Working with parameters inside Autodesk Inventor are an inherent part of developing the design, the parameters are used to store (amongst other things) the dimensional values for sketches, extrusions, fillets, chamfers etc. Whenever you input a numeric value for a sketch or feature, the value is stored as a parameter that can be re-used and edited at any time. To access the list of parameters, just click on the Parameters button on the Manage ribbon, or from the Quick Access Toolbar (QAT) at the top:
By default, parameters are given an ID, starting at d0 for the first dimension created within the document and then named sequentially for every subsequent parameter created i.e. d0, d1, d2, d3 etc. Now as you have probably guessed by now, the more complicated your design, the more parameters you will have. You could end up with hundreds of parameters.
Autodesk Inventor gives the user the ability to change the name of the parameter so that it means something more valid to the user. When creating a dimension in a sketch just add the name as part of the input:
In this example, d0 will be automatically re-named to be listed as 'height' in the parameters list. It also means it's easy for us to re-use this parameter in other dimensions. In the example below we have typed in the parameter name as part of the equation:
Whenever we use a parameter name instead of numeric value, when the included parameters value changes, any sketch or feature the parameter is used in will automatically update. But what if you don't know the parameter name, well we can easily access a list of all the named parameters by clicking on the black arrow at the end of the Edit Dimension dialogue and then select List Parameters. You will be given a list of parameters to choose from and re-use:
One tip that I use is within the parameters dialogue itself, if you hover over a parameter name it will tell you in a tooltip which sketches, features and other parameters (as part of an equation) it is used in:
In the example above, the tooltip is telling me that the parameter lip_height is used within the parameter thickness (which you can see a couple of rows below lip_height) and also in Sketch1.The tooltip will also show us the name of any features the parameter is used within:
If feature(s) are renamed in the model browser to something more appropriate e.g. from Extrusion1 to Lip_Extrusion as above, the tooltip will automatically update to reference the new feature name.
In the example we have been working with 'lip_height' itself is actually equal to the parameter 'width'. But what happens if we change the names of the parameters?
Well if I change the name of the parameter called 'width', so it has a new name of 'depth', any parameter that uses that as part of an equation will be automatically updated, and any sketch or feature that uses that parameter will also be automatically updated. The screen shot below shows the parameter 'width' is now called 'depth', and the equation that contained 'width' now contains 'depth':
And we can see in the screen shot below that the sketch that uses these parameters has also been automatically updated:
So the final thing on managing and working with numerical parameters in Autodesk Inventor is how they are displayed within a sketch. You can select exactly how you want them to be displayed by right-mouse clicking in the sketch environment (ensuring you have nothing selected) and then choosing Dimension Display. The five options will change the way sketch dimensions are displayed:
- Value shows the nominal dimension.
- Name shows the dimension as a parameter name.
- Expression shows the dimension as an expression.
- Tolerance shows the tolerance for the dimensions.
- Value shows the dimension value, ignoring any precision setting
The 'fx' in the example above denotes that the value is a calculated value and not an input static value.
