2004 BOM Qty

I have a problem that I hope someone out there may have solved and
would be willing to help me out with.
Example:
A three sheet drawing where the first sheet has assembled views of a
weldment. The weldment has two side plates and three center gussets.
When the BOM is placed on this sheet the quantities shown match the
actual quantities. The second and third sheets are detailed views of
the machined parts used in the weldment. When a BOM is placed on the
detail sheet, it lists the quantity as one since there is only one
part on that sheet. I want it to list the quantity of parts needed for
the weldment.
This is an over simplified example of our real world problem. We may
actually have a sixteen sheet drawing to detail out a fifteen part
weldment. The work around of having the entire weldment on the detail
sheets and hiding all but one part will not work for overhead reasons.
Does anyone have a tool that takes the part quantites from the first
sheet's BOM and will work with 2004?

Thanks in advance

Brad

 

I may have a workaround for you -- depending on whether I understand
your correctly. It sounds like what you need on the 2nd and subsequent
sheet is a HIDDEN view of the main weldment, to be used as the source
for the BOM on each sheet. Insert your BOM from the hidden view. If
you need to only show one line in the BOM (for the part represented on
the sheet), then right-click on the BOM and choose Properties. Go to
the Contents tab at the top of the resulting dialog box and UNcheck all
the parts except the one you have detailed on the sheet.

You can also put a note on the sheet indicating Quantity for the part
detailed there, and you can drive the value in the note with a Custom
Property -- but only if you use the Custom Properties of the part on the
sheet to drive the rest of the info in the title block (right-click on
the Sheet tab at bottom, choose Properties, and at the bottom of the
dialog box select the view from which you want to pull the Custom
Properties for the sheet).

Mark 'Sporky' Stapleton
Charlotte, NC

 

Sorry about the poor description, I posted this same question about a
year ago and was no better at explaining what I want.

The idea here is to have the weldment drawing (sheet 1) for the person
doing the assembly and welding. The detail sheets are for machinists
who do not always get the main assembly drawing.

Based on my example, the only part I want on sheet 2 would be the side
plate. If I insert the standard BOM on sheet 2, the quantity will read
one when two side plates are required. A model view of the entire
weldment could be inserted in sheet two. This would require that all
parts and BOM items except for one side plate be hidden. Doing this
does display the correct quantity; however, this becomes a problem
when the weldments have a large number of parts (things bog down,
files get big).

I want sheet two to look at the BOM in sheet 1 for the quantity of
parts needed. The name, stock size, etc could still come from the
part. Putting notes and custom part properties would work; however,
these values would not be dynamic. If I add or remove side plates from
the weldment, I want the changes to be reflected automatically in
sheet 2's BOM.

Hopefully this helps explain what I want.

Brad

 

Perhaps I was the one who didn't explain well enough. My workaround
would do exactly as you wish to do. What I think you're missing is that
you would insert views from the Part file(s) on sheets 2 and subsequent
-- ALONG WITH a view of the entire weldment (Assembly file), which you
would hide (in its entirety) BUT which you would use as the basis for
the BOM. Please go back and read my original post with that in mind.

Now, you're quite correct that the Drawing file WOULD bog down when you
have large weldments because there would be a view of the entire
weldment on each sheet (although entirely hidden), but I don't believe
there is any other way (outside of VB) in SolidWorks to accomplish
AUTOMATEDLY (from part quantity changes in the assembly file) what you
want to do.

'Spork'

 

OK, I got a chance to try and verify a method that may work for you:.
This method only works for the new SWX 2004 BOM. I could not get it to
work with the Excel based BOM.

1. Place your assembly view on sheet 1
2. Place your part view on sheet 2
3. Place a SWX BOM on sheet 1 that references your assembly view
4. Cut and paste the BOM to sheet 2 (Note: you need to click on the BOM
and then click on the little title bar that pops up to be able to cut
and paste).
5. Choose to hide all rows except the row for your item on the part
detail sheet
6. Repeat for all part sheets

Thus, you should end up with a 1 line BOM on each of your detail sheets
to call out the qty for that part. Is this what you wanted?

 

Isn't there a way to insert a BOM on sheet 2 that references a view on
sheet 1? I think if you highlight the view on sheet 1, switch to sheet
2 and then insert the BOM, this will work. (I can't verify at the
moment...)

Then you can go in and hide the rows you don't need.

If there is not a way to do the above, Spork is right, you either need a
hidden assy view or use API.

 

If the weldment is done as a 'new' 2004 weldment (actually a part) and the
bits are detailed on seperate sheets you can attach a split item balloon
(top shows item number and bottom shows number required) and this works
correctly across the different sheets (it refers back to the main weldment
cut list). However, I have not found a way to extract this info and put it
into a parametric note.

I am using this method a lot at the moment and it is working OK - generally
quicker than creating the weldment as an assembly. I have pre-defined custom
properties in the weldment library features and this auto completes the cut
list. Major drawback is that items being detailed seperately do not contain
any of the original dimensions used to create them; therefore, you have to
populate the view with reference dimensions.

Merry

 

Arlin,

Based on your description, this is what I want. The problem is that no
matter how I select the BOM, I get a Solidworks warning message that
says "This item cannot be copied to the clipboard". Any suggestions?

 

I got this message as well at first...
The solution is to first click on the BOM. A solid bar will appear at
the top of the BOM, CLICK ON THAT BAR. You should now be able to cut
and past the BOM.

 

Brad,

As you have discovered, SW is not geared to manufacturing drawings with
correct BOM's!

Several of the recommendations which you have received will work, but it
really depends on the master assembly size and if you can afford to have it
hidden in each drawing set. My last assembly was 15,000 + components.

Instead of including it in all of my drawings, or even in the first drawing
of a set, I gave each part a property "MQty" manual quantity. I the printed
one major assembly BOM (parts only) and using PDMWorks entered the correct
qty into each part.

I also Placed a property "qtyUpdate" Yes or No and set it to yes if a new
assembly could change the qty.

This allowed my to develop a BOM template with the BOM QTY column set to a
font size of 1 and qty deleted, and a manual qty column using MQty which was
titled QTY.

If some would develop an API that could look at an assembly and count the
parts so that drawings always reflect build quantities correctly that would
be great.

Tom

 

After carefully reading your posts I found the word cut. I was trying
to copy which will not work no matter what I try. I did get it to work
and it does do what I want. Thanks for your help.

 

Tom,

Leonard Kikstra has developed this AssemblyBOM
(http://webpages.charter.net/mkikstra/swx_macros.html)
which would require very little modification to do exactly that.If we all
together ask him to help maybe he'll do it.
Then we can put it in an assembly as Macro Feature and forget entering
quantities manually

Regs,
Henry

 

Henry,

I don't know Leonard, but that's a great idea. Anyone working in large
assemblies is basically left out in the cold when it comes to reasonable
solutions to get total quantities or consistent item numbers into their
drawings.

Tom