Ballooning with part numbers

For starters, I'm running SWX 2003 SP 4.0. It does everything I need and
rarely crashes, so I discontinued my subscription and have been saving
thousands annually ever since. The following is the first situation that I
can't find what I need in 2003:

How can I click on a part (or sub-assy) in an assembly and have a part
number tag get placed. Specifically, I'm looking for something as easy as
the balloon button where I click the part and the balloon is placed.
Instead of a balloon, I'd like the part number to get placed (the same part
number that would show up in the BOM). I can do this with a linked note,
but it takes too many steps. Maybe a macro?

 

How can I click on a part (or sub-assy) in an assembly and have a part

Gotta love answering your own questions. Here's the solution:

1. Create a new BOM template.
2. Set each cell in the ITEM column equal to the PARTNO column. I did this
for 150 rows since I don't think I'll ever have a BOM with more than 150
items.
3. Hide the ITEM column.
4. Set your drawing template balloon settings to use "none" instead of
"circle".
5. Place your BOM as usual by selecting a view.
6. Use the balloon command to pick parts and the part number will show up
instead of the item number.
7. Celebrate as you shave hours off of complicated assembly drawings that
span multiple configurations, have hidden and suppressed parts, and
generally suck.

 

I tried this with SW2005 and an Excel based, when I place the balloons they
still come in with the old ITEM number and CTRL+Q changes the formatting in the
spreadsheet so that the ITEM numbers return to 1, 2, 3, 4 .... bummer.

I do have a Link Notes Macro that I found thru this NG, work with the excel
based BOM, pretty slick. I'll decipher your email and send it after while.

Whit

 

I found one caveat to my balloon-with-part-numbers scheme: if you create a
ballooned drawing with a BOM and then add a new part to the assembly, the
new balloon will not be correct unless you double-click the BOM as if to
edit it. You don't have to change anything, but opening it causes Excel to
recalculate all the formulas. Until you do this, your "balloon" numbers
will be incorrect.

Whit: I got your macro and I'll take a look at it. I'm running SWX 2003sp4
so I'm not sure it will work considering you're on 2005. Also, to your note
about CTRL-Q causing the ITEM column to revert to 1, 2, 3, etc.: I don't
have that problem with 2003. Maybe try relocating your ITEM column to the
right of the $$END column in your template??

 

---<Big Clip>---
All,
The following works in SW04 & SW05 (not sure about 03)
First of all, this works in any assembly drawing and for any assembly
components including configurations. It utilizes exiting SW properties
or
any custom and/or configuration specific properties that have been
set-up in
your parts & assemblies. The best thing is that no BOMs or Macros are
required. Simple or Poor Man's Method:
Create a note (annotation), select a component in your assembly,
place the note, then select the "Link to Property" icon, next and most
importantly, select; "Component to which the annotation is attached".
Now select the drop
down arrow and select "SW- File Name" or "SW-Configuration Name" or any
of
your companies custom file properties. Add any other annotations and
then
place on drawing. To reproduce, select first note, copy & paste, then
reattach arrow to the next component. The note will update
automatically.
NOTE: I'll be posting this in the SolidWorks Discussion Forum with a
JPEG
attachment if you need more info.
Eddie

 

---<Big Clip>---
All,
The following works in SW04 & SW05 (not sure about 03)
First of all, this works in any assembly drawing and for any assembly
components including configurations. It utilizes exiting SW properties
or
any custom and/or configuration specific properties that have been
set-up in
your parts & assemblies. The best thing is that no BOMs or Macros are
required. Simple or Poor Man's Method:
Create a note (annotation), select a component in your assembly,
place the note, then select the "Link to Property" icon, next and most
importantly, select; "Component to which the annotation is attached".
Now select the drop
down arrow and select "SW- File Name" or "SW-Configuration Name" or any
of
your companies custom file properties. Add any other annotations and
then
place on drawing. To reproduce, select first note, copy & paste, then
reattach arrow to the next component. The note will update
automatically.
NOTE: See posting on SW Discussion Forum for image.

 

There is a major shortcoming with this approach: you can't select sub-assys.
Unless you have some sort of magic trick up your sleeve.

 

Mickey Reilley wrote:
---<Clip

---<EndClip
Agreed. This will only work with components. So, for sub-assemblies I
would simply create a manual note.
Sub-assembly part number could still be referenced or identified as
coming from a sub.
Enhancement Request Time!

 

Actually you can. If you grab (attach the note to) the coordinate
system in the sub-assy or any sketch element that is at the sub-assy
level it will show the information for that sub-assy. Now the trouble
is getting an element in the right location to pick.

Sometimes it is difficult to pick graphically and has to be picked via
the tree.

--Matt Feider

 

I just did some more testing and the addition of a point in a sub
assembly works great. Of course there would need to be an agreed upon
location if "Part Number/Ballooning" were to be used often.