Alibre Design - How to Drive a Part From a Layout Sketch
In this tutorial I will use a 2D sketch of the layout of a fan scroll to generate a 3D sheetmetal part using Alibre Design Software. When producing a range of centifugal fans the performance of each particular fan in the range is governed by equations called the "fan laws". Once the actual performance of one fan in the range has been established the performance of all other sizes can be predicted by these laws. This makes producing a complete range of a particular type of fan an ideal task for a parametric 3D approach to produce the drawings and other details ready for manufacture. The main dimensions of our fan are based off the diameter of the rotor.
The first step is to create a global parameters file. This feature is accessed from the "File" menu, File -> New -> Global Parameters
A new window will open. Save this file in a location to suit. I save this file in the root directory of the fan I am working on and name it Fan Parameters.
I click on the "New" icon on the toolbar. This opens a dialog box where I create a parameter I name this ROTOR_DIA an give it a value of 400mm as this is the rotor diameter of the fan I am working on.
The next step - Create a new sheet metal part
I have saved this file in the same place I saved the Global Parameters file. I have selected the X- Y plane to create a new 2D sketch.
have started this sketch with a circle that has its center at the origin of the sketch plane, also symmetrical about origin, I have constructed a square, which gives me four points, at corners, to be centers of the four arcs that will be the scroll. From these points, starting with the top left point, three arcs, spanning 90 deg, are struck, working around in an anti-clockwise direction, with the fourth arc only, in this case, swinging through 30 deg. A line tangent to the first arc is constructed vertically upwards. This sketch must be fully constrained and dimensioned as shown. The size of the square uses to generate the arcs that define the spiral the scroll will be constructed from comes from the design of the fan we are modeling. This expansion of the volume of the scroll converts some of the velocity pressure developed by the fan rotor into static pressure. This is part of the designed duty of the fan.
Next, open the function editor and link the global parameter file created earlier. The variable "ROTOR_DIA" in this file now should be available in the function editor. Key dimensions in the sketch, can now be driven by equations using this variable.
Next - Create equations to drive sketch
The first link in the sketch is to name the dimension for the circle that represents the rotor diameter of the fan, say "ROTOR", then in the function editor make this equal to the global parameter "ROTOR_DIA" . For the square that controls the scroll, I have named the dimension for one of the sides "SQ" and made the dimension for the other side to be equal to "SQ", also I have driven "SQ" by the equation SQ= ROTOR_DIA * 0.06. The values to be used are worked out previously to suit the geometry of the range of fans you are designing
It is important to name all of the dimensions that will be used to generate the scroll sheet metal part, RAD_1 is driven from ROTOR_DIA * 0.7. As the value of RAD_2, RAD_3 and RAD_4 are driven dimensions as the value of " RAD_1" and "SQ" fix these, name them as we will use them later. Also name the angle each arc rotates through as we will use these as well. A new plane, plane 1 is created, offset from W - Z plane by the equation "RAD_1 + (SQ/2). A new 2D sketch is created on this plane. This sketch is used to make a sheet metal face that will be the base feature for the scroll. This sketch is made symmetrical about Y - axis and all dimensions linked to equations from the "ROTOR_DIA" variable
Next - Generating scroll sheet metal part
The sketch on plane 1is now used to generate a sheet metal tab. Adjust the sheet metal parameters to suit your requirements ( material thickness etc. )
Use the flange tool to generate the first scroll radius. Make sure you select the "bend only option and the inside edge of the base feature. The radius for this bend is set to "RAD_1" and the bend angle set to "ANG_1".
Use the flange tool to generate the next scroll radius. Make sure you select the "bend only option and the inside edge of the previous bend. The radius for this bend is set to "RAD_2" and the bend angle set to "ANG_2".
Use the flange tool to generate the next scroll radius. Make sure you select the "bend only option and the inside edge of the previous bend. The radius for this bend is set to "RAD_3" and the bend angle set to "ANG_3".
Use the flange tool to generate the next scroll radius. Make sure you select the "bend only option and the inside edge of the previous bend. The radius for this bend is set to "RAD_4" and the bend angle set to "ANG_4".
Completed scroll, and as sheet metal part is entirely driven from one variable in a global parameters file. Editing the "ROTOR_DIA" variable in this file will generate a new size. When designing a range of fans for a particular purpose the geometry is scaled up or down to produce fans with a range of performances for a range of applications. Across this range these performances are obtained by changing rotor diameter and changing the size of the motor to drive it. Using this method, building a parametric 3D model linked to a global parameters file and drawing sheets driven from this model, producing this range of fans, ready for manufacture becomes quite automatic and efficient.