Inventor parameters control the shape and size of all part and assembly models. Parameters are added automatically every time you add a dimension to the model but they are not intelligently named. Inventor places the familiar d1, d2 … variable on the dimensions as they are placed. This leads to confusion if you are trying to reuse previous parameter values in newly created dimensions especially as the complexity of the model increases. In order to make the parameters more meaningful, they are often named to describewhat each parameter controls.
A note here about renaming parameters, they cannot contain spaces or special characters (+ / * etc.). There are two types of parameters, Model Parameters and User Parameters. Both have their uses but User Parameters can exist even if their supporting model dimensions are erased, model parameters will disappear. In the parameter table shown below if all the model dimensions in the part were erased, the user parameters would be maintained.
One of the main objectives, as you model multiple parts, is to either copy the parameters from one part to another or share them. Copied parameters are independent of their values in the original part. Changes in the original part parameters will have no effect on the part that the parameters were copied to. Shared parameters are dependent on the original part parameters. If the original part parameters are changed, the share parameters are updated and the new part changes accordingly.
There are five methods of copying or sharing parameters between models. These include:
- Copying of the parameter table
- Deriving a part into another or an assembly
into a part - Linking parameter tables between parts and
assemblies (Excel tables can be linked but is not covered in this discussion) - Copying and Pasting Features between parts
- Copying and Pasting Inventor sketch blocks
between parts
Of these, the first three are the main methods of copying and/or sharing parameters. This discussion will cover these.
Copy Parameters Table
Copying parameters between parts or assemblies is two-step process. First open up the original Inventor model and select the Manage tab. Select the down beside the panel name on the Parameters panel. This will reveal the Import from XML and Export to XML commands.
Select the Export to XML command. You can accept the default file name, which is the <filename>-params.xml, or change the name to suit. Open either an assembly or part file, return to same location and choose Import from XML.
One of the best parts about this process is that the copied properties are placed in parameter table as User Parameters even if the copied properties were Model Parameters.
If the parameters are copied into an existing model and some of the parameter names are the same, the model is updated to match the imported values. This process can be between parts and assemblies and assemblies and parts.
Deriving a Parameters Table
The Inventor Derive command is only available in the part environment. The Derive command is
mainly used to create shared parameters between models but it can be used to copy parameters. This will be my focus. You can derive parameters from either a part or an assembly into another part. The Derive command is a bit different for each so first we will derive from a part. Create a new part or open an existing one. Start the Derive command and browse to the part you wish to derive from and open it. In the Derive Dialog box deselect all features except the parameters you wish to copy. NOTE: In order to deselect the Solid Body, you will have to remove the check mark beside the design view link button indicated by the arrow. One nice feature of this method is that you can pick and choose which parameters you wish to copy. Click OK to finish.
Checking your new part parameter table, you see all the selected parameters are copied as User Parameters. At this point the properties are still linked (shared) with the original part as indicated by the gray background.
In this discussion I am talking about copying parameters so I will remove the linking to the original part. In the Browser, right click on the derived part and select Break Link With Base Component.
The parameters are no longer linked to the original part.
Copying parameters from an assembly to a part is the same in principal but the Derive dialog box is a bit different. Start a new part or open an existing one. Start the Derive command and browse
for the assembly file containing the parameters you want to copy. Open the file and Derived Assembly dialog box will appear. Select the Other tab and expand the parameters and select the ones you want to copy.
As described earlier, the parameters come in linked (shared) with the original assembly. Right click on the derived assembly in the Browser and choose Break Link With Base Component to create copied parameters.
In both cases, you can delete the Derived part or assembly from the browser if copying the parameters was its only function.
Linking a Parameters Table
Parameters tables can be copied using the Link command between all types of Inventor models.
The main purpose of linking parameter tables is to create shared parameters to control multiple features and model conditions but it can be used to copy parameters between files. This is my main focus in this discussion. I will be copying parameters between an existing part and a new one.
First I create my new part. Next I open the Parameters table from the Manage tab, Parameters panel.
At the bottom of the Parameters Table, select the Link icon.
In the Open dialog, select Inventor Files in the Files of Type dropdown at the bottom. Browse for the file you wish to copy parameters from and select Open.
In the Link Parameters dialog box, select all parameters you wish to copy from the original part. Please note you can copy any type of parameters that existing in the original part. You are not restricted.
Linking commands is mainly used to create linked (shared) parameters between files. As stated before, my focus of this discussion is how to copy parameters only.
If you wish to remove the link (sharing) of the parameters in the new part you will first need to use all the linked parameters in the part model. When you have used all the linked parameters you need, right click on the linked folder and choose Delete Folder.
Inventor will only retain the User Parameters that were used and remove the rest. It also breaks the parameter link to the original part.