Pro/ENGINEER Tutorial - Sheet Metal

In this tutorial, we are going to build a sheet metal part using Pro/E's Sheet Metal module. The final result can be seen in Figure 12.
Go to application>sheet metal and create a new sheet metal part, clip, just as you would any other part.
Now create a set of default datums to help guide the creation of further features.
The first geometry created has to be a wall. This wall can either be a flat pattern, or an extrusion of a thin profile. You will do the latter:
feature>create>sheet metal>wall>extruded | done>one side
Pick DTM3 as the sketch plane and a top orientation for DTM2.
Because it is a thin feature, you will only define one side of the sheet metal that will eventually be thickened to the specified thickness of the metal. The thickened profile will then be swept from the sketch plane much like a traditional extruded protrusion. All thickened sheet metal features have two distinct sides: green and white. When you sketch a thin feature, you sketch the green side which is then thickened to form the white side. Sketch the green side as seen in Figure 1a. Note that the sketched thin profile won't show up as green until after the feature operation is finished. During sketching, the edge is blue, just as it is in other profile sketches.
Note: because the radii are so small relative to the overall size of the sketch, you may want to sketch square corners and then use sketch>arc>fillet to create the tangent arcs.

Figure 1a.
Notice that some of the radii have differing sizes. That is because two of the radii are inside radii (R1), while the other two are outside radii (R4). The difference in the radii is defined by the thickness of the material we are using, 3.
As with other profiles, click done when finished with the profile sketch.
Make sure the red arrow is pointing up, the direction of extrusion.
The thickness of the material is 3.
The blind extrusion distance is 40.
The result of the first extrusion will look like Figure 1b.

Figure 1b.
Next, add a flat extension to the initial extrusion:
wall>flat | no radius

Note: Unless noted otherwise, all of the features being created are sheet metal features.

The flat option will let you draw the outline of a single flat surface and the no radius means the feature will not attempt to automatically put in a radius bend between your new feature and the existing part. It is worth noting that the bends shown in the model are ideal bends and, in fact, there is distortion in the metal when the bends are made. These distortions have to be accounted for in the initial flattened metal pattern. The amount of material that has to be added to the flat pattern for each bend is controlled by a number of parameters, including: type of metal, radius of the bend, and thickness of the material. You will use a generic part bend table to calculate this factor.
Select part bend table for the source of bend data.
Now select the green edge marked in Figure 1b as the attachment edge. Notice a datum is created 'on the fly' to draw your sketch on.
The red arrow indicating direction of extrusion should be pointing up.
Draw the profile as a three-sided, open loop. Make sure to align the profile to the attachment edge.
The profile should look like Figure 2a.

Figure 2a.
The resulting feature should look like Figure 2b.

Figure 2b.
The next feature will be an extrusion like the base feature. The difference is that it will attach to an existing edge and only extend part way along the edge. Because the extrusion only extends along part of an edge, a datum point is needed to define a starting point along the attachment edge. Place a datum point, PNT0, as seen in Figure 3b, using:
create>datum>point>on vertex
Now create the partial wall:
wall>extrude | no radius | done
Again, the no radius option is used because you will draw in the radius rather than letting the system create it for you. Your sketch will define a thin feature and outline the green side of the profile. In this case, it will be the inside edge of the wall.
part bend tbl | done
one side | done
Select the horizontal green edge closest to you as the attachment edge. This edge will share the vertex where you put the datum point.
Now you need to indicate where along the edge you want to start the extrusion. The sketch plane will be created normal (perpendicular) to the attachment edge at the point you pick.
Select by Point from the Setup Sk Pln menu.
Now select the datum point, (PNT0), you just created.
A new datum will be created on the fly which passes through this datum point and is normal to the attachment edge. Make sure the red arrow is pointing to the right.
Now sketch the thin profile. The radius you sketch has to be tangent to the existing surface. To help guarantee this, you should draw a straight line over top the existing edge and then draw a tangent arc. Now go back and erase the first straight line you drew and align the tangent arc to both the vertical and horizontal edges of the existing surface. finish the profile sketch. The sketch, when finished, will look likeFigure 3a.

Figure 3a.
Now, since we want to only go part way along the edge, you need to select Depth (an optional parameter) from the Wall Options dialogue box. Then click Define.
Blind | done
Extrude the wall 10. The resulting feature should look like Figure 3b.

Figure 3b.
Use the same process to create the feature seen in Figure 4. Again, you will have to start by creating a datum point on the other end of the edge. The wall will be extruded 40.

Note:To speed drawing the sketch, you can use geom tools>use edge to clone the edge profile used in the last extrusion. Note that you don't have to constrain edges created in this fashion because they inherit the constraints of the cloned edges.

Figure 4.
Repeat the process again to create a new wall on the end of the wall you just created. Add a datum point as seen in Figure 5. Now sketch the profile as seen in the figure.

Figure 5.
You have now added all of the material needed for the final part at this point. Now cutting and other material removal operations are used to shape the final part. First cut two holes in the part. These holes can be centered on a common datum axis. Create the axis, as seen in Figure 6.

Figure 6.
Now use the cut>extrude | solid feature operation twice to create the two holes in the part as seen in Figure 7. Just as you would with a typical solid part, you can select a surface on the part to define a sketch plane. Align the holes with the datum axis you just created. The diameter of the top hole is 8 and the bottom hole diameter is 12. Make sure to choose the thru next option since you are only going through one wall.

Figure 7.
The next operation is also a cut, but it spans two surfaces which are not coincident. First you will have to unbend one of the bends in the sheet metal.
create>sheet metal>unbend>regular
Next, you must choose a flat surface to stay fixed (see Figure 8).
Finally, choose a curved surface to unbend (see Figure 8).

Figure 8.
Now you can you use cut>extrude | solid to remove the excess material between the two tongues.
Select the top surface (the one marked 'fixed' in Figure 8) again, this time to use as the sketch plane.
See the profile sketch in Figure 9.

Figure 9.
Once the cut is made, you can bend the metal back:
bend back>(select the top surface to be fixed again)>bend back all | done
One more cut is needed to chamfer an edge. Use cut>extrude | solid to create the feature seen in Figure 10.

Figure 10.
Finally, radius the corners seen in Figure 11. The round feature is a solid, rather than sheet metal, feature. This is because sheet metal features only work on the primary surfaces, not the edge surfaces, of the sheet metal.
feature>solid>round

Figure 11.
When done, your part should now look like Figure 12.

Figure 12.
You can create a flattened pattern of the sheet metal part by creating a flattened instance of the part:
setup>sheet metal>flat state>create> (use the default name it gives you for the instance)>fully formed
The last option indicates that the part is currently completely bent. You are asked to name the instance. This instance is not unlike an instance created with a family table. It can be called up in the drawing module just as a part would be.
Pick the top surface again to be the fixed surface again.
The instance is now created showing your part in the flattened state. You don't see the instance, though.
Go to the drawing module and create a new drawing. Use the standard titleblock format you've used for other drawings.
Add a view and enter the name of the sheet metal part. Now you choose the flattened instance from the menu as the part to lay out. Orient and detail the flattened instance just as you would any part.
To add a pictorial view of the formed part, add a second model to your drawing:
views>dwg models>add model
Enter the name of the sheet metal part again, but this time pick generic from the menu.
This can be added in as a general view pictorial in the upper right corner. The result might look like Figure 13.