BOM Override

[reilly22]

Does anyone know of a way to override the quantity column in the excel based BOM? We are assembling our product with items that are "AR" (as required) and do not have a specific quantity. What we have done to assemble our product is create a blank part with the specified part number and inserting this blank part into the assembly. That way the P/N shows up on the BOM. The problem is, it shows up with a quantity of 1 which we want to change to AR. Thanks for the help.

 

[ctopher]

Dbl-click the Excel BOM to open, manually change from 1 to AR.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[reilly22]

We've tried the double clicking method and will work until the drawing is closed and re-opened. It then reverts back to 1.

 

[Scorch]

The problem with what ctopher has said to do the BOM will update to 1 again as soon as you rebuild the drawing. You will need to turn of Automatic update of BOM. You can do that by going to Tools-> Options-> Document Properties and toward the bottom is the check box for auto update. By unchecking this box the bom will not update if any other changes are made to the drawing.

Don't worry about people stealing your ideas. If your ideas are any good, you'll have to ram them down people's throats.
--Howard Aiken, IBM engineer

 

[ctopher]

Thanks Scorch, forgot about that.
Also, don't forget to save.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[reilly22]

Thanks ctopher and Scorch, it worked. I believe our CAD guy and I tried doing this but didn't save the option before exiting. Thanks again for the quick response.

 

[rgrayclamps]

Hi, reilly22:

Wait a minute! Turning off "Auto Update of BOM" will create more problems than it solved. As soon as you turn off "Auto Update of BOM", your BOM is no longer current. You do not want that, do you?

A better way is always to use true Bill of Material of an assembly in SW.

Alex

 

[reilly22]

Part of our BOM uses Solder and Flux. How do I have a quantity of 1 for these items?

 

[Scorch]

rgrayclamps,

The way we work around turning off auto update is to place a note next to the BOM letting the engineer know that it has been disabled. After updating the drawing, turning on auto updaate, update the drawing so the BOM updates and then turning of the auto update is a pain but in our case it is a necessay evil.

Don't worry about people stealing your ideas. If your ideas are any good, you'll have to ram them down people's throats.
--Howard Aiken, IBM engineer

 

[ctopher]

I don't use BOMS on dwgs in SW. They are separate docs. Adding BOMS on SW dwgs creates more trouble than it's worth, IMO.
Also, other depts can see BOMS without looking at dwgs.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[CorBlimeyLimey]

One simple workaround is to add a "Unit" column to the BOM. You can then add whatever units to the parts properties that you wish (eg. Each, Gallons, Lbs, A/R, BucketLoads, Feet, etc)

 

[felix7502]

This was taken from "SOLID Solutions Advanced" by Ron Yule

1.) Edit the BOM template in Excel. (We did a SaveAs first and created a BOM called bomtemp-string.xls)

2.) Add 2 columns immediately to the right of the QTY column.

3.) Add STRING and QTY as headings for the columns, assuming these will be columns C and D, respectively.

4.) In the (new) QTY column (column D), insert an Excel formula that points to the STRING column if there is any text there; i.e. =IF(ISBLANK(C2),B2,C2).

5.) Copy the formula down from D2 to D200 (or whatever is the biggest BOM you anticipate).

6.) Right-click on the column header of the original QTY column and select hide.

7.) Also hide the STRING columns (columns B and C).(I think that one of these columns was hidden in #6)

8.) In any part you want listed with a string quantity, create a custom property called STRING, and put the text string into that property (for example, "3 sets").

Note: If any changes to the assembly are made, you must edit the BOM template to update the added columns.

Our header order was different, so we just adjusted the column letters to suit. The BOM will come in with blank quantities, double-click and they will populate. Sometimes you need to delete the original BOM and enter a new one.
Sylvia

 

[rgrayclamps]

Hi, Reilly:

I do not know what is Solder and Flux. But if you do true solid modelling, you always get true BOM. Quantity of an item is only one thing. The other thing is Unit of Measure. Solidworks uses ea. as unit of measure. If you want something different, you can add additional custom properties as required.

Ctopher:

BOM on a SW drawing is a master source of component list for any assembly document, whether you use or do not use a PDM system. It is true that users view BOM information from PDM, but the data in PDM came from SW drawing documents (not from SW assembly models).

According to Solidworks and also consistent with ASME standard, assembly models do not have BOM. BOM only exists for view(s) on an assembly drawing. As matter of fact, BOM objects in SolidWorks are defined in views object.

In my oppinion, BOMs in SW document drawings should be updated because they drive PDM, not be driven by PDM.

Alex

 

[Standing]

reilly22,
Would you be willing to update to the SolidWorks BOM?

Bradley
SolidWorks 2007 SP2.0
NVIDIA Quadro FX 3400

 

[ctopher]

Alex,
If I understand you correctly ... you don't need a BOM on a SW dwg to run PDM.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[CorBlimeyLimey]

.. but the data in PDM came from SW drawing documents (not from SW assembly models).

Are you serious??? (I've never used a PDM system with SW.)
So if an assy drawing is not made, a PDM system cannot produce a BOM?

 

[rgrayclamps]

Yes, I am serious. In SW, BOM is defined by a view in drawing document. No view, no BOM.

You could retrive a part list from an assembly model file (*.sldasm) through API transverse, but that is not a BOM.

So, if an assy drawing is not made, then there is no BOM. A PDM system can still read part list from the assembly model per configurations. There is a reason for this (no BOM for an assembly model), but I do not understand why. Maybe someone can help explain.

Alex

 

[reilly22]

We would be ok with going to the Solidworks BOM rather than using the excel based BOM. We are just starting this SW system and this is one of the first bugs we need to work out.

 

[Standing]

When I create a sheet 2 with a SolidWorks BOM on it, I have found that I can delete the view that created the BOM.

Bradley
SolidWorks 2007 SP2.0
NVIDIA Quadro FX 3400

 

[ctopher]

Alex (rgrayclamps)
Two separate issues ... BOM's and PDM. They really have nothing to do with eacher other. A PDM just manages files, the BOM list's part file within an assy file.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)