Hello, all ,new fellow here.
I've been working with Solidworks for about half a year now, off and
on. Two things that have been bugging me is (1) that old nemesis,
revision control and (2) flowing info from the model into the bill of
Disclaimer: I'm new to newsgroups as well, so if there are other
threads on the subjects, could someone tell me how to find them, so as
to not waste anyone else's time? Now on to the "meat":
The way we've always done our drawings, whether of weldments or
assemblies or single parts, etc, ahs always been drawing number-based.
We've always used that "group" system, and often would lay out multiple
pieces of a fabrication on one drawing, then show it welded up, etc. on
the same sheet. Perhaps bad practice, but it's always worked for us.
Let's continue with a weldment as the example. On that drawing, the
assembled weldment would be designated as a "group". A drawing that
required that part would order it in the bill of materials as "Dwg.
XYZN01, Group X." Thus our Solidworks drawing file would be
We've figured on dumping the "group" system and concentrating more on
single-item drawings at the base level. A "group" is basically a
subassembly, anyway. The real bill of materials problem comes in at
the assembly level.
Now in that same column in the bill might be other such sub-assemblies
or weldments, as well as, say, fasterners, maybe an additional plate
(designated by it's dimensions) and so on- which are, of course,
different data types, and bam!- I'm buggered.
I've figured out a way to pass dimensional info into the bill. (Ex: a
plate, you sketch width and length, make a custom property, and
designate them for it. Then you extrude the thickness, hang a
reference dim. off of that and designate it for the same field.) But I
cannot seem to come up with unified scheme for generating a bill of
materials without several columns that used to be just one column on
The next issue then comes with revising the drawings if needed. Any
opinions as to whether it's better to do this at the model level (with
the custom property) or the drawing level? It seems like, in a
complicated assembly, that if you do it at the drawing level it's be
awfully easy to lose track of what drawings need changed when a change
is made somewhere.
I have other issues, too, with materials, but this is long enough for a
1st post. Thanks all for your reading patience and any
help/re-direction you can provide).
BTW, we are a small office that shares a single licence on an as-needed
What we've done, the two of us in this office, one of which is often 800
miles away, is create a BOM template with an extra columns, then in the
part and assy templates we have custom props that need to be filled in.
This way there is a 'standard' column in the BOM that gets populated with
the info entered into the custom props in the part and assy files.
Your way of weldment drawings sounds like ours, all the bits and pieces are
detailed in the same drawing set as the welded-up assembly.
Rev control is another matter, being small and under-funded we use pdf
files as the 'official' released drawing, changes become REV-A or whatever,
while the CAD parts and models merely change as needed. We have the pdf
"drawing" to look at the history if necessary.
Really, that PDF idea is sparkling. We often send drawings out that
way, but using it as REV control could save the day, with a little
self-discipline. I'm still exploring how the revison custom property
in the model (be it assembly or part) would flow to the child drawings,
that may also help.
But do you have a BOM that has a bunch of columns? They've got too
much white space in these already, that's all I need is extraneous
columns. I am exploring using, say part no., or any custom property,
in a differnt way depending on the file type. In other words, if I had
a plate, it's part no would be it's dimensions; if I had a subassembly,
it's part no. would be it's file name...
At the end if the day, you order off of the BOM. I'd sure like to know
what they were thinking on this one.
Yeah, it works OK with the two of us, and theoretically the guys in the
shop or on the floor can access the files easily too. If there were more
than 2 or 3 in the office it could easily become a headache.
I haven't delved too deep into the "new" BOM but I should be able to set it
up much the same as the old Excel based BOM, mine has columns for ITEM NO.,
QTY, DESCRIPTION, SIZE, MATERIAL, PART NAME ,etc
With the BOM I simply hide the unnecessary columns in the filetypes that
don't need the extra columns. For the weldment files I have a column named
'SIZE' where I entered the size of the plate or the length of the pipe, the
'MATERIAL' column would state 3/8" COLD ROLLED or 2" SQ. STEEL TUBE or
whatever. Though the 'new' BOM covers that in the DESCRIPTION.
In the upper lever Assembly files I use the PART NAME coulmn and hide SIZE
and the others. PART NAME is really just a general description to go with
the Item No., Qty., and Part No.
Also jsut today I discovered a way to cut down on the white-space used by
SWX in the 'new' BOM, when dragging a column skinnier it stops way short of
where I want it, select the column from the top of the BOM, rightclick,
select Formatting..., Column Width!!! You can force columns to a specific
I hope that made some sense and was of some help. Being essentially a
one-man operation my grasp of how best to deal with BOM's etc is always
evolving, what I did last year isn't necessarily how I'll do it this year.
I'll try to send you a couple pdf's so you can see what I'm talking about.
Thanks again, Whit - got your samples this morning.
I'm working with the non-excel BOM (I suppose that's the "new" one).
I've been fiddling around with the custom properties, and like I said,
I can get dimensional info to transfer - it's the mixed data types that
mess me up, particularly at the assembly level. Then, too, if I just
want to call out an A36 Steel in materials, there is no such bird in
the supplied library - for a reason, I know, but still...
I could probably split this off into a coupe of threads, and maybe some
of this is simply my ignorance of how the program is supposed to work.
But another BOM-related problem comes in from a different angle. Say
you wanna make a very simple "U" shape out of a piece of material , say
30" long, 2" wide, 1/4 thick. Okay, I could just order it on the Bill
that way. But in reality, I want my piece to have 10" legs with a 5"
overall width and a 4.5" inside radius bend at the top. The developed
length of the piece is somewhat less than 30" -and this is what my guy
would have drawn in the first place. Now there is no way to get that
info into the BOM. BUT THE INFO IS THERE! Solidworks can tell you
everything about that piece - you just can't link it into your bill.
I quote now (at the risk of drawing in that guy that keeps gong on
about VX...) from my reply to a vendor who offered a $1000
solution to my problem:
"it makes me madder than two wildcats in a burlap sack that a
multithousand dollar program with all this functionality (some VERY
good, by the way) clogs up when it gets to the most important part -
ordering and cutting metal. I generally do analysis here, and the FEA
aspect of this thing isn't half bad. But if I'm off a couple of
thousand psi, it generally doesn't matter. On the other hand, that
drawing and that BOM had better be lock-on correct. I have a draftsman
entering size data and material info into a Solidworks BOM by hand
(material library comes up short as well) - same as in AutoCAD - and
prone to the same mistakes, not to mention the loss of productivity and
the parametric link. What's worse, THE INFO IS IN THE PROGRAM. It's
all there! Why should I have to be an API writer to get at it for this
most basic - and yet most important - of tasks? Dumb, dumb, dumb."
There. My rant for the day!
Thanks again, Whit!
Glad the email made it thru, my method just specific enough for our needs,
it sounds like you're deeper into it than we are.
I agree with the rant, but I think maybe this illustrates part of the
problem , everybody wants/needs to use the BOM differently. Unfortunately,
either SWX decided not to develop it fully or they haven't done a very good
job of explaining how best to utilize it.
I don't know if we are into it deeper or not. You know, with regards
to my "U" shaped piece, I did discover a way to do it: You model it as
a sheet metal part, flat, and then use the sheet metal tools to put the
bends in. Supposedly (with the use of the proper bend table...?),
Solidworks calculates the proper developed length. I don't know how to
access this length for BOM purposes, though. However, if I dimension
my unbent piece, I can get that info into the bill.
Trouble is, we don't usually model our stuff that way. Maybe we
should. But if I have finished dimensios to meet, why start from a
flat piece? I'm going to draw (model) to my finshed dimensions.
We were sold this program on it's flexibility - i.e. it molds to your
ways instead of vice versa. I've been involved with computers & CAE
since punch card days and so had a well-hardened cynicism of said
claim. I hate being right...
Gee, Whit, this thread isn't attracting much attention... just you and
me... You think the others know something we don't, or are they jsut
as perplexedas we are? I'm starting to feel dumb! ;)
Take a look at the sheet metal section in Help. You have a variety of
methods available to produce accurate sheet metal parts, and lots of people
are doing it. It sounds like the method you "discovered" is sketched bend,
which is a valuable tool. However, as you point out, the primary thought is
usually what it will look like in the formed state. So, build it that way
by either starting with a base flange, or by modeling the solid and
We also put multiple views of multiple parts & assy's on our drawings, and
each assy has its own BOM. We use a system called "mark numbers" which I am
told long ago came from the statement to "mark that number on the part."
So, a top level assy would have a mark number of say 100A, and its BOM would
call out piece parts detailed on that drawing (in which case the BOM would
list the material), or purchased parts, hardware, etc, or other subassy's or
parts made on other sheets (101A, 101B, 103C, etc.) I think this is
probably what you are discussing here??? Any help?
As to your first post, yeah, I think I have some exploring to do in tha
area. What I'm taking about, though, isn't sheet metal in the sense
that I generally think of it, like, say, stamping out framing (nailing)
brackes for home construction. Mostly it is, say 1/4 in. stuff as
housings for motors & generators, often with big radii, etc. I'm
trying to remember, I think I did one as you suggested, unfolded it,
dimesioned the developed length, put the dimesion into the custom
property field, and VIOLA! Except that, to rebuild everything
properly, the model had to be refolded, at which point the dimesion in
the bill changed to reflect the distance between the two points when
folded. I had to use the method posted to get an unchanging linked
dimesion for my bill.
As to your second post, yup, it sounds like what we do. Are you saying
you have mulitple BOM's on one drawing? If so, have you eliminated the
titles across the top so you can stack'em and make them look like a
single bill? You know, the durn things take up to much space already!
At any rate, that's what is buggering me right now - essentially mixed
data types. I'm thinking I might have a way around it, and it sounds
like you do, but I'm carrying this thread on whilst being pulled away
by anoher job and cannot check it out right now.
Sheet metal can be 2" thick for some people! The point was that the sheet
metal features in SW are pretty good with brake formed bends and if you plan
on forming it like that, SW will probably handle it.
The only way I have found to tie a property to the flat pattern length is to
insert a sketch line that has the length controlled by an equation. This
equation is the sum of all the legs & and neutral axis lines through all the
The problem with just using an overall dimension in the flat is that the
dimension is a 3D dimension between two points in space, and in the folded
state, those two points get closer than they are in the flat pattern. The
dimension is still a correct dimension - your points just moved! So, we
usually just key in the flat dimension - not as nice as would be desired,
but it works.
We do put multiple BOM's on a drawing. We keep the titles and have each one
start with a new number series, like the first one is 1-14 and the next one
starts with 20. That way each "mark" number has its own BOM.
Well, as to general BOM info, the only "multi-use" field is the Part
No. By checking the "Use Title Summary" box, you can put whatever you
want into the title field on the Summary page of "File - Properties"
and it will come up in the BOM. However, some limitations exist. In
order to get the dimensional info into the title field, you have to
create a dummy custom property (as outlined in the help file, "how to
insert dimesions into custom properties"), and then cut'n'paste into
the title field. Also, as with custom properties, if you refer to a
global variable, that's ALL that can go in that field. And I don't
think that I can use the file name in that field (I'll put up with the
redundacy at this point).
Like I said, maybe I just don't know how these features "should" be
used. But I'm amazed at the lack of flexibilty I find here.
Solidworks "knows" everthing I want to put in the bill. You just can't
get it there...Unless you're an API programmer. One salesman has
contacted me already, and nothing against him, but why should I have to
shell out another grand for something that ought to be the prime
functionality of SW in the first place? Criiminee, there's a dozen
programs out there that can easily create 3d geom and let you spin it
around on your monitor endlessly. The drawing and the BOM are where
the rubber meets the road.