Use of Family Tables, good or bad for computer resource requirements?

[fsincox]

I have been discussing this issue with my colleges and there seems to be a diversity of opinion. Does anyone have the formal SolidWorks position on this, or know and can share.
Does using large family table of parts (fasteners) require more resources because the tables may be large or is it somehow more efficient?
Thanks, Frank

 

[JMirisola]

If you're talking about configurations, then yes, using configurations uses up more resources. It's not so much a 'formal' SolidWorks position versus a reality. A configuration laden file is much larger than a file without configurations and opening/having open such a file uses more resources.
That all being said, depending on your computer's power, as well as the manner in which you're utilizing said file(s), may render the whole issue moot.

Jeff Mirisola, CSWE
My Blog

 

[Updraft]

I have not done a formal comparison, but recall something to the effect that a file with ten different configurations would be slightly smaller than the sum of those ten configurations if they were saved as individual files, for instance. The advantage of configurations is two-fold: shared/similar part definitions, and convenience in changing configurations. The disadvantage is the files can get large, depending on the number and complexity of the configurations.

Since you are talking specifically about fasteners if you were to have a file with a Design Table (the correct SolidWorks term) it would be very easy to populate the file with all the different configurations and descriptions of the fasteners for a given type. It would also be very easy to change the use of a fastener in an assembly. For instance, say you have an M4x20 SHCS and you later decide it should be 25mm. it is a very simple matter to change that fastener from the 20mm to the 25mm configuration with a configured file. On the down side, if you are using only one or two different fasteners in an assembly you are now accessing what could be a large file.

Like anything there are trade-offs. For fasteners I would recommend the configured file because the benefits you'll love while the slightly slower access of a large file you'll hardly notice. Just think of how much more difficult it would be to change fasteners as in the example given if the two were separate files.

With all that said, however, we use Toolbox for our fasteners. Once you learn how to properly set it up it is a real benefit to use.

- - -Updraft

 

[ShaggyPE]

To add to what Updraft stated, I would recommend a hybrid approach. Configured hardware (driven by a design table) where there are separate files for a given screw diameter. Example: M4_shcs.sldprt would contain every length of M4 socket head cap screw. M5_shcs.sldprt would contain every M5 length. In this case, changing lengths is as simple as changing configurations. If you want to change the screw diameter, you have to do a replace part in your assembly. Since the parts are all based off of the same original donor part, no mates are broken. Changing the screw size is slightly more tedious than changing the length, but generally when designing, you change the fastener size less often than the length.

Just my 2 cents, having used 1000+ configuration design table parts in the past (where only a couple are ever used).

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[BiPolarMoment]

...a file with ten different configurations would be slightly smaller than the sum of those ten configurations if they were saved as individual files

A bit off topic but you just inspired me to search and there is actually a way (at least in SW2013+) to purge the cached configuration data to reduce the file size of configured parts further. This is interesting to know since that has often been a hang-up of mine when it would have been much more efficient to send a smart SW model rather than many dumb ones. Here's a link for the curious: Managing Configuration Data

 

[NTME76249]

What i would recommend depending on your possible configurations is to use a design table but keep it to only 2 configs. You can drive multiple tables in a design table that all feed one configuration. Put in some simple validation lists and you are good to go. This is not a good approach if you only have 10-15 possible configurations but if you have more than that it may warrant the time setting up the design table.

For example.
I deal with pipe in my assembly's. everything from 1/2" to 36" in every schedule possible. And also different materials for some.
I can have drop downs on "Od", Sch" and Material. My design table will pull Od, thk, material, description, part number and anything else i want it to determine from lookups and such.
it all feeds in to one configuration. If i know that i am using 5 or 6 different pipes in an assembly then i generally set it up with 10 possible configuration that auto fill as i make my selections.


Michael McMillan, CSWP

http://www.linkedin.com/pub/michael-mcmillan/53/375/52b

 

[Regret]

If you had Creo, you could use accelerated files for family tables and manage the way instances are used, incurring no performance deficit. Solidworks and Inventor have no such functionality.... As for CATIA family tables...

 

[Agriego]

I'm new to Solidworks, so I still have a LOT to learn, but this is what I've been doing for standard parts. In order to keep my part configuration files from getting too big, I break them down by thread size and material for screws/bolts. For instance, I'll take a fastener like MS27039 pan head machine screw, and do a separate configuration file for the different material types, and depending on how many different lengths are in the part table I either do them in one file or break each thread size down into its own configuration file as well. That seems to work okay so far. Now I haven't heard of Toolbox, and I can't find anything about it on my system. Is that a separate add on? I don't think we bought it.

Al

 

[patdh1028]

I have used huge configured files and still do. I have one file, it has pretty much all possible 18-8 metric socket screws. Socket-head, button-head, flat-head, low-head. All thread sizes from M1.6 to M40 or something. The file is ~5MB. The original part with no configs is ~400KB. Once you're working with more than 12 unique fasteners, the configured file is more efficient from an IO standpoint although it takes a lot longer to rebuild. I would never go back to separate files, personally. The custom properties mean that everything is uniform and I can make changes to the custom props in the central file and have it immediately propagate across all assemblies (of course with many kinds of parts that's a huge liability but in this case it is desirable). I've put a lot of work into the files and now they automate all kinds of manual processes and make our BOMs extremely thorough without relying on engineers taking the time to manage metadata. I make my own configured files for all kinds of family-table parts from Misumi and other suppliers as file management is much simpler and it's a one-and-done process of metadata management. People get used to having the configs available so they don't look for new suppliers or sources for the same stuff, we can let purchasing handle that. So even though there are many cases where the computing performance takes a hit, I think overall efficiency is much higher.