BOM questions

I am currently evaluating SW2006. Last year I purchased Alibre Pro and
have enjoyed a lot of benefits switching to 3d-based parametric CAD.
Perhaps I'm guilty of a "grass always greener" syndrome, but I've been
tempted to look at SW mainly because Alibre is fairly weak in it's
production of 2d design drawings with regards to speed (20-30 minutes
for view creation on mildly complex assemblies) & aesthetic control
(annotations and such are limited). At the end of the day, it's the
drawing that still allows my shop to build machinery so the 2d
production drawings are critical.

With my 30-day money-back guarantee slipping away rapidly, I'm trying
to build some test assemblies in SW2006 to make sure the seven-fold
increase in price is worthwhile. I've run into some sticky spots, some
of which are surely my ignorance (though the lack of a proper manual is
a tad frustrating at this price point!). In particular, I'm not sure I
grasp the SW methodology behind the BOM.

In Alibre (pardon the comparison), a BOM is a separate file just like a
part or assembly. The BOM is linked to an assembly and is
automatically populated with the assemblies parts. In SW terminology,
this is a "Parts Only" BOM there is no option for indented sub-assembly
(though you can optionally specify a subassembly to be treated as a
part). When working within a drawing, you can link the drawing file to
a BOM. Then, any view, on any sheet will reference the same BOM file.
In fact, you can have many drawing files (each with multiple sheets)
all referencing the same BOM file. This can be convenient if a drawing
file becomes unwieldy (which often happens around sheet 5), just start
a new drawing file, link to the original BOM file and all item numbers
are kept constant.

Using this approach, you can create views of parts or subassemblies and
the item numbers ALWAYS match the BOM file. In SW2006, it appears that
the BOM is attached to a specific view of an assembly. If I create a
view of an assembly on sheet 1 and insert a BOM I can balloon the parts
in the assembly to my heart's content. On sheet 2, I may want to
create detail views of the individual parts of the assembly. If I then
try to balloon those parts, the item numbers do not match the assembly
(in fact they are all listed as "1").

I've done some googling, and searching on the SW forum, and it appears
that many people find this behaviour to be problematic. Answers seem
to range from:

1. Manually override the balloons on the part views. Not an
acceptable substitute as it leaves the drawings open for too many
errors.

2. Instead of creating views of parts, create views of the main
assembly and hide the unwanted parts. Not acceptable substitute
because this quickly brings the system performance down and seems to
defeat the purpose of part, subassembly, assembly modeling.

3. Use a custom property in each part file that is unique, and use
notes that reference this property rather than the item number in the
BOM. This seems the most likely candidate for success, and perhaps
better than the Alibre method since accross the product line a part
will have a consistent designator regardless of the assembly. The only
downside is that using part designators is harder to look-up in the
BOM. When a fabricator references the BOM to find the quantity of a
particular part, searching the BOM for "DEB-1.5-6-STL" is harder to
locate than "#6", which of course comes after "#5" and is thus easy to
locat in a long list.

Whew! That was a bit long, my apologies. Please let me know if I'm
missing the underlying philosophy of the BOM in SW, I really want to
give Solidworks a fair shake and determine its cost/reward ratio when
compared to my current software. My preliminary observation is that
while I haven't been "blown away" by the capabilities, the 2d drawing
package does show more polish than AD, which is what I had hoped.

Best regards,
Gareth Conner

 

Ok, I'm a bit confused as I just tried a few things and it all worked
properly.

I have not tested SW2006 much because of lack of time, but I just did a
test. I dropped an assy into a drawing, inserted a SW BOM (not the Excel
version,) ballooned it, added another view ballooned it, added another
sheet, added a view, ballooned it, put a section view on the first sheet,
ballooned it, cut that section view from that sheet and pasted it onto the
second sheet, ballooned it, ......... and all the balloons matched. Whew!

So,,,, a bit of explanation here for you. The SW BOM is not tied to a view,
as was the old Excel BOM - rather it's tied to a configuration. The BOM can
be top level only, all parts, or an indented BOM, and with the indented, it
can number the subparts like 6.1, 6.2, etc. If you have different configs
in your drawing views, then sometimes you have to tell the drawing view to
"Keep linked to BOM" and specify which one.

Your comment on the lack of a "proper" book is noted, however, the online
help is really quite good, and I have found that I like it better than a
paper book because of all the examples, video clips, and hyperlinks. Go to
the help and look up Bill of Materials - I think you might find most of what
you have missed. Then if you still have questions, come back here - we aim
to please.

WT

 

Hi Wayne,

Thanks for the response!

Everything seems to work fine as long as you are ballooning an assy.
However, if I detail a part by creating a model view of a part (not the
entire assy) the balloon item number does not match.

I often have a couple of sheets of a drawing that show the entire
assembly (orthos, isos, exploded isos). Then typically I'll have
several sheets that are just details of the individual parts, mostly
for the machined parts or laser profiles. For the views of individual
parts generated from Part files, not Assembly files, the BOM numbering
doesn't remain consistent.

I think the basic problem is that there is not way to associate a
single part view with the certain BOM associated with the assembly. In
single part views I've started placing a balloon on the elevation to
help the fabricator (or even myself) identify the part as it relates to
the BOM. This doesn't seem possible in SW, but you can instead stick a
note on the part that automatically displays the part name (or custom
property) which may be fine for my needs.

I have seen the indented BOM, which is a great feature. The only
drawback I see is that the part quantities are listed per subassembly.
Therefore, if I have multiple subassemblies, the part count needs to be
multiplied by the subassembly count in order to generate a PO. This is
OK, but I'll need to exercise some caution so that I don't end up short
parts!

The online help is adequate, but I'm just stubborn when it comes to
books Ideally, I'd like to have both the online help and a
reference book on my desk. I've purchased the Dave Murray "Inside
Solidworks 2003" book which seems like a handy reference (though a
couple of releases old, and thus it seems like it pre-dates the 'new'
BOM?).

Thanks again, I think I'm slowly getting up to speed!

 

Thanks Dale,

Sounds like I need to adjust my drawing practices a bit, glad to know
that option #3 still sounds like the most prudent.

Thanks for the SWit link, I'll have to invetigate that.

I appreciate your help!

-Gareth Conner

 

If the detail is taken from the assembly:
RMB on the model view - Select Properties - Select "Keep linked to BOM"

If you insert a view of a part by loading the part separately:
Connect the balloon to the part in the assembly and place the balloon next
to the part. Remove the leader with the "no leader" option

and the balloons have to match now.

\/\/im

 

Thanks, I'll try out your second option that may be a fine workaround.

I appreciate your help.

Best regards,
Gareth Conner