Image Credit: Ken Middleton – Flickr
Did you ever need to manage Autodesk Inventor Sheet Metal Thickness parameters from another file? A good example of using this is in Top-Down Modeling.
Sheet Thickness Function Categories
I have found it to be very good practice to establish function categories in managed parameters, such as ‘SheetThickHeat1’, ‘SheetThickLoad2’, etc. These form the basis for managing the thicknesses of common sheet metal components based on the environmental factors they will experience, or the funtions they will serve.
Let’s take a turbine engine bay concept including internal liner shields, and external casing panels separated by an insulator. Both groups are going to experience thermal stress, but the inner liner is critical, the insulated outer casing is not.
I would assign the following example:
Non-critical thermal loading – ‘SheetThickHeat1’ = SS14Ga
Critical thermal loading – ‘SheetThickHeat2’ = SS11Ga (actually, I might not use stainless, but you get the point)
Brackets that take a heavy bending load would be assigned a different function parameter than sheet metal parts that don’t.
These parameters are developed in the master skeleton file, and derived into every related part file. I assign these parameters as if I were applying a function category to the part. If the client decides that they wish to increase the heat in a critical thermal load area, I can change the SheetThickHeat2 parameter and update the liner panels and every other part that shares that parameter. This process takes a bit of creativity and proper application, but I have found it useful in numerous circumstances.
I load all the gauge thicknesses for my steel sheets in the master skeleton parameters as well. In U.S. military aviation we rarely dealt with sheet steel by gauge, but I run into it a lot on the private side of things. Plus, remembering the conversion in mm from one vendor to another is difficult. Having the parameters named such as SS18Ga makes things easier for me.
Tying the Sheet Metal Thickness to a Derived Parameter
In the distant past you could not do this. There was no avenue and all you could do was enter an override integer.
Sheet Metal parameters in a Read-Only state.
However you can currently achieve this in two ways.
Manually Enter the Parameter in the Style Editor
You may have noticed that Inventor will permit you to pick a parameter from a recent use list, but there is no ‘List Parameters’ option here. No problem.
Simply manually type the parameter in, and Inventor will allow it.
Manually Override the ‘Use Thickness from Rule’ Option
This is a better option.
If you uncheck this option in the Sheet Metal Defaults, the option to use another parameter is enabled, and the ‘List Parameters’ option appears on the right of the Thickness field.
Additionally, this unlocks the parameter field in the Parameter Editor, where you can manually type the derived parameter name, or simply use the ‘List Parameters’ option as well.
This workflow allows very simple changes to a broad use of sheet metal in an assembly design. Some of my clients like to change their minds, and I enjoy providing a little flexibility.
The only warning I offer in this workflow is this: when developing tight features such as in the image below, it is a good idea to leave some wiggle room in the design for thickness increase and manufacturability concerns. If you don’t, you may run out of bending room as the thicknesses increase, and the parts will fail to build.