Autodesk Inventor 2015: Accessing Sheet Metal Extents information in IDW and BOM
In this post I will take you through how to add sheet metal extents (the length and width of a piece of sheet metal required to make the component) to your bill of materials, which you can then use in your IDW by either adding it to your parts list or by just adding it as text. Please note that this can be extremely helpful if your assembly has a large number of sheet metal components, as this method will get the extents for all components.
Also note that if you want the extents for just a single part then there is no need to create an assembly. The Part will just require that the Flat Pattern has been created to be able to generate the extents.
Fist we need a sheet metal part, so for this example I’m just going to use a simple box I created.
The box is 500mm x 420mm x 200mm high.
So before you’re save your sheet metal part/s make sure to create the flat pattern. Note: the extents will ONLY work if you have already created a flat pattern!
So once your sheet metal part/parts are in an assembly open the Bill of Materials.
Once in your Bill of Materials create two new custom iproperty columns.
Naming one Width and one Length as such and setting the data type to text.
Notice how the Width and Length columns have been added to the Bill of Materials
Then click on width and enter an expression at the top as follows, type in “=<SHEET METAL WIDTH>” for the width.
Then click on the length to edit the expression for the length and you will notice a value will populate the width column/s. Add the expression “=<SHEET METAL LENGTH>” for the length and press enter and notice how the column/s are populated.
Once that is complete you can save and take the part or assembly into an IDW. Depending on whether you add the extents as text or in the parts list will depend on if you need to use the part file or assembly file in the IDW.
To add the extents as Text do as follows:
Select the Text icon from the Annotate tab.
Select the text Icon and place the text where you would like. And the Text Editor will open.
Then make sure you select “Sheet metal properties” from “Type” (In Red). And you will notice you can select different values from “Properties” (In Orange), here is where you select the type of extent you want.
Once you have selected the correct “Type”, “Property” and “Component” select the icon below (In Red) to add the Extent to the text (In Orange). You can then select the other Extent and add that by selecting the other extent (In Green) and select the icon as previous.
When you are happy with the properties you can add some normal text to the window before clicking ok to specify which is which.
Then see the added text in your IDW as below. Notice that they values come out to be the exact measured distances, note I did this to show that the extents are accurate.
When Adding the Extents in the parts list you can add it to a part IDW or an assembly IDW.
So bring the assembly into the IDW and insert the parts list referencing to the assembly.
Once your parts list is in the IDW edit the parts list by right clicking and selecting “Edit Parts List”.
The “Parts List” window will open, so select the “Column Chooser” icon, because we are now going to add the custom Bill of Material “Width” and “Length” columns.
Once the “Column Chooser” window opens, remove or add properties you would like, I’m doing to remove my description column and add two “New Property” columns.
Select the “New Property” icon above in Green. The “Define New Property” window opens, then click to add the properties as below.
Select ok and notice how the properties are added to the “Selected Properties”
Click ok again and notice the columns are added to the parts list as well as their extents. Note that None Sheet metal components will have blank “Width” and “Length” columns. Then select apply and then close the parts list editor and notice the sheet metal extents added to the IDW parts list.
So this concludes adding sheet metal extents to your IDW’s.
Thanks for your Interest,