Correct me if im wrong, but creating a model in SolidWorks the way
manufacturing will build it is NOT the correct way to model. I say
this because im trying to figure out the best way to handle my
problem. We dont use a unique numbering system, so all of our part
numbers are sequential. If I am making a frame weldment with 8 legs,
and the legs have 3 bearings on each leg, I make an assembly with the
leg, bearings, tubing caps, and spacers the bearings mount to. Our
manufacturing dept doesnt weld each leg separately, rather they like
the entire frame weldment on 1 drawing with all components called out.
If I designed the model like this, I would have to mate 24 bearings,
caps, and spacers for each leg. Of course this is a headache in
SolidWorks. With our current system, I have to generate a part number
for this "imaginary" assy/weldment of the leg. This takes a part
number up, plus it! might confuse people in the future who didnt
create the model.
Can you give me your opinions on what the best way to go about this?
What does your company do for this? What is the "best practice" for
Any comments/suggestions greatly appreciated. Thanks.
The answer seems simple to me, but since it seems unlikely that a simple
answer hasn't occured to you I presume that I'm probably missing
something. But here goes anyway . . .
Why do you need to assign part numbers right up front while modeling?
If you were to use descriptive names as a preliminary, then you could
model up your subassemblies in the way that is most logical for
Solidworks (creating your Mates as appropriate), then once you have your
overall assembly together you simply Dissolve the subassemblies and
number the parts logically as your manufacturing will build it. So --
tell me what's wrong with that. I'm sure there must be something.
I should have mentioned that we use Smarteam, and we need to assign
the model a part number when checking the models into Smarteam. I
could of course check it in as "Leg", but then I would have to make
sure those are deleted later.
On Sat, 15 May 2004 22:00:20 -0400, Sporkman
I agree with Mark's suggestions. Using assemblies and sub-assemblies for
grouping and mating, then dissolving them later works good.
Also, When I'm designing a new project, I work strictly off my hard drive. I
use descriptions and date codes for part numbers. When the owner wants to
see the latest, I show him what I have, and the date code helps to
distinguish it from a previous version.
Only released documents get checked into the vault.
Devon T. Sowell
Well, I work in a team with 5 people. We are all working on the same
major assembly, so we need to share files. Thats is the main reason I
have to check files in, so others can use them.
As for dissolving mates in "imaginary" assemblies at the end of the
design stage, what happens if you have to change a part in those assys
that were resolved later on?
On Sun, 16 May 2004 06:08:57 -0700, "Devon T. Sowell"
I'd suggest maybe that your organization's priorities and your own
negative approach to problem-solving are what are getting in your way .
. . not the way SolidWorks works. If you've got to share portions of
your design before the design is finished then you're going to run into
problems no matter what software you are using. That's certainly the
reality in a lot of companies and a lot of design work, but I really
can't imagine how a software company can solve those problems FOR you.
Can you? I CAN imagine how YOU can make changes to make things easier
for yourself, however. Can't you?
Regarding having to change a part in the bogus assemblies after they are
dissolved . . . I'd simply delete the outdated components and replace
them. Use the original Parts and modify them if possible, and in that
way you'll run into only minimal problem with Mates.
I don't mean to be hard on ya, Mr. Monkey, but aren't ya coming up with
objections to solutions without trying to adapt the solutions to yer
needs? If your project managers insist on seeing major assemblies
together -- the result of the work of several people modeling separate
portions of a project -- you must simply educate them in the realities
of the software or find a way to share files without causing problems.
Or both. In one such scenario I can imagine you assign a valid system
part number to the major subassembly each of you are working on, and
that part number doesn't change. When you draw together the various
portions of the project in a top assembly you can simply use the Replace
function and the top assembly updates accordingly. If you wish to have
a contiguous block of part numbers for each portion of the top assembly,
then assign blocks of part numbers to each designer. If your company's
internal processes prevent that then call a meeting to discuss the
problems. Be creative my friend. There are solutions all around you,
but you won't find them by saying "yes, BUT ... ".
Mark 'Sporky' Stapleton
Watermark Design, LLC
In an assembly, sometimes I'll create a temporary assembly to group
components that are locally positioned properly. Then, as a group, I'll move
them to their new location. When the design is ready for a BOM, I'll
dissolve this sub-assembly.
I always fix every component in place and delete all mates when the assembly
is finished. I use mates less and less as time goes on. I prefer to move
components into position.
I too, have worked in large teams recently. We decided that only released
documents would go into the vault. We used date codes and each persons own
initials to identify each persons components. The team leader's computer was
made available to all team members and he was responsible for maintaining
the master assembly. This method works quite well for us and avoids the
hassles of using PDM Works unnecessarily. We got used to using SolidWorks
Explorer and found it to be quite adequate.
Devon T. Sowell
So, here's another example, this is how we really work.
Say there is a component called widet-1.
Say we want Devon, Tom, Owen and Chris to work on this part, each person to
submit his own design..
Same part, different names, no problem. During the week, each designer
submits his design to the team leader. The team leader inserts each part
into a copy of the master assembly and then decides which design is the
best. When the decision is made by the team leader, he renames the "winning"
part to the correct name.
We also use this method for assembly and drawing files. We use SolidWorks
Explorer to copy and rename drawings, assemblies and parts into new folders.
Devon T. Sowell
Thanks Matt and Sean-Michael Adams for the response. I felt like
Sporkman was giving me a hard time, maybe he doenst understand PDM? I
should have responded sooner, but been busy. I stated we work in
teams, but we dont compete to see who has the best design. That
sounds a little silly to me, but its most likely because we would
never do that here (i could see that being the way at companys who
design products around customers ideas). Each person on our team gets
a section of the project, for example, 1 person gets the frame,
another the housing, etc.
Back to the subject, as stated, part numbers are cheap, we wont be
running out anytime soon, thats why we use the system that we have
now. I have tried changing part numbers later in the design, and what
a pain in the azz it is with Smarteam. I will keep some of the ideas
in this thread in mind.
Keep the opinions coming :)
Let me just offer a different point of view. The other suggestions have
their merits, but may also have some drawbacks especially in light of
you using SmarTeam.
I think sequential part numbers are good, in fact, with a PDM system,
they're almost essential. If you don't use them, there's a lot of
maintenance that you'll have to do later with the names. I don't see a
problem with what you're doing there. PDM systems work great with
custom property description information. If you're dealing with a PDM
system, changing part names is not a game you wanna get into.
Also, don't worrry about something "taking up a part number", cuz
numbers are cheap, and if you have a good system, you won't run out in
the next decade or so.
You're right to say that you don't always model parts the way you
manufacture. I think you'd also be right to say that you don't make SW
assemblies the same way you assemble on the floor, although it's nice if
you can. If the end product that MFG sees is a sheet of paper, then who
cares how the SW assembly was built? If you use the SW BOM on your
drawing, just tell it to show the parts only, so every part will get its
own part number in the top level assy. Assign a prefix or suffix for a
part number to designate a "phantom". Certainly you have other
assemblies that use parts that don't get shipped to a customer, like a
model of a screwdriver to show how/where an adjustment is made for
service / documentation purposes.
Dissolving sounds like a good solution, the only problem being what to
do if you now want each leg to have 4 bearings? It limits the
editability in the future.
Also, what do you do if you start using the SolidWorks Weldments? That
may complicate things some, because the weldment is created as a
I wanted to ask if you could expand on this a little. We're about to
implement a new part numbering system without PDM but we should be
prepared if it's something we add later. I've been reading this
newsgroup a lot lately and you've always got good comments so thanks
I do PDMWorks implementation for a living, among other things. I get to
see how a lot of different companies do things. The customer in the end
always makes the decision about part numbering, but I try to guide them
by laying out strengths and weaknesses of various scenarios. I try not
to give my honest personal opinion unless they ask, or if I see that
they're doing something which is plainly stupid.
Definitely don't put the rev level in the file name. If you do this,
you will create a file management nightmare. The only exception to this
which might not be all that awful would be to put the rev in the file
name for archived docs if you are not using a PDM system. Use "Save As
Copy" or SW Explorer for this.
Everyone prefers to have file names be something readable, which has
some sort of meaning. The only problem with this is that you are likely
to make duplicate names, and "unique file names" is the #1 rule about
SolidWorks file management. If you can use "descriptive names" and
guarantee unique names, more power to you.
Another problem with descriptive names is when the function of a part is
used in the name, and the part is used in multiple assemblies where the
function may be different, for example a "locating bracket" may be used
as a "support brace" somewhere else. Project names in the file name are
not a great idea either because some parts may be used in multiple
I have some people take the information that descriptive names and
project names are not good to use individually and somehow come up with
the idea that it would be ok if you put them together to make the
filename. Don't fall down that trap.
I have seen people choose to put the designer's name in the file name.
That's useless, in my opinion.
Really, the file name is not for the user at all. The file name is for
the OS and the software that is using the file. Especially with
SolidWorks, you have the ability to use custom property information
which helps you identify the associated text-based, non-geometric data
that goes with each document (part, assembly, drawing). Stuff like
"description", "material", "finish", "vendor", "process", "make or buy",
etc. is all information that needs to be associated with the part, but
should not be part of the file name.
Why does the government know you by your SSN#? It's exactly the same
answer. The database is keyed on a uniquely identifiable number,
specifically because there may be 1000 other people in the country with
your exact name.
My opinion is that the file name needs to be something uniquely
identifiable, and the best way to do this is to use some sort of
sequential component to the file name. It is ok to use a bit of a
prefix or a suffix to briefly identify the function of the document, but
this should be minimal. Something like XX-12345 where XX denotes some
function (part drawing, assy drawing, model, work instructions,
schematic, test results, etc), and 12345 is sequential.
Of course whatever you select needs to work for both your PDM and MRP
systems, so you might want to consult the business types to see what
will work for them.
The reason I said with a PDM system sequential PNs are almost essential
is that the only way for PDM to identify a documet is by the file name.
If you have 2 docs with the same file name, PDMWorks sees the second one
as a revision of the first.
This is a frequent discussion on this ng and it is something that old-
timers in particular tend to get almost religious about. Just remember
that you need to have a rational reason for picking a system, and a
rational reason isn't "that's the way we've always done it", or "back in
the War, we did it this way", or "that's the only thing I know so it
must be right".
firstname.lastname@example.org (skrug) wrote in wrote in message
Hi Monkey -
Your problem is common for composite assemblies.
For a given component, I personally like the base number plus
For Example 12345_Rib.sldprt, 12345_Gusset.sldprt,
12345_Bearing.sldprt going into 12345.sldasm. This works great for a
composite assembly and does not needlessly "consume" numbers. My real
criteria for naming is this "will this model have a unique identity in
MRP or will it be 'masked' by the assembly or part it lives in?"
(generally vendor supplied or parts not visible to MRP like weldment
raw stock). If the part will not have an MRP record of its own, then
it serves the parent part (12345) and gets an appended name like
12345_Thing.sldprt. If the part (or sub part) gets an MRP record,
use that for the name.
Personally, I think it is self-defeating to "rename stuff later", it's
a pain in the keester and better to have a number scheme while
starting out. This is particularly true with PDM, especially when
your system requires unique names. Your company has a number system
which pretty much dictates what you need to use, so let that guide
Keep the number of BOM levels sensible if you can control it - Flat
line BOMs are great, 72 tiers in a BOM are not (subs in subs in subs
Dissolving makes no sense to me as the mates invariably do not migrate
upward with the dissolved components. Start where you want to end up.
Think about the assembly structure prior to your modeling and try to
get it structured right out of the gates.
Personally, I thing that one would like to build parity between your
MRP & PDM database wherever it naturally exists. The question you
pose is essentially that. MRP generally must drive CAD and one will
serve the other, usually MRP will dominated as this is what is
This is a long ramble, but generally since the two systems MRP & PDM
are not always synchronous, they can help and compliment each other
while one must be the "master" the other must conform. Personally I
try to make parity when possible, but if I can't I don't sweat it.
Treat your available part numbers like gold and use them for something
you will plan & fabricate (mrp-wise) but dont feel like you need to
hijack them to manage your cad data. That always makes one miserable
in the end. As you said "It may not be clear to future generations .
"Philosophy - The Science Of A Better Question"
You could make the frame as a weldment BUT make sure that the legs are a
pattern (i.e do one leg and pattern it - you could always use a sketch
driven pattern). Then you only have to mate one set of your assembly
components to one leg and use a 'FEATURE DRIVEN' PATTERN to populate the
other 7 sets of assembly parts.
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.