Methods of Sharing Parameters Between Inventor Parts - Part 2

In this article I would like to continue with the methods of sharing parameters between Inventor parts.  If you missed the first article, I suggest you click here to review it before continuing.  The second method of sharing parameters is linking parameters between parts.  The process begins inside the Inventor Parameters table which can be opened from the Quick Access Toolbar, if it is enabled, or from the Manage tab on the Parameters panel.

I am using the same part model from the first article which contains two model parameters and one user parameter.

I will next create a new part and open up the Parameters table.  At this point it is empty because I do not have an saved parameters in my Inventor part template.  I will click the "Link" icon at the lower left of the table.  At the bottom of the resulting Open dialog box I have selected "Inventor Files" as my file type and selected the Hole Plate,ipt as my source file.  Select "Open" to continue.

The Link Parameters dialog box opens and you have to opportunity to select which model parameters you wish to link with the new part.  The small green arrow means these parameters have been exported from the referenced model.  Select the gray ball beside each parameter to enable linking and select again to return to a non-linked state.  I have selected all three parameters.  If you remove the check mark beside"Show All Parameters" only the exported parameters will be available for selection.  Select "OK" to continue.

The selected parameters will appear under User Parameters in the Parameters table listed under the path of the file they are referenced from.  They cannot be edited in this state which is indicated by the gray background and will automatically update if the source file parameters change.

Starting a new sketch, you may wonder how to use the parameters directly in the sketch dimensions.  The familiar ">" symbol on the right hand side of the dimension box is not available which would allow you to select model parameters from a list.  A little trick to make the selection symbol appear is to type the "=" key, then you can select parameters from the drop down list.

After you have used the linked parameters, they will appear under the Model Parameters in the Parameters table.  

The Lgth and Width parameters are still linked to the Hole Plate.ipt and will update automatically if the parameters change in the referenced model.  There will be times when you desire to break the link between the new part and the referenced file.  This is easily accomplished by two methods.  The first is to open up the Parameters table in the new part, right click on the linked file path and select "Delete Folder".  This will break the link for the Lgth and Width parameters turning them into editable User Parameters since they have been used.  The Hole_Dia parameter will be lost because it has not been used in the new part.

If you desire to break the parameter link for one or more parameters and retain the parameters that have not been used, right click on the reference file and select "Edit Folder".   In the Link Parameters dialog box you can deselect the parameters you which to break the link.

The resulting Parameter table is shown below.  The Lgth and Width parameters become User Parameters independent of the referenced part and the Hole_Dia remains linked and available for use in the new model.

In the next article I will cover the other two options for sharing Inventor part parameters.