Materials & Weights for Toolbox parts (to BOM)

I'm working on a standardized BOM system for my company.

For now it looks like I'm stuck using the Toobox, warnings from others
notwithstanding.

Is there any way to designate a material for these parts once brought
into an assembly, and a weight property similar to other parts?

I've come up with a pretty straighforward BOM system, but the inability
to designate these two properties for my fasteners has me buggered.

Well, that and the fact that I can't seem to find a way to get a
default description for a class of fastener (such as "HVY HEX NUT" for
Heavy Hex nuts). And the part numbers provided are stupid, which means
you're editing these as well...

But I think I can live with that if the material & weight issues can be
addressed.

Thanks,

Tom

 

Tom,

You can apply a material to the toolbox parts by browsing out to the
location of your toolbox item. But before opening it remove the
read-only properties to that you have right acess. Then you can apply
the material like you would with any other solidworks part. Save it and
then make sure to put the read-only acess back on. You can also use
this method to put specific properties in toolbox items also. There may
be an easier way but this is what has worked for us.

If you want to have a custom description and part-number for your
fasteners you just need to right click the fastener in your assembly
and select Edit Toolbox Definition or when bringing in a new tool box
item it will give you the same screen. You can select the radio buttons
to list by part number or description. Then click Add. This bring you
to another screen where you can give it the custom description and part
number. However keep in mind that toolbox will not allow you to assign
the same part number for a different screw for obvious reasons. We use
an acess database to keep track of part numbers otherwise it could get
kinda confusing.

Hope that this helps!

Jon

 

Jon:

Thanks. However, I don't want to overwrite the original part
definition, so what I think we'll do is save the part to he directory
tree of the project, and then assign the properties to the copied out
part. This allows us to choose between say, a grade 5 fasteer and a
grade 8. Part no's don't really work with us, but one stupid thing
about the way they do theirs is taking up three part numbers just to
designate a different thread display! duh...

Tom

 

Tom,

I know this won't help your immediate problem.....but.....

I've had an SPR issued that will allow the same part number to be
issued to identical geometry.
Also, I've got another SPR regarding the ability to import
configuration properties using the toolbox import function.
And the third item is to follow the ASME naming convention when filling
in the description of the fastener.

Len

 

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This switch has existed for years. Where'd you get an "spr" number
from? Toolbox menu, Browser Configuration, Part Numbers, "Allow
duplicate part numbers for geometrically equal components"

Hmmm, you can do this too. Tools, Options, Data Options, then select
some part type in the window on the left, then you have to scroll the
list of tabs on the right all the way over to the far right, and select
"All Configurations", hit "Export" and it puts out an Excel file of all
the data, but not in a Design Table form the way it might be useful, but
anyway you can put property info in and reimport. I agree that this is
pretty obscure, but this is exactly why we need to get away from a
database for toolbox.

 

Matt,

Having the switch and working the way its suppose to are two different
things.
I had a nice 1/2 hour converstation with SW technical support last week
where I was able to demonstrate the problems.

They did additional tests and determined that there were issues that
needing corrective action.

Hence the SPR's to "fix" the existing functions.

As for Toolbox being in a database form -- there is nothing wrong with
this type of implementation if it is done correctly. The sad part is
not a whole lot has changed since Toolbox was purchased from Cimlogic
years ago. Its another one of those SW applications that marketing says
is "close enough" --- with the resulting productivity hit by general
users who then have to fix or try to work around these fundamental
flaws.

This is a prime example of why programmers and marketing types should
have to use the program in the "real world". One or two days of putting
up with this "BS" would have these problems corrected in no time.

My toolbox pet peeves:
1. Why does SW think that nobody will ever assign a material to a
fastener?
2. Why does SW think that nobody uses o-rings, snap rings, or star
washers?
3. Why does SW think that nobody will ever need to order fasteners from
a BOM where proper callouts are needed (Take a look at configuration
names). Machinist handbook has standards for nomenclature as well as
ANSI/ISO standards for proper fastener callouts - why not use them?
4. I really don't care if I represent a fastener using simple,
detailed, or schematic representation - they all need to be called the
same thing and use the same number.
Why does SW think we are putting hardware in an assembly?


Len

 

Len, My pet peeves are yours, you really nailed it, and Matt thanks
again for you input & insight.

To the software guy, well, I understand you're just like me, out there
trying to make a buck. It's probably a good program. ButVER, EVER
EVER tell me a piece of software is "zero effort." NEVER. Don't do
it. Can't happen. Further, when you've been at this as long as I
have (and I know how to keypunch, pal), you get weary of performance
promises, weary of having to buy (and configure, and learn) yet another
piece of software that will have to be kept up alongside Solidworks,
when, for the love of God, this very basic, very pivotal functionality
should have been there from the get-go. God knows they want enough
money for it. 3 stinking CD's full of code and the biggest problem with
it is the most important part.

For Pete's sake, there's any one of an number of programs that will
make pretty shaded 3D geometry. And I'm the FEA guy here, but so what
about CosmosWorks? If I'm off 1000 psi, it's probably no biggie. But
at the end of the day, I have to have a drawing with a bill of material
that's spot-on corrrect.

Sheesh. Happy Monday everyone. </rant>

Tom