linear feet in BOM 2

[solidmodeler]

Instead of just the quanity of parts in the BOM I would like take the quanity and multiply it by a length dimension of that part and have that "linear feet" displayed in the BOM. Then when the qty and length change this linear feet for the project will update. Can I do this?

 

[TateJ]

I suspect you'll have to use some VBAdoo for this - I'm ignorant.
There may be a clever way to get what you want, but without knowing the Big Picture, I can't offer any suggestions.
Are we talking about pipe, or bar stock, or garden hose?
Are you trying to perform a purchasing function?
We have a separate ERP program that adds-up all this for us.
So, this ain't a problem for me.
Please clarify a little...

Consume mass quantities...
tatej@usfilter.com​

 

[solidmodeler]

Actually, I am modeling a covered bridge (I know, unusual). Typically, in 2D, we call out linear feet qty's on certain items. my model represents some things, like floor planking, in one long length- and in reality it will be many short lengths- so I would like to just state the linear feet needed- which would be the length dim multiplied by the qty.

Thanks.

 

[TateJ]

OK - here we go... I haven't tried specifically this, but I'm 90% sure it will work. Let's say your're doing decking - you model the bridge with all these 4 x 6 planks patterned along the top. You can then insert an fake plate - define it in-context with the patterened decking so that it runs from one end of your bridge to the other. Then you can make some custom properties in this one - via a design table - that will calculate the linear feet and stick this in another custom property that you can put in you BOM. There are some minor caveats in this plan, but is this heading in the right direction for you?
Let me know...

Consume mass quantities...
tatej@usfilter.com​

 

[solidmodeler]

I will try this and let you know how it goes, Thanks.

 

[SnowCrash]

I have tried to include calculated part dimensions in a BOM without success. There may be a way to do this, but what I have done is to put the information you want in a custom property as text and include it in a custom BOM.

Crashj 'not very helpful this morning' Johnson

 

[dhinners]

There IS a way to accomplish what you want. Use the power of excel in your BOM.
Edit Your BOM template file.
Add a column for UOM (Unit of measure)
Add a column for QTY (Quantity entered)
Use 'Insert/Name/Define' in Excel to read custom props referencing UOM and QTY.
Naturally, your parts will need added custom properties for UOM and QTY for where you want to see a special value.
Add a column for QTY (Quantity calculated). Excel will fill this out, so you don't need to add a custom prop reference.

Assume your column 'B' is the standard SWX 'quantity' as measured by SolidWorks, column 'C' is for 'UOM', column 'D' is for quantity entered, and column 'E' is for quantity calculated. Use a formula in column 'E' such as:
=IF(ISTEXT(C4),(CONCATENATE((D4*B4)," ",C4)),B4)

This formula says:
If text is entered in UOM,
then fill in the 'Quantity Calculated' as
the SWX measured quantity multiplied by
the 'Quantity Entered' value
and add on the UOM as a suffix.
Otherwise, just use the SWX measured quantity value.

Copy the formula down for as many rows as your BOM might use. Then hide columns 'B', 'C', and 'D', leaving the 'quantity calculated' column showing.
To use it, you would need to populate the custom property in the part for UOM and QTY. For example, if your deck planks as modeled were 10 feet long, put FT in the UOM field, and 10 in the QTY field. Now if you use your new template for your BOM, it should fill in '10 FT' in the 'quantity calculated' column. By the way, the header can still just be 'QTY' - SolidWorks doesn't care about the header, only the name used in the 'Insert/Name/Define' box.

I hope that all makes some sense!

D Hinners

 

[solidmodeler]

D Hinners,

Great response, thank you.
This is the type of solution I was working on- using excel- the only thing I wish could be accomplished is to bring a dimension value right into the excel bom. It seems like that if every dim is a parameter this value should be (somehow?) available to be read in excel?

This would automatically input the lenght for your QTY field... can this be done?

 

[dhinners]

You can easily capture parametric dimensions in your BOM. When entering your custom properties, just double click the part. All the feature dimensions will display (so its best to view it in ISO). Then while your cursor is in the text area for your custom property value, you can click on a part dimension & SolidWorks will add a parameter such as:
"D1@Extrude1@Example1.SLDPRT"
The value will display in the BOM the same as in the dimension, so if you want feet make sure your units are feet. If you add a property that only contains this value, I think Excel could use in a formula such as discussed above.

 

[solidmodeler]

That was what I was asking- how to include the dim value as a custom property. And it is very easy! Thanks.

But now I am having another problem. I have saved the bom (that has the excel formula in one column) as a template. Now when I insert this template in another drawing at the creation of a new bom, the formulas are erased... am I doing something wrong? The heading of the column in the bom with the formula is a custom property that has a blank value in every part/assembly file, I think I have to have this custom prop value b/c if I just have a blank heading the bom ends at that cell, or do I need to have that formula as the value of that custom prop in each of the files? (I guess I could just change my part/assembly start template to have that formula saved as the custom prop value)

Thanks.

 

[alecu]

I have problems with printing BOM that has formulas inside... My BOM looks similar with dhinners proposal,(jan 15), everithing is fine but if I want to update drawing or if I try to print out document, that column in BOM that contain formula become empty. I'am sure that is a simple way to solve this. Thank you.

 

[dhinners]

solidmodeler & alecu:

It looks like you are both having a similar difficulty. My guess is that it has to do with how you modify your BOM template.

First, it is important that you actually modify the BOM template. If you insert a BOM, then modify that BOM in the drawing, those changes will be lost when the BOM updates.

Also, do not apply a custom property to the column that contains the formula. If you do, SolidWorks will insert the value of the custom property into that column for every part, wiping out your formula. You DO need a column header, but it should be just plain text with no custom property tied to it.

Hope that helps!

 

[alecu]

I found what was wrong with my BOM!! The column's title!!!
This was a real surprise for me. It supposes to use any name, right?! It's not so easy... More than that, that column was not associated with SWX custom properties; it contains formulas that managed other stock list data from my excel file. So, I called this column "MATERIAL". Again, BOM was regenerate fine with double click, but when I pressed rebuild, or saved the drawing, or try to print out, this column cells become empty. Solution! I change the column's name from "MATERIAL" to "STOCK" and everything was fine!!?