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Parts quantity not correct in bill of material

Question asked by Mattew Stafford on Feb 6, 2017
Latest reply on Feb 13, 2017 by Deepak Gupta

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I am new to using Solidworks 2d & bill of material, etc. I used toolbox components and noticed that Solidworks separates the parts in the BOM, but item #23 shows a quantity of 111 of the 1/2-13 hex bolts x 1.75" long. Item #24 shows one hex bolt (which I am pretty certain should be labeled the same as item #23). I don't like the callout of these toolbox fasteners & see some information out there on correcting this, but I want to figure out the quantity issue first. Any ideas on how I can find what model that this hex bolt_ai is referring to? Any ideas on how this can be corrected? Thank you

John Stoltzfus Feb 6, 2017 2:45 PM

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Might be the same part but they are different configurations, I think there is an option for that when you insert the toolbox parts...

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Glenn Schroeder Feb 6, 2017 2:25 PM
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Mattew Stafford wrote:

Any ideas on how I can find what model that this hex bolt_ai is referring to?

Right-click on a cell and you should be able to see the file name, and open it if you want.
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Mattew Stafford @ Glenn Schroeder on Feb 6, 2017 2:35 PM
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Thanks Glenn. Good information. When I do the right click-open, for both items 23 & 24 (probably because they are a toolbox component) they say that they are the same part. I am not sure why they are splitting them into two different item numbers.
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John Stoltzfus @ Mattew Stafford on Feb 6, 2017 2:45 PM
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Might be the same part but they are different configurations, I think there is an option for that when you insert the toolbox parts...
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Dennis Dohogne Feb 6, 2017 2:58 PM
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Two things:

1. Depending on how you have your Toolbox setup you can easily have different sizes and show the same part file. They would be different configurations of that TB part file such as a 3/8" and 5/16" size bolt. Even lengths will be different configurations.

You will eliminate a ton of headaches if you setup your own descriptions/part numbers in TB. Do a little research on these forums and within Help -> Toolbox Help to learn how to do this.

2. How do you have your BOM set? Is it set to show Parts Only or Top Level Only. It is not evident from your screen shot. That could easily affect how the quantities are displayed in your BOM.
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Vladimir Urazhdin @ Mattew Stafford on Feb 6, 2017 3:09 PM
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Click on left-upper corner of BOM. Expend Part Configurations Grouping. Mark "Display all configurations of the same part as one item".
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Mattew Stafford @ Dennis Dohogne on Feb 6, 2017 3:17 PM
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Thanks John Stoltzfus & Dennis Dohogne,
1. I will have to do some more research on setting up toolbox. It looks like a lot of people just use toolbox as a template for creating their own library. I suppose that is an option as well.
2. The BOM was set to " top level only", but I experimented with all the settings and still nothing.

Here is what I did in order to get it to work. I created a folder in my assembly tree (didn't know that I could do that) and placed all of the hex bolts of that length in there. According to the assembly tree, they all had the same name and were the same size (thread, overall length & thread length)..as far as I could tell anyway. Then with all of them selected in the folder, I then clicked on the size of bolt that I wanted. If there was a different configuration, I couldn't find it, but it works now. Thanks,
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Mattew Stafford @ Vladimir Urazhdin on Feb 6, 2017 3:20 PM
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I imagine there would be a good reason to use this feature somewhere, but when I have different length bolts I am using, I don't want to have them named the same thing. Thank you,
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Dennis Dohogne @ Mattew Stafford on Feb 6, 2017 5:06 PM
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SWX2017 added a new feature that I had been asking for for years, perhaps that is what you just did. In 2017 you can now select a multiple of Toolbox fasteners, RMB and select Edit Toolbox Components. This allows you to select a bunch of fasteners and make them all the same. In the past these changes had to be done one by one so this is a big help. In your case it makes it very easy to make sure they are all the same size and length.
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Dennis Dohogne @ Mattew Stafford on Feb 6, 2017 3:28 PM
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If they are the same size, but different lengths then those lengths will be different configurations so they will indeed show up as separate line items in the BOM, just as you want.
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John Stoltzfus @ Mattew Stafford on Feb 6, 2017 3:43 PM
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You didn't ask for my opinion, but I'm gonna give it anyhow - Don't waste your time with Toolbox, setup your own library........
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Mattew Stafford @ John Stoltzfus on Feb 7, 2017 5:00 AM
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I can see us moving in that direction in due time, once we get a little more familiar with the workflow in Solidworks drawings. I worked with U.G. NX for 16 years & it was beneficial for us to have our own library.
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Deepak Gupta @ John Stoltzfus on Feb 7, 2017 5:10 AM
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I've never been able to understand as why many users are against Toolbox. If it has been set up correctly and then locked, I see no reason why one should not be using it.
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Mattew Stafford @ Dennis Dohogne on Feb 7, 2017 6:35 AM
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So I played around a bit with the Toolbox settings under "Start"- All Programs - Solidworks 2016- Solidworks Tools and added a description under the 1/2-13 X 1 3/4 X 1 1/4 Hex bolt & noticed a few problems.. After I typed in the description 1/2-13 x 1 3/4" LONG HEX BOLT (in the red circled area), saved it and closed out:
1.) This new "description" is showing up in the "Price" column.
2.) When I closed out of Solidworks & opened my assembly back up, it reverted back to the previous BOM & did not save my new description.
3.) When I opened up the "Toolbox settings" the description I typed in disappeared.
4.) I understand that there is a configuration setting (see bottom attached image) to point to what is supposed to be called out in the BOM, but these are read only parts. I am assuming I need to get write access in order to get this functionality?
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John Stoltzfus @ Deepak Gupta on Feb 7, 2017 6:38 AM
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Like always everyone has their own opinions It is much easier and quicker for me to work with design tables and working with my own custom properties in the design table verses manipulating Toolbox components. Also like I said many times I did use Toolbox extensively and got burned big time with a Toolbox bug and I still shudder when I think back of all the projects I opened up and all my Toolbox components were ten times the size and the feature tree was lit up like a forest fire.
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Dennis Dohogne @ Deepak Gupta on Feb 7, 2017 8:53 AM
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I'm with you, Deepak Gupta. Once we looked into Toolbox we saw it as the most handy and reliable/consistent way to handle our fasteners. We have our TB on the network and everyone is pointed to it. Our part numbers and descriptions were easily imported from our ERP system so now when we go to insert a fastener we choose from fasteners already in our system. We can even export our BOMs from SWX to a spreadsheet for importing into our ERP system and they are complete with all part numbers and descriptions.

I'll admit that in its early days TB had some big problems, but those are well behind now. Sure, if TB were to be rewritten from scratch they would do some things differently, but we've been on it here since we bought SWX eight years ago without any problems.
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Dennis Dohogne @ Mattew Stafford on Feb 7, 2017 9:11 AM
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Mattew Stafford, The way we setup our TB is this:

We made a copy of the pertinent standards and named them our company name such as Company-metric and Company-inch. We then modified those standards with our part numbers and file names. We also checked/unchecked which fasteners show up by size and length. It is still easy to choose a fastener that we have not assigned a part number to, with the intention of adding that information once we are sure we are going to use it.

Perhaps because we are doing all this to our versions of the standard files it works for us as it should. To be honest with you, we set up our TB right away (it was pretty easy with import/export of information in spreadsheets). As a result, we have not tried to change the descriptions in the default standard libraries, though I would think you should be able to achieve that.
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Mattew Stafford @ Dennis Dohogne on Feb 7, 2017 9:13 AM
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I have looked over numerous threads and am still more confused than ever. My IT guy copied the Solidworks data folder over to a network drive, so that when I create, modify the parts, everyone will be working with the same data. As my last message shows, when I create a description for a toolbox part, it shows up in the Price column on the BOM. Is there something in the BOM I need to change? Or is it in the base part? Then there is a column in the BOM called manual exploded/QTY. I can understand the QTY, but where does the manual explode come in? and how can it be changed? Thank you for any help!
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Dennis Dohogne @ Mattew Stafford on Feb 7, 2017 9:42 AM
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Mattew Stafford
1. Everyone will need to have their TB directory pointed to the same location on the network.
2. I think it might be as simple as copying the whole directory that your TB had been pointed to, but you might check with your VAR to be sure (or perhaps someone on the forum with the right knowledge can supply the answer).
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Mattew Stafford @ Dennis Dohogne on Feb 7, 2017 9:55 AM
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I think that I am attempting to do something similar. We have copied the Solidworks data directory into a new location so that we are not modifying the base parts. Why did you modify the file names out of curiosity?
Like I mentioned, the problem I am having is that the BOM is not working correctly.
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Dennis Dohogne @ Mattew Stafford on Feb 7, 2017 10:04 AM
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You might not be setting up TB in the most direct route, by copying the directory to the network after you installed it, but I think that part of it should still work.

Copying the standards to our Company-metric and -inch was done inside of TB, not externally to it in Windows. Be aware of this.

All we did was to put in our part number and our description in the Part Number and Description fields. We did not modify any file names.

I fear you might be trying to get what you want by external manipulation rather than by using the built-in capabilities of TB. Keep at it, you'll be glad you did.
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Mattew Stafford @ Dennis Dohogne on Feb 7, 2017 10:11 AM
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Ok, I see what you are saying now. I guess that I am actually doing a little bit of both. Solidworks is installed on the local hard drive on each computer here, including the toolbox. I can add folders to toolbox internally, but it was only visible to me. I could copy everyone with the changes I make, but I thought it would be much easier if everyone accessed the same thing on a network drive.
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Dennis Dohogne @ Mattew Stafford on Feb 7, 2017 1:24 PM
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Make sure your network location of TB works. Outside of SWX rename the TB directory on your local hard drive so your SWX installation cannot successfully find that version, only the network location. Once you have closed/opened SWX and it is still pointing to your network location then make the changes to the fields you want in TB. Verify that hose changes show up in your BOM. To be safe, make a new assembly of just a few of the TB parts that you assigned names/numbers to. Create a BOM to verify the information shows up as you want it to.

Once you have setup your network TB to your liking then you can have everyone else point their installations to the network. I would also have them rename their local TB directories so their SWX cannot go look to the wrong TB.

Do not make the mistake of trying to have a customized TB on everyone's hard drive. This is too easy to get out of sync. You might add a fastener and someone else might change a description, but if these changes are only to your local drives then you don't have each others changes. Getting TB setup the way you want and pointing everyone to the one location on the network is the way to go.
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Stephen Bittner @ John Stoltzfus on Feb 13, 2017 2:07 PM
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Agreed! TOOLBOX has been a complete nightmare for us. Let the thread be a testament to that. I abandoned it years ago.
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Deepak Gupta @ Dennis Dohogne on Feb 13, 2017 2:35 PM
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Dennis Dohogne wrote:

Make sure your network location of TB works. Outside of SWX rename the TB directory on your local hard drive so your SWX installation cannot successfully find that version, only the network location. Once you have closed/opened SWX and it is still pointing to your network location then make the changes to the fields you want in TB. Verify that hose changes show up in your BOM. To be safe, make a new assembly of just a few of the TB parts that you assigned names/numbers to. Create a BOM to verify the information shows up as you want it to.

Once you have setup your network TB to your liking then you can have everyone else point their installations to the network. I would also have them rename their local TB directories so their SWX cannot go look to the wrong TB.

Do not make the mistake of trying to have a customized TB on everyone's hard drive. This is too easy to get out of sync. You might add a fastener and someone else might change a description, but if these changes are only to your local drives then you don't have each others changes. Getting TB setup the way you want and pointing everyone to the one location on the network is the way to go.
I would rather advise to keep toolbox files locally and avoid network glitches. But with that said, there should be only one master toolbox which should be on network and only one person to handle the changes.

And other users can keep their toolbox synced (one way) with network master toolbox using tools like GoodSync (it can be set to auto sync itself). Also user should create the path like on the network so that no glitches when opening files else where.
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Mattew Stafford @ Deepak Gupta on Feb 13, 2017 3:03 PM
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Good info all! I didn't even know that such tools existed. For now, I have done as Dennis suggested & things have been working good so far.
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Parts quantity not correct in bill of material

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