# iLogic Tutorial for the iDoor – 05

## iLogic Tutorial – Continuing the hinge skeletons (sketches)

Rename this sketch Sm Hinge Layout. Rotate the part by clicking on the Back face of the View Cube
which will stand the part up and place the sketch normal to the screen. Now window select all of the geometry and right click anywhere in the graphics window. Select Properties. The Geometry Properties dialog box will pop up. Change the Line Color from Default to Red. This will help differentiate geometry later.

We will now draw six lines, each one beginning on one of the six points  in the sketch and going a short way, an inch or so, towards the top something like the image below…

To these lines we will add a formula. The standard offset is 3 �” from each end. There is also a 2 �” offset that will be used on very small doors. Instead of recreating what we already have, we will just subtract one from the other and use the difference to locate the small version. To do so, get the Dimension tool  from the Constrain Panel and select one of the lines (an outer one will make things easier – see below)

Enter the following formula  Hinge_Offset_L – Hinge_Offset_S by going to the parameter list and choosing the first selection, Hinge_Offset_L then add the minus sign -which will turn the equation red – then go back to the parameter list and chose the Hinge_Offset_S parameter. The equation will now turn black as it is a valid equation. your dimension should now read fx:1.250

Now go to the Constrain panel and get the Equal constraint tool and click on the line that was just dimensioned. Do the same for all lines, making sure to start with the same, dimensioned line. If you were to create an equal constraint to one line, then from that line to the next, and continue on that way, it would be called daisy chaining. Daisy chaining is easier to do, but uses more resources and can slow down the model’s responsiveness. Its a bad habit to get into –don’t do it. Now you need to add Points to the tops of each line just drawn, and add and dimension circles just as you did in the first drawing. Again, these are just to add clarity when creating the holes in the next step. The big, inner holes are the Hinge_Cup_Diam parameter and the smaller, outer ones are the Hinge_Dowel_Diam parameter. make sure the circles are not centered on the red points. Click the Finish check mark on the exit panel (its the only tool on the panel) and save.