Huge screws!

....to borrow a phrase I read in Matt's site.

Just ran into this one. I guess I'm hitting them all!

What were they thinking?

For me it's a matter of perceived value. The value of a work of
engineering. Hours, days, weeks, months. Lots of time, money, thought,
consideration and study goes into these works.

Given that, the very tools with which we document and create these designs
must not conspire against us. The unique ability that Toolbox has to damage
a design if used as delivered is simply a failure by SW to place any value
on their customers work. For this is the only way one could consider
designing a system that would allow such a grotesque alteration of a design
to take place.

Design data integrity must be a fundamental guarantee of a high-end tool.
The design must be a solid unit that can survive transport and archival
without having to resort to error-prone manipulation. One such example is
using the "copy" option in Toolbox; appending these files to any archive or
transmission and later having to recreate a structure just to be able to see
the design without missing parts or distortions. Not only is this a mess
that is unreliable (it might not survive an employee leaving, for example)
but it is prone to such basic issues such as file naming collisions and
other tragedies one can think of. There are examples of this type of
problem with other tools. One that comes to mind with ACAD is the image
issue. ACAD saves absolute paths to images used in drawings. All you have
to do to break such a drawing is move the directory from drive C to drive D.
The only fix is to manually tell the program where the images are.

Gotta love it!

I'm adopting a tip I saw while searching the NG's archives for this problem:

Insert all the Toolbox parts you need.
Select a representative or each part type.
Open it.
Use "Save As" to save it to the design directory.

Now it's a permanent part of that design. The whole directory could be
zipped-up and moved to the other end of the planet with a reasonable
guarantee that a 4-40 nut won't turn into one used to fasten tires on 747's.
The good news is that you only have to do this once per part "family" due to
configurations.

-Martin

 

Our department is in the process of converting to Solidworks. I am
the one highly experienced CAD guy in the department and definitely
have had some bad experiences in the past with Autocad and directory
structures for images and x-refs.

But, I personally, am not on solidworks yet and therefore do not have
the knowledge to advise the department on how they should handle thinks
like this. Thanks for the heads-up on this issue.

Am I correct in understanding your recommendation as follows;
- All files related to a particular design should be contained in
one directory (and/or sub directories)
- It should be taboo to reference components in any kind of shared
directory.

But perhaps such standard parts as bolts could be handled by keeping
the shared component directory exactly as it was when the program was
first installed, and making it a read-only directory. Is this
possible, or does the toolbox need to be writable for some reason?
Would you recommend this approach?

Joe Dunfee

 

We don't use Toolbox here (wasn't used when I arrived) and instead have a
common library of hardware, etc. on our Z: drive. This way we don't have
any Toolbox issues - all standard nuts, bolts, washers, etc. already exist
as configs of part files, and the existing parts don't change - only add
configs for unusual stuff not already there. We also have a library of
purchased parts models so we reuse them from a common location, rather than
hunting all over to try to find the last place we used it, and then having
multiple copies.

WT

 

WARNING: Please, do not take what I say as "recommended practices" or even
absolute fact about SW. I have 20 years experience with ACAD and about four
months, a class, a bunch of tutorials and a couple of designs with SW. I
am, most definetly, not the person to look up to for recommendations. There
are real experts on this newsgroup who can help you. I'm sure they'll pitch
in.

It is clear that, as any new tool out there, SW requires learning. Part of
that learning has to do with letting go of what you know and shifting your
thinking to best utilize the new toolset. For example, today my VAR
suggested a neat trick that involves using the cavity tool to have a part
punch holes in another part without having to resort to piles of external
references. I think I can safely say that I never would have thought of
this independently.

Anyhow, make sure that you listen to experts advice. I'm just a newbee
relating some of my experience and frustrations in hopes that it helps
others and, of course, to help me learn about the errors in my own ways.

-Martin

 

Having said that, I realized I didn't elaborate on what I posted with
regards to Toolbox.

It's very simple really. I don't need to work on highly complex designs.
Mostly electronic devices to be mounted on standard 19 inch racks. In this
context SW will be used to design sheetmetal and some of the plastic parts.
In more general terms, to model the various sub-assemblies for form, fit and
some function (doors, slides, etc.).

It is clear that my needs out of toolbox are simple. A few fastener types
per design. Nothing fancy. And so, I've decided to opt for avoiding the
whole issue of Toolbox building parts on drag-and-drop and require that all
designs have all parts needed for the design within the folder structure for
that design. For example:

Widget1
Front panel (a part)
Keypad (an assembly)
Buttons
Knobs
Etc.
Chassis
Cover
Fasteners

The Widget1 project survives the test of time and place (for the most part).
You should be able to move it from computer to computer and even send it to
vendors and have all parts come-up as per the original design. No need to
worry about whether or not Toolbox is installed and where/how/when/if a
certain part and/or configuration was built. In other words, the file
package is a true description of the whole design with the only caveat being
that you might have to use the same version of SW to open it as that which
created it. Maybe the addition of a plain-text "Readme.txt" file at the top
of the hierarchy could be used to communicate such things. This approach
should also survive hardware upgrades and even changes in engineering team
makeup.

Yes, it replicates parts from design to design. I'm willing to accept this
in exchange for the freedom and independence this approach provides from
software, computer, network, etc.

I don't know how PDM might modify the above.

Hope this helps.

-Martin

 

Hi Joe,
As response the following:

The toolbox on the server has to be made read-only. When someone add a
configuration, the status will be changed to write-access and then back to
read-only. For the correct toolbox installation see:
http://files.solidworks.com/supportfiles/Toolbox_Multiuser/2005/English/toolbox_installation.htm

We also use our own common parts from directories on the server, but when a
project is finished, we make a copy of the project with Solidworks Explorer
to a new directory with "copy children" enabled. So all common parts and
bolts are inluded into one directory (The drawings have to be copied
seperately). Then you can use a program like EcoSqueeze to reduce the
filesize. In this way you aren't depended on future changes in directory
structure.

\/\/im

 

I re-located tool box to the server, and have inserted our common used
parts, micro switches etc.. into the tool box.
The only time I had 747 wheel bolts, was when an assembly was incorrectly
saved, without the file references and then opened on another PC.

This also applies to, any assembly, that uses parts located in a different
directory.
The easiest thing to forget, is to use the find references and copy the
files from there, (even preserving the directory structure if you wish), and
not from the windows or solidworks explorer.
This way, you to can take the whole assembly home with you work on it , add
more bolts and then take it back to work, where the toolbox definitions are
updated with the new data.

 

Absolutely the best way to go! We started a long time ago creating standard
purchased parts, and common components. We took the extra few minutes then
when we created lets say, a 4-40 nut model to add a design table and enter
in the rest of the B18.6.3 data into excel chart. Keeping that mentality
over the last couple years has helped build an enormous flexible base of
parts. (A good example of this is our NHBB ball bearing standard. It was
set up very nicely so that even if we need a bearing we've never used, we
just enter the mfrs p/n in design table and it generates the model ) We
used to have a macro for bringing in the parts, but the need was eliminated
in 2005 with the addition of the design library. Now, all standard parts
were relocated in the design library, so we just have to drag and drop into
the model, choose the config and we're done. Anyway, totally agree with
Wayne here....

Scott

 

On the subject of purchased parts. Which vendors and products do you
recommend?
I'm talking mostly about fasteners and the like.

-Martin