Another question... on bill of materials 1

[Morglisn]

Hello, again!

I'm trying to include the square footage of my pieces on my BOM. Unfortunately, almost ALL of our pieces are cut as flat patterns, then folded, so.. I've been drawing them in the finished product, then unfolding. Unfortunately, the flattened dimensions always show up as referenced dimensions, and can't be used in my BOM. Am I perhaps doing something incorrectly, or is there another way? Oh, and we do plan to disregard thickness in our calculation. It's for estimating purposes, and all we need is the square footage of raw material we're using.

Thanks!

 

[MadMango]

You could try an API call to pull the Total Area from the model file, then divide that by 2 to get square area. Sheet metal is usualy thin, so just dividing by 2 shouldn't increase that value that much. I know nothing of the API though, so I can't help further than the suggestion... Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[Morglisn]

Our only problem with that is that we're not using the thinner sheet metal. We're using insulation, which can be up to 3-7" thick.

Thanks!

 

[SBaugh]

You can't add them (Dimensions) to the file\properties\custom of the parts and then place them into a custom BOM? Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.3dmca.com

faq731-376
When in doubt, always check the help

 

[DetroitPickles]

Morglisn,

Can you do this?

If you know the outer dimensions, make an equation that calculates the flat length like you would have years ago with a calculator. In some Sketch, draw a construction line and dimension its length. Make the dimension equal the equation (or is it vice versa?). Don't forget the K-Factor in the equation.

Use can then grab the "dummy" dimension (included in a Custom Property string) as the Sq Ft number to use in the BOM.

Mr. Pickles

 

[Morglisn]

I'll definitely try that. Thanks a bunch!

 

[TheTick]

DetroitPickles:
Your last reply seems to highlight one of the frustrating shortcomings of SolidWorks: the inability to have variables controlled by equations without attaching them to dimensions!

Sorry, just venting. Gravity is a harsh mistress.

 

[DetroitPickles]

TheTick,

You can vent at my posts. I didn't write the program. If I did, I would spend a bucket full of hours working on the drawing portion, instead of "needed" stuff like the little "Shadows in Shaded Mode" button and expanding right-click menus.

But I do send in SPR requests and/or enhancement requests, and sometimes they listen to me....

Mr. Pickles

 

[dhinners]

I am guessing that the source of your trouble is that the dimensions you put in are different between the flat pattern and as-bent? If you go to the flat pattern configuration to put in reference dimensions, they will change when you switch to the as-bent configuration, since the positions of the edges, etc. have actually moved.

Well, you CAN use geometry based dimensions in the BOM for sheetmetal parts. All you have to do is add an unfold feature at the end of your design tree, which will give you your flattened version. Then insert a sketch on this flat face and put in the (reference) dimensions you want to see in the BOM. Then you can add a fold feature after the sketch to bring your model back to its as-bent shape. I know it seems redundant, but its value lies in the parametric dimensions. Since the flattened sketch is created by the unfold feature, the dimensions will always reference the correct geometry.

Let me know if this was unclear, or if I totally missed the point.