iLogic Tutorial for Creating a SmartPart 1

 In this Inventor iLogic Tutorial we will create a SmartPart that represents all of the hanger bolts used by a fiction small woodworking shop. We will then place it in the Shaker Table model and have it controlled automatically by same.

To begin this iLogic tutorial the first thing we need to do in this  is to define the hanger bolts. A look at McFeely’s turned up the following list:

  

 

With the list of options on-hand, we can get modeling. We could actually not model anything at all and still have the hardware show up on the parts list and the BOM, but we’ll leave that for another day. The shape of the hanger bolt is incredibly simple, so all I will do here is say that you should make it to roughly three inches long, and have the following constraints added (during drawing if possible, otherwise add them)…

 

 

 

 

 

 

You also need to create the parameters Bolt_Diam with an equation of 5/16” and Bolt_Length with an equation of 3”. Also note that the left line, the one constrained to the Origin Point, is a Center Line. Now we can add the constraints.

With all of that done, you can add the dimensions to fully constrain the drawing. Two things to note:

The arc at the top that will create the bolt’s point uses the formula Bolt_Diam * 3 UL (the UL stands for unit less), and the Bolt_Diam dimension goes from the Centerline to the right-hand line (for those who are unfamiliar with how centerlines work in Inventor).  

The arc formula should give a decent look throughout the range of adjustment –remember, we are not manufacturing a hanger bolt, we are just looking for a realistic looking representation.

 

 

 

 

 

Now hit the R key on your keyboard. You should see the following…

 

 

 

 

 

 

 

…which means you are good-to-go. Click OK to accept. You now have a hanger bolt blank.

Now we need to add some threads. Since there is a blank area in the middle and several lengths of bolts, we need to create a formula for the thread lengths.

I came up with 2/5 of the length, but on the pointy end, we will need to subtract the point itself since the Thread tool only works on cylinders (fix it Autodesk!). We could use the Coil tool and put some real screw threads on it, but that would be a tutorial all is itself. If you are interested, you can use the Q & A link and ask….

 

 

 

 

 

 

So in order to create one of the formulas we need to know the length of the point, so you need to double click on the sketch in the Browser Bar to go back to the sketch, then add a driven dimension to the point as shown below…

 

 

 

 

 

 Once this is done, right click on the dimension you just made and change the name to Point_Length (you are changing the name in the parameter table), and now would be a good time to name the features in the Browser Bar as well (Hanger Bolt and Layout). Now for the threads themselves. Grab the Thread tool and click on the bolt end of the hanger bolt, then enter the formula:(Bolt_Length / 5) * 2ul for the length. Switch tabs and double check the details. They should be like those to the right automatically. 5/16”–18 is what we need.

 

 

 

 

 

 

Now for the formula, click the little arrow in the Length box, and choose the same one we just made from the list of recently used dimensions. Modify the formula to remove the point length as such:

(( Bolt_Length / 5 ul ) * 2 ul ) – Point_Length

 

 

 

 

 

 

 

 At this point I added a .02 chamfer on the bolt end to make things look right, and did a bit of renaming of the features as can be seen in the image to the right…

 

 

 

 

 

 

Now for some assembly. Create a new assembly called Hanger Bolt, and place the Hanger Bolt part in it. Then select Place from Content Center from the drop-down menu on the Place panel, and choose the Hex Nut – Inch from the library…

 

 

 

..you will then get the ever so cool AutoDrop placement help which is slick as snot, with one exception –you cannot place a part as ‘Custom’ as you can with the old-school placement dialog. Whatever…. we don’t need a custom part, so we can just click to accept the part, then right click and choose Place to end the operation.

 

 

 

Now to place a washer in the same manor. We will place it on the back side of the nut, and it should constrain itself to both the nut and bolt.

 

Fasteners > Washers > Plain > Circular Washer (Inch)

 

 

 

That’s a good place to stop for today. A bunch of code and some more Content Center stuff coming in the next installment, which should be tomorrow….. but there’s a blizzard going on here so one never knows. Later.

 

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