Tip #4 - Parametric Part Rotation

Note: This tip will work in both versions 2.0 and 3.0 of Mechanical Desktop®.  This tutorial was based on the use of version 3.0.  You will have to construct the parts using local or active part variables in version 2.0 to be able to take advantage of linking to Excel.

Hello and welcome to the fourth installment in our series of Mechanical Desktop® tips and tricks, Parametric Part Rotation.  In working with pressure vessels (of course this tip can be applied beyond this application!), I have found that there is no such thing as a standard configuration.   Each customer wants different sizes, elevations and orientations for the connections required.  The previous tips have shown how to handle changes in size, configuration and even if the connection is visible.  In this installment, we will talk about how you can control orientation of parts using variables.   (This tip also demonstrates how through using global design variables, you can create features and cut outs in parts based on other part's geometry.)

In this very simplified example, we will construct a circular shell with a cutout for a perpendicular nozzle.  We will then create a circular nozzle and constrain it to the shell so that both nozzle and nozzle cutout can be rotated (0° - 360°) about the shell's center line using variables.  We will create this example using global part variables and utilize version 3's ability to table link them.

You should now have Mechanical Desktop® open and be ready to create a new part. Following are step by step instructions to create the shell and nozzle.

Step 1 - Create the Variables
Table 1 shows the variable names and values to create.  Figure 1 is a screen shot of the AMVARS dialog showing all the variables required. (Note: The variable nozzle_elevation is not shown in Figure 1.)

Figure 1.

Step 2 - Create the Basic Shell Part.
Profile and extrude a cylinder using shell_od as the diameter and shell_height as the extrusion depth.   Using the shell command (AMSHELL), create an open ended cylinder with a thickness of shell_thk.

Step 3 - Create the necessary Work Planes.
 First, create a work axis on the cylinder (see Figure 2).   We will need a work plane to act as the base reference for the rotated work planes.   Figure 2 shows that I have selected "North" as my 0° direction.  Create a work plane normal to this 0° - 180° axis by using the "On Edge/Axis" and "Planar Parallel" modifiers.  Select the work axis and World ZX as your input to create the work plane (the "black" plane in Figure 2).  Now we must create the rotated planes that will act as the base for our rotated feature (the nozzle cut out in the shell) and part (the nozzle).  This could be accomplished with a rotated work plane.  However, like most of the angular assembly constraints, input is limited to 180°.  How do we accomplish a full 360° rotation?  The solution is to "piggyback"  2 rotated work planes.   In other words, rotate the first work plane half the desired rotation from the base work plane and rotate the second work plane half the desired rotation from the first work plane.  In this way you can get a full 360° rotation (180 + 180) without exceeding the limits of Mechanical Desktop®.   To do this, create a work plane rotated from the base work plane by using the "On Edge/Axis" and "Planar Angle" modifiers.  Input the variable plane_rotation as the specified angle. Select the work axis and the base work plane (the "black" plane in Figure 2) as your input to create the new work plane.  "Flip" the work plane so that it is rotated clockwise from the base work plane and accept (see the "green" plane in Figure 2).  The last step is to create the second or "piggy-backed" work plane that will be used as the base for our further work.   Create a work plane rotated from the second work plane by again using the "On Edge/Axis" and "Planar Angle" modifiers.  Input the variable plane_rotation as the specified angle. Select the work axis and the second work plane (the "green" plane in Figure 2) as your input to create the new work plane.  "Flip" the work plane so that it is rotated clockwise from the base work plane and accept (see the "magenta" plane in Figure 2).   The shell should now look like Figure 2.  Please note that I have added the 0° annotation and reference line, and modified the work plane colors as noted above for clarity.

Figure 2.

Step 4 - Add the nozzle cut out feature in the shell.
First we must add one additional work plane to position the nozzle cut out (and the nozzle) feature.  This will position the nozzle from the base of the shell (The nozzle elevation).  Create a work plane offset from the base of the shell by using the "Planar Parallel" and "Offset" modifiers.  Input the variable nozzle_elevation as the specified offset. Select the bottom face of the shell as your input to create the new work plane and "flip" so that it is positioned above the base of the shell (see the "cyan" plane in Figure 3).  Now we can add the cut out feature.  First, to avoid clutter and confusion, turn off visibility of the "Base" (black) and "First" (green) rotated work plane.  We must now set the sketch plane to the second (magenta) rotated work plane.  This insures that the cut out profile rotates parametrically with the work plane as the rotation value is changed.  After you have done this, draw a circle and profile it.  This circle will be the hole cut out in the shell.  We must constrain this to the elevation work plane created earlier and to the center of the shell.  This is done using the Project constraint.  Select the center of the circle (using the CENTER object snap) and then select the elevation (cyan) work plane.  Using the project constraint again, project the center of the circle to the shell work axis.  Now dimension the circle with a value of nozzle_od and you should have a fully constrained sketch.  Using a cut extrusion, extrude the circle to the outside face of the shell (the direction should be in the "2 o'clock" direction) to create the nozzle cut out.  Finish up by adding a work axis for the nozzle cut out.  The shell should now look like Figure 3.

Figure 3.

Step 5 - Create the Nozzle Part.
Create a new part and name it "Nozzle".  Profile and extrude a cylinder using nozzle_od as the diameter and nozzle_projection as the extrusion depth.   Using the shell command (AMSHELL), create an open ended cylinder with a thickness of nozzle_thk.  Create a work plane that is planar parallel and flush to the bottom surface of the nozzle (this plane will mark the center of the shell when we "fishmouth" the nozzle) by using the "Planar Parallel" and "Offset" modifiers.  Enter 0 (zero) as the offset distance and select the bottom face of the nozzle as your input to create the work plane (the "magenta" plane in Figure 4).  Create a work axis on the nozzle.   Now we add a work plane to act as a base to create the "fishmouth" cutout feature.   Create a work plane by using the "On Edge/Axis" and "Planar Parallel" modifiers.  Select the work axis and World ZY as your input to create the work plane (the "cyan" plane in Figure 4).  The Nozzle should now look like Figure 4.

Figure 4.

Step 6 - Create the "fishmouth" cutout in the nozzle.
Set the sketch plane to the second (cyan) work plane.  After you have done this, draw a circle and profile it.  This circle will cut the "fishmouth" cutout (The shell OD) in the nozzle.  We must constrain this to the base or center line work plane created earlier and to the center (work axis) of the nozzle.  This is done using the Project constraint.  Select the center of the circle (using the CENTER object snap) and then select the base (magenta) work plane.  Using the project constraint again, project the center of the circle to the nozzle work axis.  Now dimension the circle with a value of shell_od and you should have a fully constrained sketch.  Using a cut/mid plane extrusion type, extrude the circle using a value of nozzle_od as the extrusion distance to create the "fishmouth" cut out.  The nozzle should now look like Figure 5.  Both Parts are now complete and ready for assembly.

Figure 5.

Step 7 - Add the assembly constraints.
The assembly process is completed by adding a Mate constraint between the work axis of the nozzle and the work axis of the shell cutout.  This keeps the nozzle and shell cutout aligned during rotation.  Next add a Flush constraint (with a 0 (zero) offset) between the base (magenta) work plane of the nozzle and the second rotated work plane (magenta) of the shell.  Finish by adding another Flush constraint (with a 0 (zero) offset) between the elevation (cyan) work plane of the nozzle and the elevation (cyan) work plane of the shell.  The completed model should now look like Figure 6.

Figure 6.

Step 8 - Link the variables to the spreadsheet.
Using the AMVARS command, link the global parameters to an Excel spreadsheet.   Edit the spreadsheet as shown in Figure 7 to add the additional configurations.  We have renamed the "generic" values to "Size 1" and added values for 2 other possible versions for the part, "Size 2" and "Size 3".  Update the link and return to Mechanical Desktop®.

Figure 7.

Step 9 - Update the Part!!!
The browser will now show 3 possible configurations for the part (you can add as many as you like!!!), see Figure 8.  All you need do now is double-click on the version name that you wish to activate in the browser and the shell and nozzle will update automatically.  Figure 8 shows the "size 2" configuration (notice the 200° orientation/rotation) and Figure 9 shows the "size 3" configuration (notice the 300° orientation/rotation).

Figure 8.

Figure 9.

Wrap Up
This technique becomes especially useful in configurations where you have 2 or more nozzles or parts to rotate (I have built one with 16 different nozzles).  Good Luck and please let us know if you found this tip useful.

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