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BOM Length as QTY...???

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dutch7777

Mechanical
Nov 8, 2001
175
Is there a way to tie the length of a part to the QTY.
in a BOM...Say 5 inches of wire as opposed to 1 wire...???
I'm trying to avoid creating another column for length...

TIA
 
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TIA, We came up with a very complicated way of doing this. I copied my manual with how too. The pictures do not show up here, nor does the SolidWorks excel BOM come in. If you post your e-mail I could send you the MS Word doc, with the Excel BOM.

BOM - Linear feet in BOM
In preparation for building all Bills of Materials automatically, you will find a new text box field (UoM) on the Alt R Revision control dialog box. Shown in the lower right hand corner of the figure below. You will no longer have to delete a Bill of Material and re-enter edited text for length. This also includes any referenced text. This does not have to be run on all parts and subassemblies in a BOM. The inserted BOM will assume a UoM to be EA when the property within a model has no UoM set in the model. Warning: If you delete the BOM you will have to re-enter any text in the reference column. See heading below “Corrupt BOM’s”.



For a part that has a unit of measure of “Each”, EA will be in the text box under UoM (Unit of Measure). When the part has a unit of measure of “Feet”, FT will be placed in the text box. To access the list of alternate (UoM) units of measure, click in the text box shown in the above figure where EA is.



Now click on FT, EA, 0, QTY, or 2PL. Change your revision and click Save Changes.
As a side note: The 0 (zero) you see under UoM is the number zero. The property that is entered in the model is NA. The zero you see is just a visual, meaning no quantity.
Upon completion of updating the drawing and models, every model that gets a UoM added to the properties must be checked back into the PDM.
For those of you that use “Duct, Wire Routing PVC” and similar items in your assemblies, we have a new Unit of Measure “ 2PL ”. “Duct, Wire Routing PVC” comes in 6-foot lengths. The quantity that is required in your Bill of Materials is a percentage of 6-foot lengths. For example 620780 Assy, Support Tray, Cable, Upper Inserter requires 4.5 feet. Item 4 of the drawing that is in the PDM is .75 only. No EA or FT required.
A synopsis of what we have now.
FT Feet - Wire, tubing, hose, tape and etc.
EA Each - Purchased as “each” e.g. nuts, fuses, computers and etc.
0 Zero - The number zero for referenced items e.g. Do Not Use.
QTY Quantity - Put 1 part in Assembly, QTY can be 437 parts.
2PL % - Percentage of Each e.g. Ducting.

Warning:
Those of you who refuse to run the Alt R button must add or change this property manually. The UoM does not have to be added to all parts and subassemblies in a BOM. The inserted BOM will assume a UoM to be EA when the property within a model has no UoM set in the model. There is no rule that says you must run the Alt R button, but the SolidWorks property “UoM” must be added and the Unit of Measure must be set.

Just the steps for you “know it all’s”.
1. Turn on “Automatic update BOM”. If you delete the BOM you will have to retype in any reference data.
2. Create a configuration in part model named the length of the item e.g. 2.0 FT
3. Create a sketch on the “Top” plane and rename the sketch to “Length”.
4. Draw & dimension a line from zero. Hide, and drag to under origin.
5. Double click on Length in the feature manager tree, the dimension will show up in the model. Double click on that dimension, you will see the following Modify dialog box. At this point set to “This Configuration” as shown in following figure.

6. To Link Configuration Specific to Total_Length see following figure. Click “Total_Length” in the “Name” field. Now click in the “Value” text box, which is blank at this time. Now click on the dimension shown when you double clicked on Length in the feature manager tree. If no dimension is shown then double clicked on Length again in the feature manager tree. SolidWorks will fill in the “Value” text field.

7. Open your assembly model. Right mouse click on the model number in the feature manager tree you want to set the configuration for. Chose “Component Properties…” click name of wanted Configuration. Save your assembly.
8. Open your drawing. Insert BOM. When you rebuild drawing your quantity will disappear if you have done everything right so far. Edit BOM in drawing and click outside of BOM. You do not need to do anything at the point. The reference column will be manually entered. If you need a carriage return in the reference column then put in the “||” found in the finish properties. Word wrap does not work well within SolidWorks Excel BOM’s.
9. The Excel version of the BOM is built using bomtemp.xls.


Bradley
 
Bradley Thanks

TIA=Thanks in advance...oops...;o)

Send away to:

drdXXX@microcomcorp.com <-remove the XXX's

TIA again

Dave
 
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