Recently I published an article on the Inventor "Redefine" command which was used to redefine the plane or face a feature sketch was created on. This article is about another valuable tool found in both in the part and assembly environment. In the title I placed "Work" to emphasis that the "Redefine Feature" command is used to change the location and orientation of any existing Inventor work feature in the model. The power of this process becomes evident if a feature or a sketch is connected to the work feature being redefined. In my model below, the side extrusion sketch has been created on a work plane which is parallel to the origin X-Z plane and tangent to the outer diameter of the model.
The extruded feature is modeled 180 degrees from the end keyway. The design has changed and the feature needs to be at 90 degrees to the keyway on the front side. Thinking back to the steps used to originally create the feature, you realize it will take quite a few steps to re-model it. This situation is a perfect example to use the "Redefine Feature" command. The theory is simple, since the feature sketch was placed on the created work plane, use the command to simply redefine the location of the work plane and the sketch and the extrusion will follow. Any valid method can be used to create the redefined work plane, in this case the same method will be used except the origin Y-Z plane will be used as the reference plane. Along with the selection of the outer diameter of the model the work plane will be redefined to a new position carrying the feature sketch along with it.
Right click on the sketch work plane and select the command "Redefine Feature".
At this point the extrusion feature will disappear but do not worry, it will return after the work plane has been redefined. Select the origin Y-Z plane and the front outer diameter of the model. The work plane appears and the extrusion moves to the new design location. How is that for speed?
Occasional when using the "Redefine Feature" tool to redefine a work plane, the resulting work plane will develop with the "normal" side pointing to the model. This will cause the existing extrusion to fail because the extrusion direction is pointing away from the main model. There are two quick fixes for this condition, I will mention both so you can choose. Below I have redefined the work plane to the back side of the model. You will notice that the extrusion has failed and the light orange side of the work plane is toward the model. I am right clicking on the edge of the work plane and selecting "Flip
Normal" from the menu. This will correct the extrusion.
The other solution is to select the extrusion feature and right click. From the right click menu select "Edit Feature" and simply reverse the direction of the extrusion. Remember there are always more than one way to do anything in Inventor!
I must warn you that if the work plane has been used to create or define other model features or work features, the process can get complicated. Plan well and your Inventor models will be easy to use the "Redefine Feature" command to make changes. Do not forget, this command works on work axis and work points as well.