox again and found your post. Wondering have you changed your opinion of Toolbox?.
We abandoned Toolbox a number of years back and went with design libraries and configurations. We did this for pretty much the reasons you detailed in your post.
We too add part numbers as needed, and prefer to use sizes we have used in the past just to keep inventory under efficient control. We have some custom fasteners (head modifications, non standard lengths and buy these in minimum quantities of 10,000). So curious as to the current state of usefulness of Toolbox.
I have been using SW since 1996 and am aware that TB has its issues along the way. With a properly set up backend, I find the TB extremely fast and indispensable. It is bewildering to me when I read such negative reviews of it. Drag n drop, resize, and ... BOOM! there's the exact PN. I just haven't experienced many problems with it at all since line the late 90's. There hasn't been a design I've produced in years that wasn't done using TB. I've created custom TB parts, like rivets, SEMS screws and KEPS nuts, that act exactly like all of the other TB parts. Just need to set it up properly.
Wow this thread is really making me think twice about working to implementing Toolbox. I had a conversation with a VAR to discuss the positive developments since the pre 2012 toolbox and was fairly convinced the previous issues I had were fully fixed. From this thread it sounds like there are still major issues even recently. Is there anyone that is a regular user of Toolbox and that has positive things to say?
Grant,
I'll paste my comment above, in case you missed it. I use it exclusively all the time and never have issues with it.
"I have been using SW since 1996 and am aware that TB has its issues along the way. With a properly set up backend, I find the TB extremely fast and indispensable. It is bewildering to me when I read such negative reviews of it. Drag n drop, resize, and ... BOOM! there's the exact PN. I just haven't experienced many problems with it at all since line the late 90's. There hasn't been a design I've produced in years that wasn't done using TB. I've created custom TB parts, like rivets, SEMS screws and KEPS nuts, that act exactly like all of the other TB parts. Just need to set it up properly."
Grant Mattis, I heartily second what Doug Dina just wrote. We've used Toolbox for about 10 years so that spans the 2012 issue that SWX had. That particular issue just kept us from upgrading for a few months and nothing else.
Here is what we did:
1. Exported the fasteners from our ERP system into a spreadsheet to include at least the information of the part number and description.
2. Exported from Toolbox a spreadsheet for each different fastener type.
3. Using simple Excel commands such as VLOOKUP we modified the spreadsheets from TB with the matching part number and description from our ERP system.
4. Import this modified spreadsheet back into TB.
5. Repeat the process for the other fastener types.
6. Enjoyed the use of Toolbox by selecting OUR fasteners containing OUR part number and description to properly show up in the BOM. Consequently this also was a shorter list of fasteners to choose from since the list is populated with only our sizes, not all that exist in the world.
The setup/customizing of TB is actually easy once you learn how to exploit the Export/Import function. This work is FAR less than the work involved in doing this with separate part files and configurations. In addition the TB parts carry some nice attributes such as smart mates and a flag to include/exclude them from BOMs or other selections. In SWX2017 they introduced a nifty new feature where you can select a bunch of TB fasteners, even of different types, and RMB to Edit Toolbox Components and change all of them at once. What's not to like?
In my opinion a lot of folks never took the time to figure out how to fully capitalize on TB so they went another route. That's perfectly fine, but I did that in SWX from 1995 to 2007. In 2007 I went to a new company and was in charge of the design and manufacturing engineering groups. Setting up Toolbox was one of many things I did there to dramatically improve our operations. The only way I'll NOT use Toolbox is if I am at a company that doesn't have SWX.
By the way, our Toolbox is on the network and we have no issues with it that way. It is actually better because when we add a fastener to our ERP and then to Toolbox we only have to add it once since everyone is pointed to the same TB.