We are started using solid works toolbox. We have made our own toolbox but the problem is when we use Smart Fastener command then it will allots hardware to the hole wizards. But it allots wrong hardware e.g. in counter bore it allots hex bolt etc.
If any one have solutions for it please do needful.
Also I want some solutions regarding Hole wizard, can we change the type can we change the hole wizard standard from IS to ISO or from one standard form to other?
Yes you are right, but by using toolbox we can save the time if solidworks toolbox populate all the hardware correct.
That is why I am asking for effective method for this if any or any micro.
There are many people that use Toolbox and like it, however there are a lot of us that don't use it for many different reasons. For me it is much much quicker to create your own hardware using design tables, where you can add all the custom properties you want, rather then being limited what Toolbox gives you.
What do you want to do using a macro?
Yes you are right. But if solidworks populate correct hardware then it will be benificial.
That is why I am asking for any effective method if any or any macro.
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.
Ok - Pro-Box
Using a SolidWorks Part file for fasteners is very quick once you setup the first one and it is easy to create additional similar model files, just open the file and edit the design table, change the diameter, material in the first row, highlight that row and drag copy for all your other sizes, so with in a few minutes you can have a brand new product in your Parts Library, which can be setup and shown on the left hand side of your screen..
from
Con-Box
John,
1. Yes
2. Yes
3. Have not needed to since TB has every standard under the sun
4. and 5. Do not need to have the actual helical thread and can change the thread representation from Simplified to Cosmetic to Schematic. Actual helical features, especially on a lot of fasteners, is unnecessary and would dramatically bog down the software.
6. Yes
7. Yes
8. Heck yes!!
We very easily customized TB to include our part numbers and fasteners, not one by one but en masse using a spreadsheet. We exported a spreadsheet out of TB and then, using a simple Excel VLOOKUP command matched the lines there to a spreadsheet we had exported from our ERP with our part number, description, material, cost, vendor, vendor part number, etc. We then imported this spreadsheet back into TB and presto! The information was there and readily used by SWX.
We did not have to create a single part. Therefore we didn't have to model a single part and figure out the rules/relationships to configure them. We also didn't have to download a whole bunch of fasteners from McM-Carr and then go through the tedium of cleaning them up and adding our company information.
To each there own, but I honestly think too many folks bashing Toolbox either haven't learned how to make it sing for them (we just asked our VAR) or have already gone so far down the rabbit hole with alternatives that they don't want to change.
Well, you just said put this in your pipe and smoke it
That is what I expected and wanted as an answer from someone that is going down that path and has jumped in that proverbial rabbit hole - hehhe
I know there were a lot of updates and it seems like bugs have been fumigated and cleared up.. If I were to go back to equipment design, I would definitely take another stab at it and like you said get my VAR to assist, if needed, however I do have tons of files available in my library.. Here I barely use or show fasteners in my models, with the exception of Custom Projects..
So what your saying is that I am an unnecessary Toolbox Masher, something Deepak Gupta was trying to tell me long time ago
John, I'm not calling you a masher, but I wouldn't be surprised to hear you've been called that before.
Potato Masher
All kidding to the side - I would be hard pressed not to use Toolbox and eventually I'll give some stuff a try - but as it is right now, there is no justification for us to go through that learning curve "right now" and that is why I asked the questions that I did, so the new guys can see what a few concerns might have been and the answers, so thank you Dennis Dohogne
Dennis,
Unfortunately we are one of those companies that used TB back in the day when it was a total disaster and went the other way as fast as we could. Now with thousands of assemblies with non-TB fasteners in them to change is almost impossible. Maybe someone like you is the person to get Nikhii started on the right path as they appear to be getting started.
Jim, like you I ran into the early problems with Toolbox at another company. When I moved to another company I brought in SolidWorks so we were starting from scratch. I believed that SWX would fix Toolbox, and they did, so we gave it a shot and have been using it ever since.
I understand if a company is heavily invested in their non-Toolbox method of handling fasteners, but if you aren't too deep or are just getting started then you should definitely give Toolbox a shot.
Dennis,
I am in the process of setting up the TB for our Company, using the import from Excel option works pretty good.
I have a few questions for you.
are you using TB in PDM?
do you let TB configurator generate all configs. or you add as needed?
or do you create new Part file?
Thanks
Andreas
I prefer allowing Toolbox to create new part files, whether in PDM or not. As you generate dozens, if not hundreds, or more configuration in ANY file, toolbox or not, the part file size gets bloated and can cause performance issues further down the line.
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.
This is exactly the reason that I stopped using Toolbox.
I ran into 4 different situations where suddenly all the fasteners in my assembly were suddenly way oversized or way undersized.
I think that it came from making tweaks to the toolbox that was on the network.
2 days later, I after tediously replacing every fastener, the situation was fixed.
Then, I went back into the Toolbox settings, and unchecked a folder of bolts that we don't use, so that we don't see them when we use toolbox, and BAM it happened again!
On top of that, I was told by our VAR that the toolbox was designed for people who use 2 or 3 different size bolts/washers/nuts, etc. NOT almost every conceivable kind of bolt there is out there.
Every job that I do is potentially completely different than the last job. So bolt size is NEVER a standard here.
Every time we used a different bolt size, it would add a configuration to the file. This would increase the file size slightly.
It got to the point where every time I wanted to do ANYTHING with a toolbox component, there would be a 5-10 second delay. After researching the issue, I found out that my little bolt now had literally thousands of configurations and was in the range of 100 MB large in file size.
My VAR told me to try the "Create Parts" option rather than the "Create Configurations" option, but when I did that, BAM! All the bolts got replaced again. I gave up immediately because I was extremely frustrated. I did not contact the VAR again, and just created my own set of bolts. Yeah, it might take a little longer per different size bolt, but it comes without the frustration!
For guys not familiar with parts that have design tables and how you can do your setup files, see the attached... You can do a ton of stuff using excel..
Yes, but isn't the issue with that the same thing that bit me in the butt in the first place? Won't the file size be huge once I add the thousands of different sized fasteners into that one file?
Not if you create smaller files and what I did was to keep the files manageable where I would have one part file per Diameter. Then in the design process you kind of know what is needed then I would add that particular part and if for any reason it would need to be changed later then it's easy to replace components, without loosing any references and/or exploded view references.
What version SW was this created in?
Not even sure - maybe 2012 don't remember
I did open it though and resaved the file in 2016 so if you need earlier versions you can download them from my 3dcontentcentral.com site...
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.
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.
Thank you Dennis Dohogne, standard can be change by this method that I knew, but the problem is that the kind of I am doing right now is to insert hardware from the toolbox. As we have made our own standard so I want to change every hole wizard feature to my own standard for every part. As my machine contain over 600 designed components so I have to do it for all the components. So I am asking for any macro or any other method to do it fast and then I can insert hardware from toolbox by using Smart Fastener and populate all command.
The number 1 reason we do not use ToolBox is that when we first started with SW we only had "Standard" seats. We eventually upgraded 2 of the 4 active seats to Pro version. That means that they have the ability to use TB but the seats that are still (and will remain) as Standard seats can not use it. If we all used Pro version then we might use TB but we rarely use enough detail to require us to add fasteners and when we do we download them from McMaster (probably less than 20 fasteners).
Sir we have 7 seats of Professional and 2 seats of Premium.
Dennis Dohogne wrote:
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.
As an adder to Mr. Dohogne's post, what drops down depends on what's selected for the HW setup.
I've checked these, so...
…I only get these:
Kevin
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.
Paul Risley, we also buy most of our fasteners from Fastenal, but I haven't found anybody's website as thorough and easy to navigate as McMaster-Carr's. I wish more companies would do as well with their website as McM-C does.
And when you find an error in one or their models, if you let them know, they generally fix it within 24 hours.
This has happened to me 3 times, but they were awesome about it.
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<><
I've republished the Toolbox chapter from my 2009 SolidWorks Administration Bible on my blog. Yes, it is ten years old, but it is still mostly valid. It goes through some stuff you may not need like installation, but also through the options for configuring toolbox, and some of the ways you can avoid the file management problems it poses by default.
Thank you Matt
Here where I work they turned away from toolbox many years ago because of many of the issues in the early stages. Now we have 15 years of assemblies with other hardware and I am seeing that there are benefits of using toolbox parts but have all the legacy assemblies to deal with. Without PDM is there a way to change to toolbox parts without having to open 15 years of assemblies and replace them?
Unfortunately no. Toolbox parts have a internal 'flag' on them so SOLIDWORKS knows how to update/replace them directly. I would suggest the following though.
First off, customize the toolbox of your dreams (with Part numbers, materials, etc....) and all the options it needs, per the SOLIDWORKS Toolbox Bible Matt refers to. Throw that in the vault and configure your vault to integrate with the Toolbox (just a few minutes, nothing crazy here).
Then... as you need - open the legacy assemblies, delete the unneeded COTS files, and use 'Smart Fasteners' to autopopulate with hardware stacks.
Thank you Nadia Shea
That was exactly the answer I was expecting. Since I am relatively new here and 5 of the other 4 engineers have been here for over 15 years, I don't see that happening. Oh well.
We tried to use Toolbox when we first started but had too many problems. I don't remember the specifics but it was mostly related to common server location and poor connections, speed of connecting to the server and then finding the parts we needed.
We also rarely use fasteners (since we don't share our assemblies with the customer often and hardly do "Finished" assemblies (the top level people here don't give the time to do it up fully). We don't even do exploded view assemblies / sub-assemblies or BOM's most of the time (I am trying to change that but it's a slow battle).
The biggest problem that we are starting to face is that we are still on (and will be for a while) 2015. Now, most companies like McMaster-Carr only keep 3 years (versions) worth of files - so mostly now they will be using 2016 - 2019 parts - and we won't be able to use them (if we haven't already downloaded the older versions). It's only bit us a couple times so far but soon we will have to make all our own parts.
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.
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?
Nadia Shea wrote:
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 also mean no snarkiness.
We have run into the "larger than life SHCS issue" at least 4 times. All 4 times, it was a gigantic undertaking in trying to fix all of our assemblies. Meanwhile, the boss is breathing down our necks.
Either the documentation is not clear enough for our situation, or I just don't fully understand how it works. I have run through almost every conceivable setting combination and every time we had the issue. I finally gave up after the fourth time.
I don't always download from McMaster-Carr, but I do it a lot.
Here is the same bolt that you referenced after I suppressed the helix. I have a standard process in which, when I download a bolt from McMaster-Carr, I immediately suppress the helix, then update the custom properties. It takes about a minute. That is 1 minute per bolt. That might add up to hours in the end....but it still will be less time than we spent fiddling with toolbox and fixing broken assemblies.
I like the idea behind toolbox. But it is WAY too flaky to depend on.
Maybe things have gotten better now that we are on SW 2017......but now I have 3 years worth of assemblies with McMaster-Carr fasteners in them. And on top of that, I have 3 projects that need my attention. So dedicating a giant amount of time to Toolbox again without a warm fuzzy that we won't run into the same problems that we ran into before just isn't high on my priority list.
I agree with Matt Lombard, in that....toolbox would be great if it were just me on a closed network. But its not just me.
I appreciate the open dialogue. Thanks for giving me feedback to think on.
I think it all stems back to how flaky it was when introduced. I have worked at 2-3 different companies that initially used toolbox and had problems with it so they went away from it. Now several years later even if We felt comfortable about the reliability there would be so many man hours required to try it again that the savings are not enough to warrant the expense.
To further make us reluctant, we do have some toolbox fasteners that were saved out of the toolbox and given our custom properties. Even though these fasteners are stored in a different folder, on the server rather than the personal computer like the toolbox, SW will randomly replace them with the toolbox version and we have to do a hunt and kill to get rid of them. I have run the utility to set as "not Toolbox" a couple of times but they are persistent little buggers.
I agree. We started with TB, and when it began blowing up, we developed an independent hardware category within the Design Library.
It works great! ...Until it does not. Then, regardless of available fixes or workarounds, we made a more robust method that has better stability year-over-year and release-after-update-release.
Burn me once...
“There's an old saying in Tennessee — I know it's in Texas, probably in Tennessee — that says, fool me once, shame on — shame on you. Fool me — you can't get fooled again.”
― George W. Bush
I never tried suppressing the helix on McMaster models. Great tip! Thanks!
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?
One time I took on a project of renumbering all the fasteners and had to fix all legacy drawings. It was a lot of work, but we tackled it over time. Some drawings just naturally came up for change, and we fixed those at that time. If it's just a modeling issue, you can probably get away without changing all the legacy stuff unless it comes up for change anyway. I would use the setup tools to make sure you've got the toolbox properties all squared away before you start using it.
The bugs really affect new users most, and they are the ones least equipped to deal with them. This program should have been fixed 15 years ago. There are so many automated things it can do that it's hard to just discard it, but you've gotta make sure you've got everything straightened out before you roll it out to a bunch of users - and make sure the users are trained on how to deal with it and how to fix problems when they arise.
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
Jay Markey wrote:
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
Agree with 1.
Nevermind... based on reading all the stuff above, I was rethinking decision of configurations over parts and found this on the tab relevant to that...
Duplicate Part NO NO NO NO.
Seems like the way to do it. Why not?
This is what I was looking for. It allows me to have the same part number for different thread displays (which should be the default, in my opinion). Also, because I'm rightfully cautious about this, I tested it a bit. It still throws an error if you try to save items with different size, length, or thread length with the same part number. Unfortunately, it does NOT distinguish between different categories. For example, size, length, and thread length can be identical between, say, a hex bolt and an SHCS, and it allows me to name them both the same. However, because I'm administrating the thing and we are a small team, I'm ok with it. Now, if file names could conflict, that would be scarier to me.
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
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.