configurations and file management

[aferro]

hi to all of you

this is a strange question.. i'm finishing the library of materials for a company, and i have a doubt on how to proceed for a part..

this company uses metal tubes of different measures long (from 120mm to 1800 mm in 50 variations), with 3 different diameters (13,17,21) and 3 different combination of threads (a,b,c)..

my solution an unique file, with all the (450!!!) configurations inside, so they can change it in the assembly when they are drawing or using a template assembly.. but it's a 50MB file, and i'm sincerely not sure that is the best solution managing great assembly (even if i didn't have any problems in situation like this in the past)

the tree is this one:

9802.130-.0000
9802.130A.0000
9802.130A.0120
...
and so on...

according to you which is the best solution:

- the one i go with
- 3 files (one for 13, one for 17, one for 21)
- 3 files (one for thread A, one for B, one for C)

as i wrote.. this time i'm not sure this is a good deal......................

thanks in advance for the suggestions!

Alvise

 

[NomLaser]

Break it into 9 files.

13A
13B
13C

17A
17B
17C

21A
21B
21C

Then vary the length with configurations. It will be much easier to manage than having 150 configurations in each diameter. This way you only have 50 and they are just the length that changes.

 

[CorBlimeyLimey]

How many tubes are used per assy?
How are the part numbers being handled?
Does the company use a PDM system? If not, do they have plans to?

I would probably opt for multiple configs in which only the length varies.

 

[Russell67]

Personally i would go with one file with configurations for each dia and use configurations for the lengths. This way as they replace parts within the assembly all the mates will follow.

Keep in mind that if you are using a PLM tool that if they need to add items between values that this may require a revision for as they are added.

Another solution is to create a tabulated drawing and as they need parts they do a save as from a master part. Helps to prevent someone from forgettting to make sure they have "this configuration" option checked when changing dimensions. Also if htey do that then the mates follow as well. Also eliminates creating lengths that may never get used.

 

[CorBlimeyLimey]

Russell67 brings up an important point regarding mates. Make sure each tube version is created from a common file so that the face ID's remain constant. That should eliminate/minimise mate problems when replacing tubes.

 

[NomLaser]

Basically what CorBlimeyLimey is saying make the 13A with all of the configurations. Perform a SaveAs and save it as 13B. Make your changes and save it then perform a SaveAs 13C. Make your changes and save it. Then another SaveAs 17A...etc. This way the surface ID's all stay the same and you can easily swap out the files and not break the mates.

 

[acavite]

I think I'd create 1 master file with 3 configurations for each thread set and use a top level "Settings" sketch that controls the Dia and Length settings. Right click, edit sketch, change od, change length, save, choose thread, done.

This file should easily float around 1mb... probably less since the part seems rather simple.


One thing I have noticed... when working with design tables and configurations and making lots of changes, the file size tends to get padded. I made a fitting model once and it ended up at over 6mb, which was unacceptable for something I'd be making copies of for each job that called for it... and then I made a copy and it was only a 600kb. It seems to store all the changes you make in the file, but when you copy it to a new file, it just takes into account what it is currently and not how it got there.

 

[SteveJJH]

If you do decide to save a part with loads of configs (which i don't think i'd recommend) make sure you turn down the "shaded and draft quality HLR/HLV resolution" slider under document properties, image quality. that should make the file size much smaller

 

[ZillionM]

If you use "save as", the file decreases dramaticly in size. You can repeat this by opening the "saved as" file and use "save as" again. You can do this until the file doesnt decreasing anymore. This way, I turned a 80 Mb file into a 1.4 Mb file, and it still works fine. I dont know for sure its gonna work for you, but you should give it a try

 

[aferro]

Hi to all of you, sorry i'm posting late (my wife began works, so i'm 50% a technician and 50% a baby sitter, full time in the Weekend!)

CorBl. :
- usually 1 tube per assy
- i can decide the part number
- no, there's no PDM, maybe in 2/3 years they'll have one, but depends also from the production software and from the production manager

so... after a lot of time i decided! 1 file, all the configuraqtion in that file.. because they have an assembly template, and they change on this template the parts in order to configure every assembly (it's a lighting company).. so as CorBl. said, there's a lot of chances to avoid mates problem

but i prepared also the files.. let's see what will happen, THEY have to decide working on what to do!

btw, as u suggested i made a save as... from 60 MB to 1 MB (!!!)... my Solidworks VAR said me about this probl 1 year ago, but i thought it was only a 2008 Bug!!

 

[aferro]

and, obviously...

THANKS !!!

cause i sincerely appreciate all the help you provide!

Alvise

 

[ZillionM]

lol! a bug..
I wish we could have those kind of bug swarms in our solidworld

anytime

(im sry. maybe a little oftopic here)