BOM parameters to determine Sq. Ft. of material

[gerrard.hickson]

I just had a quick crack at it now, and I managed to get the area from the model to appear in the drawing parts list but that was using parameters Area = Length * Width so it'll work well enough for a simple rectangle... I can't see any simple way of achieving the same thing for a more complex shape without using VBA. I'll have another look at a VBA solution tonight at home if I get the chance.

[lgunter]

Thanks I will try the formula and see if I can get it to work, Thanks

[lgunter]

Please excuse my ignorance but I go the custom properties to display in the parts list accurately but I could not the formula "Area = Length * Width" to work is there a symbol or certain way of typing this to get it to calculate?

[gerrard.hickson]

Sorry for the late reply, I don't get the notification e-mails, and i just plain forgot about the thread... I've listed what I did below, but it might not be what your after, and there might be problems with it that I don't know about... I've never used it in practice, it's just something I figured out now since you've asked the question. Have a look, see if it does what you need.

So, the steps I took won't translate literally for you since your not using 2009 SP2, but it goes something like this (once you've got the basic gist, you can adapt it to your application).
1.Open a New part file (.ipt)
2.First sketch, I drew a simple rectangle, constrained it as I pleased, then added dimensions for length (i typed "length = 100", and that automatically adds a parameter called "length" so you'll have to manually open your parameters window (not custom properties) and create a parameter called "length") then I did the same for width
3. Then I opened the parameters window, and created a new user parameter called "area" and set it's equation to "length * width". Then I clicked the "export" button, which is on the same line as the rest of the options for the parameter name "area". Then I closed the parameters window.
4.Open up the iProperties for the part, go to the 'custom' tab. You SHOULD see "area" with some value next to it. in my case 500
5. Save your part file as you would normally.
6. Open up a new drawing (.idw) and insert a view of the part you made above.
7. Insert a parts list, then double click on the parts list to open up the edit window.
8. Click the "Column Chooser" button in the top left
9. Click "New Property" down the bottom left.
10. Click "<<Click here to add new property>>" and type in "area" (exactly as you typed it in the parts parameters.
11. Click 'OK' to exit out of the 'New Property' window
12. Click 'OK' again, to exit out of the 'Column Chooser' Window.
13. Click 'OK' again, to exit out of the 'Parts List" window.
14. If you don't see your "area" parameter shown in your parts list, something is wrong.

[gerrard.hickson]

Did you have any luck with this one at all??

It would be great to hear some feedback if you get the chance...

[jon.ottewell]

If you're able to use the sheet metal template to create your parts, this is even easier. Inventor automatically calculates the area you're asking for in sheet metal. Finding it can be a little difficult, so I've attached a screenshot showing where to look.

I've created a simple sheet metal part, placed it into an idw, and now have the leader text edit dialog box open. We insert the area by selecting Type as 'Sheet Metal Properties' and Property as 'FLAT PATTERN EXTENTS AREA', then clicking the x down arrow button.

It's also worthwhile to note that setting type as 'Custom Properties - Model' will give you access to any model parameters you marked for export.

I've found this knowledge to be a big help in my day to day work, and hope others find it equally useful.