Hi,
I use DIN9861 punches all the time, and I would like to create a design table for this part and use the configuration publisher to make it more convenient to work with.
There are almost 800 different configurations for this part.
I am quite new to working with design tables, can this be done in a more efficient way than typing all the different configurations manually ?
Please let me know how you would solve this :-)
Once you go past a 100 to 200 items in a design table will slow everything down in your assemblies, (Depends on the complexity of the component)...
To go a little further on what John says.....Whenever I need to use an AS568 O-ring in an assembly, I save the dash number I need as a separate parts and use that just so it doesn't slow down my assembly at all.
Chris
I am glad I only did 35 different configurations, and not 800. Thanks for telling me.
What else can I do ?
Can I somehow add the design table to the ToolBox, and make it work the same way as when you drag and drop a bolt from the toolbox ?
Hello Victor,
I would change the naming convention for the configurations. The current one is long and has redundant info DIN 9861 Ø0,30x71. The configuration name is quite important, since it is used as an identifier in your assembly and should be kept simple, short and ideally without the use of special characters (very important). I would use a dumb number that easily sorts and use a $description column to add descriptive information. I would go with a configuration name that has a fixed length like XX.XX-YY.YY (00.30x71.00) without the Ø-symbol. Add DIN 9861 as a separate configuration property. You can concatenate the properties inside the design table if you want to show it in the format DIN 9861 Ø0,30x71. The fixed length will make sorting your table easy when you add different sizes along the way. I usually format the configuration name based on the feature dimensions. Say in cell "B2" you have the diameter 0.30 mm and you wanted to call the configuration name a fixed length of the diameter. I then put following formula into cell "A2": =TEXT(B2,"00.00") That way you configuration will always be 5 digit wide an 3.1 will show as 03.10, or 71 will show as 71.00. If you don't do that than your lists sort like 1,10,11,12,2,3,31...etc. instead of 1,2,3,10,11,31
Using formulas will make filling your design table easy and avoid data entry errors. A 3.0x71 wont end up being a 3.0 x 70 by typing error since your dimensions drive the configuration name. You can copy the dimensional values from a pdf table or the web and all other information will be automatically created via excel equations.
That are just some simple rules that can work for you.
Elmar
Thats not true. SW only uses an information from active configuration. I use a bolt with 1500 configurations with no lag, the file size is 150 MB.
Victor Fagerlund - be aware that unless you click on every single configuration in you part, you won't have the 3d parasolid data. Therefore changing configuration of your part in an assembly won't change the geometry of that part. Solution:
1. Purge all configurations in your part
2. Add save mark to all configuration. ALL
3. Run the attached macro, it rebuilds all configurations. Depending on your part and your computer, it may take from a few seconds/minutes, to a few hours. My bolt with 1500 configurations takes about 80 minutes.
4. Save your part
5. Make it read-only. Set your machine to not save read-only elements (close automatically without suggesting to save). Otherwise it will try to save the part every time you save the assembly.
Ben D. wrote:
Thats not true.
Glad it works for ya...
Apparently your files were not as complicated or your system is more robust...
I tested it also this way: I uploaded the part to windows shared folder and tried to open it from there.
The time it takes to load from SSD: 5 seconds
Time to read from shared folder: 12 seconds
Time to fully download the part to my computer: 42 seconds
This shows that data for only active configuration is loaded when using the component (otherwise it would take the same time to load from shared folder and to fully download it).
Maybe your problem is elsewhere, not at the number of configurations?
I haven't looked because I've got a 2.5 year old on my lap and am lucky to get a few sentences typed. If this pin is in TB, and I'll bet it is since it follows a DIN standard, then that alone is justification enough to use Toolbox.
If you must use a DT then there are ways to figure out the logic of the sizes and naming convention and just using Excel functions to populate all the cells and create the configurations. I use a simple function in the first line for the configuration name all the time that looks like this:
=&b2&", "&c2&", "&g2
This would make the string of the contents of the cells B2, C2, and G2 (in this example) separated by ", ". Easy peazy.
Hi Dennis,
Thank you for getting back to me.
This piece (DIN9861) is not part of the Toolbox it self.
Is there any way I can add this part to the Toolbox, and make it work the same way as the rest of the Toolbox ? I would like to get the ability to choose between the 800 different configurations when I drag and drop the part from the Toolbox.
SWX2017 added the ability to Rebuild All configurations and it even shows the "health" of each rebuilt configuration, i.e., an "X" if the configuration has a rebuild error.
Victor Fagerlund , I haven't added outside parts to TB so I cannot speak from direct experience. SWX help has always been very good, in my opinion, so I'd like to suggest looking in the TB help for this. I would look for it myself except I'm away from SWX for the next week so I can't.
I don't seem to have that problem ?
I have all these configurations that have not been ticked yet, and still I can choose between all of them in an assembly.
When I choose them in an assembly they will get ticked.
This way you will save this part every time you save the assembly. It is way more efficient to rebuild all configurations, and make this part read-only
The DIN standard in my 2016 toolbox has an o-ring already spec 3771. You can copy this part in the Toolbox Settings tool and call it 9861 then populate as you see fit.
Steve
I did a new part that consist of 500 configurations.
It took 45 mins to rebuild it.
But I can't open it, SolidWorks crash everytime I try :-/
If you still want to do this after all of the comments above, you could try to add an excel sheet to fill up the main sheet. You can initialize the part there, list the option for each setting and do something smart to create the first sheet. Use a macro if necessary.
Solidworks only looks at the sheet that was open active you closed the Excel file, so make sure you go to the main sheet before returning to Solidworks. The design table becomes corrupt if you forget, although you'll be able to fix it sometimes by reopening it and going to the right sheet again.
This was a quite simple part with a huge amount of configurations I did to see how slow my system would be.
Quite slow it turned out to be.
No, you are right, as mentioned in all the above comments, I wish I could do something else.
I wish I could add the parts to the Toolbox and control all the configurations through the Toolbox.
But I don't think it is possible to create a new part in the Toolbox environment with properties and configurations and make it work the same way as the standard hardware.
Take a 'Socket Head Cap Screw' as an example, it has over 9800 possible configurations, and the desired configuration is created the moment you drag and drop it. This works perfectly.
I have a lot of hardware I use on a regular basis that each would consist of hundres of configurations.
I wish these parts could be a part of the Toolbox the same way as the rest of the standard hardware.
Hi Victor,
Your problem is the number of configurations. If you have all configuration available through the drop down list, then you run into the rebuild and memory issue. As you have found out itself. So forget about this approach. Make a copy of your toolbox part instead and place it into your project folder. Then generate only the configurations that you need. This approach has its pro's and con's obviously, but it rebuilds fast and can use all the advantages of toolbox items.
In the end you will spend time designing your things. The idea is to minimize that time. This approach will work for you if you want it to.
Elmar
I am not sure if you saw my post above. It may have gotten lost in the middle. You cannot add brand new parts to the toolbox and have them work properly. You can, however, copy an existing toolbox part, rename it and use it as you want. My DIN standard in 2016 has an existing o-ring in it. If you have SW2016 you should be able to go into your Toolbox Settings tool, copy the existing o-ring to your standard and populate it as a toolbox part. I have done this many times with good success.
Steve
Hi Steve,
I am looking into this right now, unfortunately there are no existing hardware in the Toolbox that will be similar to a DIN9861 I can copy.
I guess it will be too difficult then.
Hi Victor,
Not sure what Steve means by "you can not add brand new...& work properly". You can indeed add custom parts to your toolbox.
They will show up in your toolbox browser (drag & drop and insert functions work incl. selecting configuration). They are listed as part but the configurations are not displayed (see image below). That however doesn't stop you from editing the toolbox item by itself and make the changes in the design table.
So the basic idea is to create your part with all configurations. Use a design table to add your properties and sizes. Then add the part to your toolbox. I have the Size table on the second Excel sheet and the configuration info on the first sheet. All cells on the first sheet are linked with lookup formulas & drop down lists to the Size Table. I add a workbook macro to make sure the first sheet is always selected before closing the Workbook (Sometimes I need to add a size to the table and SW throws an error if you forget to activate the first sheet before closing the Workbook). If you need more sizes then you just copy down the formula on sheet 1 and select another size.
We do all formatting and part identification in the table. Part numbers are linked to file names and update automatically.
Private Sub Workbook_BeforeClose(Cancel As Boolean)
' This macro automatically runs when the spreadsheet is closed
Sheets("Sheet1").Select
End Sub
Size Table:
Configuration Sheet with lookup formula in cells
Victor, I always face problems with Solidworks when working with large spreadsheets, containing dozens/hundreds of configurations. You just have to deal with it. Some advice:
1. When creating a part/assembly with lots of configurations, firstly write everything to a separate excel file, instead of putting data directly into "Design table", which is embeded and opened from Solidworks. Then it will never crash.
2. Secondly (continuation from point 1) , if you make a syntax mistake in the spreadsheet (for example if you mistakenly write comma instead of dot to separate the decimals), then SW will usually delete all spreadsheet data below that syntax error. Having all data in separate file saves you from losing data.
3. Before pasting data from separate excel sheet to SW Design table spreadsheet, make backup copies of separate excel spreadsheet and the part file. Quite often I get the error "Range out of limit" or something like that, causing to crash both Solidworks and Excel.
At the certain time in the past I spent lots of hours getting around these bugs and searching for workarounds. Please read this my thread for some more advice:
Thanks for all the replies.
I did that to some of my custom hardware, setting everything up with a design table.
But when I insert one of my custom hardware that I added to the Toolbox, the dialogue will look like this:
I wish it was possible to get all the information like you do when you insert standard hardware.
As in this case when you insert a bolt you will see the sizes and lenghts.
Victor.
I don't see an easy way around it unless you can cut/paste from a table. I did a model for an AS568 o-ring with all the different sizes and I cut and paste a lot of the info from tables found on the web into the excel design table. Not sure it will help but take a look at the attached model to see how I did it with the tolerances as well.
Chris