Pro/ENGINEER Tutorial 4 - Simple Assembly 

In this tutorial we will be assembling a mug with its handle and its lid. We will combine the previously learned commands from the earlier tutorials with the following commands:

Creating the mug body

Start by going back out to the desktop and creating a new subdirectory called tutorial4 to put your files for this tutorial in. Assemblies require all related part files to be present for the assembly file to open up properly. The best way to make sure that none of the part files are accidentally erased is to keep them all in a separate subdirectory

Return to Pro/E and set your working directory:

file>working directory (choose tutorial4)
With the working directory set to your new subdirectory, you can start making parts in it.

Let's start by creating the mug body part and call it tut4-mug. First we will create the default datum planes.

create>datum>plane>default

Once the datum planes have been created, we will create a revolved part (sketch shown in Figure 1) using the following commands:

create>solid>protrusion>revolve | solid | done>one side | done

Pick DTM3 as the sketching plane and DTM2 as the top reference plane.

NOTE: This profile section will give you a lot of trouble if you don't do the following:

Remember to use what you have previously learned for aligning, dimensioning and regenerating geometry and datum planes. Once you have drawn the geometry and regenerated successfully, pick done.

Figure 1.

Two rounds need to be added to the mug body (highlighted in red in Figure 1a). Pick the bottom edge only using:

create>solid>round>constant | Edge Chain | done>Tangent Chain | (select bottom edge) | done

Set the radius of the bottom edge to 0.20. Circular edges are broken into two semicircles. The Tangent Chain option picks both of them in one click.

Add another round on the top edge with a radius of 0.10.

Figure 1a.

Next we are going to use the sweep command to attach the handle to the mug. Sweeping is a more advanced feature operation which is done in two parts. Instead of sweeping a sketch profile along a linear (extrude) or circular (revolve) path, a path sketched by the user is used. The first stage is to sketch this path (trajectory):

create>solid>protrusion>sweep | solid | done>sketch traj>Use Prev | okay

You can use the same datum sketch plane and horizontal datum plane as above by choosing Use Prev when prompted for a sketch plane.

Start drawing the trajectory at the arrow on the right side of the mug as shown in Figure 2 . Do not forget to align the beginning and ending points to the side of the mug. Place dimensions as shown. 

Hint: You can use mouse sketch to draw this path.

Figure 2.

Once the trajectory has been sketched and properly dimensioned, perform the following:

regenerate | done>merge ends | done

Now notice the intersecting chain lines on the center left-hand side of the screen (see Figure 3). This view is normal (perpendicular) to the first line segment of the trajectory (the one with the arrow and the chain line intersection marks the location of the first point of the trajectory. We are going to use this as the cross section for the handle during the sweep.

Zoom in on the cross hair and draw the sketch as shown in Figure 3. Make sure you place the sketch as shown in the figure. The bottom of larger arc should be tangent to the vertical chain line after regeneration. All dimensional constraints need to be tied to either elements of the sketch or to the chain lines.

Figure 3.

Once this feature is done, the mug body is complete. Make sure to save your file at this point.

Creating the mug lid

Now create a new part and call it tut4-lid.

Again, create the default datum planes.

Create the base feature for the lid as a revolved protrusion. Use the same sketch (DTM3) and reference (DTM2) planes you used for the mug body. Sketch the geometry shown in Figure 4. being careful to align and dimension as needed. Remember to align the centerline with DTM1.

NOTE: When you create a second part, the old part is not closed out. Instead, a new, smaller window is created on top of the other part's window. You will notice that the new window is the 'active' one because it has a series of asterisks (*******) on either side of the file name. You can switch active windows by choosing the appropriate file name under the Windows menu above the tool icons. From this menu, you can also close windows you are not using. 

 

Figure 4.

We are now going to cut out the material on the bottom of the lid:

create>solid>cut>extrude | solid | done>Both Sides | done

Use Previous sketch and reference planes. Sketch the geometry shown and dimension accordingly as shown in Figure 5. Make sure to align the angled line to DTM2 and the horizontal line to the side of the lid. Note the dimensional constraint scheme. You should tie the horizontal dimensions to DTM1 since the vertical side of the lid you see is the limiting extent of a curved surface which varies in distance to the angled end of the sketch. After you have regenerated successfully, pick done, and make sure your arrow is pointing in the correct direction for the cut.

Figure 5.

Now we are going to use the shell command to cut out the inside portion of the lid. Shelling is a technique used extensively in the design of injection molded plastic parts. Shelling allows you to define the exterior form of the part through solid modeling operations like the ones used to date, and then 'hollow out' the interior with the shell command. You can define a constant wall thickness when shelling out or select surfaces with different thicknesses. There has to be an entry point for the shelling (i.e., you can't create a void inside of a solid), so you must define the shelling operation by picking the surface to be removed:

create>solid>shell

Pick on the top surface of the lid and click done.

The next menu, the feature reference menu, queries whether you want to add additional references for specifying different thicknesses. Pick Done Refs.

For the thickness type in 0.10 and press enter. Next pick OK and the shell should be created. Check to make sure by comparing with Figure 6.

Figure 6.

Next we will create a punch through the lid to create a place to drink through (see Figure 7).

create>solid>cut>extrude | solid | done>one side | done

Use DTM2 as your sketch plane and DTM3 as your reference plane.

Feel free to zoom in on the area where you are sketching. Sketch and constrain the notch as shown in Figure 7. Don't forget the align a horizontal center line to DTM3.


 

Figure 7.

After successful regeneration pick done and make sure to orient the arrow to the portion of the notch to be removed. The cut can be made Thru Next. The end result should look like Figure 8.

Figure 8.

Creating the assembly

The last part of the tutorial will invovle a new 'module' of Pro/E, Assembly. In this module, you will bring the two parts, the mug and lid, together into the assembly. The parts are not copied, but referenced, in the assembly. This means that you can't move or delete the part files referenced in the assembly.

Note: You can use the assembly instructional sheet to help with creating the assembly. 

Create a new assembly by going to:

file>new

Now you need to change the File Type to Assembly. Then enter tut4-assm for the file name.

Initially, the assembly is empty. We create the assembly by placing parts or other assemblies (called 'components') in the assembly window. The first part we will bring into the assembly is the mug:

component>assemble> (choose tut4-mug)

The mug part is retreived and placed in the assembly window.

Now a second part will be placed in the assembly. Pick on assemble again and choose tut4-lid.

Notice that a new window opens at this point. One window, the component placement dialogue, helps track the progress of constraining the new part (component) into the assembly. The other window is the part window of the part you are bringing into the assembly.

First, make sure that assembly is checked in the check box so that you can constrain the new component in the assembly window, rather than having to switch back and forth between the part and assembly windows.

Note: You can use the Move tab and the options contained under it to move the lid closer to the mug while you constrain it. 

In order to bring in another component, it must be constrained to the initial part. Even though you can see the lid in the assembly window, it will not stay there if you clicked on done at this point. Constraining is done through two primary types:

These two options, plus others, are found under Constraint Type. We will start with a Mate.

First pick the top-most (outer ring) surface of the mug. Notice this surface is now listed under Assembly Reference in the dialogue box.

Then pick the matching surface of the lip for the lid (you will may need to use query select to pick this surface). Imagine these two parts going together to figure out which surfaces to pick. Zoom, rotate, and pan as necessary to pick your surfaces.

Notice that the lid has moved slightly, but not in place on top of the mug. We have only constrained in one of the three dimensions so far.

Next align axes. Choose Align under Constraint Type, then pick axis A1 on the lid and then axis A1 on the mug. Now the lid moves over top the mug.

The prompt line now reads:

The component can now be placed.

This indicates that the two parts are fully constrained. The axis alignment constrained movement in the other two dimensions. Even though the lid is constrained enough for placement, we also want to control the rotation about axis A_1 by constraining its rotation. We will orient the lid so that the sipper hole is located appropriately for a right-handed drinker.

Choose Align again as the constraint type.

Now choose DTM3 on the lid. A window will pop up asking whether you want the yellow or red side of the datum to be the 'chosen side' (the direction the arrow will point). Choose the yellow side of the datum.

Then choose DTM1 on the mug. Pick the direction so that both arrows point the same direction when the sipper hole is in the orientation seen in Figure 9.

NOTE: If you pick the wrong side of the datum for alignment, you can reselect the Assembly Reference in the Component Placement dialogue. 

Pick done on the Component Placement dialogue.

The final assembly should look like Figure 9.

Figure 9.

Printing can be accomplished in a similar manner to printing parts.
 


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