Export flat pattern properties

[pdecker]

I've found similar requests for this but it doesn't seem to answer what my goal is. I am able to display Flat Pattern Length and Flat Pattern Width on my drawing but I need it to export with the BOM (of the assembly the part is in) so that it can be imported into our ERP program for costing.

[johnsonshiue]

Hi! There are primarily two ways to do that: Custom iProperties vs iLogic Rule.

iProperties:

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2019/ENU/Inve...

iLogic:

https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/part-and-sheetmetal-extents-from-ass...

https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/automated-flat-pattern-dimensions/td...

Many thanks!

[pcrawley · Accepted solution]

Did you use a custom iProperty (or a standard iProperty) to store =<Sheet Metal Length> and =<Sheet Metal Width> so you can show them on the drawing?  

If so, you need to create "Custom iProperty Columns" in the assembly BOM.  Name the iProps you are using for sheet metal length & width - and the data will appear in the assembly BOM ready for export.

[pdecker]

Worked great, thanks

While I'm at it though, is there a similar exportable field/parameter for length of items cut from bar stock or tube/pipe?

[pcrawley]

Glad it worked, and thanks for accepting it as a solution.

For extruded profiles like tube/pipe/bar/flat etc... It's been the subject of numerous threads here, but the short answer is an unhelpful "yes and no".  There's nothing quite like =<Flat Pattern Length>, but depending on how you draw things, you can call other parameters into the Parts List.

If you are placing profiles from Content Centre, then there is a parameter called G_L which is the cut length of product (so you can add =<G_L> as an iProperty).  

If you draw something like a round bar, or flat bar from scratch, then you can easily expose the extrusion length parameter in the same way as =<Flat Pattern Length> - see Re: iProperties Length, Width, Height in Description and how to fix unit to just have " instead of '...

[BAshcroftXN9FJ]

does this help

[Mario.VanWiechen]

This is the I-Logic we use. G_L does work for some parts but is not accurate depending on how Frame generator parts get trimmed. 

Parameter("LENGTH") = Measure.ExtentsHeight

'Setting Part Number to File
If Not ThisDoc.FileName(False) = "" Then
	iProperties.Value("Project", "Part Number") = ThisDoc.FileName(False)
End If

This will give you the full length of the part, if you extrude a shape on a part the G_L will not be the length anymore 

[cadman777]

The way I solved this for FB & SB CC parts is to make them sheetmetal and add to them flat patterns.

The only problem with that is the flat pattern won't always show the cuts.

Example: When I do railing with FB and SQ pickets, I can get the flat pattern length extents for each part.

I haven't figured out a way to do this with any of the other structural shapes, pipes or RB.

However, when using the FG, the thing that fixed the incorrect reporting was learning that there is a sequence to end treatments. First I had to do the Shorten-Lengthen or Miter, and then Cope. If Cope is done first, then the software won't register the length correctly.

Example: Railing post against top railing.

First shorten post to below top rail centerline, then add cope.

If I add the cope first, then shorten/cut, the length reports incorrectly.