Extracting Sheet Metal Extents Parameters in Inventor 2009
Some of you may be aware that in the latest release of Inventor (2009) Autodesk have made the sheet metal extents parameters available as a selection inside text boxes on drawings. But unfortunately the same functionality is not available, should you wish to add this information into a parts list or custom iproperties etc.
After a bit of exploring, we have come up with a work around for this, using the three parameters below:
=<Flat Pattern Area>
=<Flat Pattern Length>
=<Flat Pattern Width>
These can be entered in the sheet metal model iproperties dialogue box, under Custom, see example below. DO NOT name the custom iproperties as Flat Pattern Area/Length/Width as this can cause conflicts. Instead name them Development Area/Length/Width for example. Once you click Apply, the Value equation will disappear, being replaced with a 0.
This is all good except for the fact that the parameters come through as cm and cm^2, which is not a regularly used engineering unit, as many of you will be working in mm or m. But you can format the column unit properties for Flat Pattern Extents Length and Width, unfortunately the Area will always be cm^2, follow the procedure below.
To start with you need to go into the drawing environment (i.e. open an idw or dwg), then to the Format menu, Style and Standard Editor, then under Parts List you can either edit the iso parts list to add the relevant columns. Or in this example we have created a copy of the iso parts list specific to sheet metal parts, which will automatically populate with these new properties. The columns are added by going to Column Chooser and adding New Property, using the same name as in your model iproperties, so in this case they will be Development Length and Width.
After the new columns have been added, you can right click on each of the new rows above to get the Format Column dialogue box up. In here you need to select Apply Units Formatting and mm as the Units, this will then change the values from cm to mm in the parts list table.
Once all of the table has been setup and saved, including saving it back to your Design Data for future use or others to use. You can place a Parts List down on to the drawing sheet and it will populate with the required information as below:
Please Note: A Technical Document for this Tip has been added to the Technical Documents section under Members, called TD0143 - Extracting Sheet Metal Extents Parameters in Inventor 2009.
An easy option for using the flat pattern properties is via the Micro Concepts Inventor Tools program which can be set to automatically populate model parameters with the flat pattern information.