The Match Shape, and conversely the Match Contour option is available in the Extrude and Revolve Features. These are not rocket science options, but do occasionally present confusion, either by the situation they are used with, or by the Inventor help available.
When an Extrude feature is created, it expects a closed loop profile, from which it will add a feature perpendicular to the plane the profile lies on. Alternately, an open profile can be selected.
In the image below you should notice a small tray with a sketch containing an open profile dimensioned 20mm x 20mm. The sketch was created on the face of the tray bottom.
Notice in the image, the purple 2D sketch geometry that was referenced from the existing part geometry, and projected automatically when we selected the part face for the sketch plane. This comprises a closed loop profile. What will happen when we try and select the open profile in the corner? This…
The entire bottom of the tray highlights, after automatically selecting the closed loop profile from the projected geometry. The application will not let go.
If we go back into the sketch and remove one of the projected curves, and present the application with an open profile there as well, the application will allow either open profile to be selected.
When the open profile is selected, the ends of the profile are extended into the side of the part (orange arrows), and then the remainder of the open profile is ‘traced’ around the closest edge of the part (blue arrows) until the other extended geometry is met up with.
The remaining options are then processed as if it were a normal closed loop profile
Once an open profile is selected, the Match Shape option becomes selectable, and active by default. While you could have read the Inventor Help for this feature, you chose actually understand the situation….that’s why you are reading this instead. The explanation available with the application is so hard to read.
With the check box off, the application will extrude the part perpendicular to the plane the profile sketch lies on. If Taper is applied for example, the the extrusion is tapered accordingly in all directions parallel to the sketch plane, regardless of the adjacent part edges.
Here is the Match Contour standard extrusion (no taper).
If the Match Shape option is selected, the application still processed the closure of the profile the same way. However the extrusion will be added in a much different manner.
The ‘Flood Fill’ result that Inventor Help indicates doesn’t make any difference along the sketch plane, but what it does do is to fill the exstrusion along the portion of the profile that was ‘traced’ (along existing edges). In the example below, as the standoff is extruded, it fills in to meet the edge of the existing part.
We can also apply a taper at the same time.
The ‘traced’ edges along the part hold the existing part angle, but the sketched edges taper as requested. The remainder of the features act as you would expect, only the ‘traced’ edges of the profile fill according to the existing part edges.