In my post titled Square Holes In Autodesk Inventor?, I promised to give a quick tutorial on how to create a mortising tool as an iFeature, so here it goes…
Inventor iFeatures are incredibly easy to create, and can save huge amounts of time on those tasks you need to perform on a regular basis, and are not already present as a tool in the main program. What it does is allows you to save a feature and its underlying sketch and parameters for perpetual reuse.
How I generally create these is that during the course of regular modeling, I come across a feature that I need to create that I feel will be needed again enough to warrant creating an iFeature. They are very easy to make, so the only problem you may run into is having too many —and possibly having a hard time finding the one you are looking for. Whatever the case may be, one you decide to create on, you just model the feature as you would normally, making sure to create parameters for any dimensions as they will be reused and cam be modified in future iterations of the feature.
In the case of the mortise iFeature, I simply drew a rectangle to rough size right on the part I was creating at the time, then created some positioning crosshairs that are coincident constrained to the centers of the rectangle’s lines (look for the little green dot along with the coincident constrain glyph to let you know you are on center).
The crosshairs were then split with the Split Tool from the Modify panel, and turned into construction lines by selecting all four of them, then selecting the Construction tool from the Format panel. You may need to add collinear constraints between the sets of lines as well if they were not created automatically –in this case, I did have to.
These crosshairs will give me convenient centerlines to measure to if needed when the feature is placed in the future.
Now for some constraints. For the simple mortise needed here, three parameters are all that are needed…… Width, Length, and Depth as can be seen in the User Parameters area in the image below. When the iFeature is created, these will be used to size all future iterations of the feature…
Now the rectangle needs to be sized using the Width and Length parameters, then created by extrude/cutting the profile into the part using the Depth parameter for distance…
….which creates this…
.
It may seem like a long row to hoe just to get a rectangular hole … but in reality it took maybe a minute to do. Once turned into an iFeature, the creation time will drop to a fraction of that. Like a bazillionth of a second or something.
I named the extrusion ‘Mortise’…which I didn’t really need to do to create the iFeature. The feature itself will be named. It’s just good practice to always name features. So do it.
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