Tutorial on Sheet Metal Design using PRO/Engineer

[Magneto]

Introduction

Sheet metal is a commonly used material for the design of engineering systems. In this tutorial, you will learn to design sheet metal parts containing multiple walls, bends, cuts, and holes. You will also learn how to create a flat pattern of the part.

(1) Start Pro/E Wildfire.
(2) Select [File] -> [New], and type the part name [Example9] in Text Box.
(3) Make sure [Part] is selected from the Type menu, and select [Sheetmetal] from the Sub-type menu. Click [OK] Button.
(4) Select the Create Unattached Extruded Wall icon from the tool bar at the right of the screen, as shown in Figure.

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(5) Select [One Side] from the ATTRIBUTES menu of the menu manager. This will cause the part to be extruded in one direction only.
(6) Select the FRONT plane as the sketching plane.
(7) Flip the arrow if it is not facing away from you, and select [Okay] from the DIRECTION menu.
(8) Select [Default] from the SKET VIEW menu. Pro/E should now enter Sketcher mode.
(9) Draw the profile shown in Figure 9.2 and dimension it as shown. Notice that two of the radii have dimensions of 5 while two have dimensions of 10. This is because some represent inner corners of the part while the others represent outer corners. Also note that you are not drawing a closed profile, since the sheet metal is of constant thickness which you will define later.

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(10) Click the check mark or select [Done] to exit Sketcher mode.
(11) Make sure the arrow indicating the thickening direction is facing down, and select [Okay] from the DIRECTION menu.
(12) Enter [5] into the textbox on the dashboard to set the thickness of the sheet metal, and click the check button.
(13) Make sure SPROBOT.LK TO is set to [Blind] in the Menu Manager, and select [Done].
(14) Enter [120] into the textbox on the dashboard to set the extrusion depth, and click the check button.
(15) All of the properties of the part should be shown in the window that reads FIRST WALL: Extrude as shown in Figure If you need to change any properties later, you will use this window. Select the Okay button in this window. You should see the part shown in Figure.

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Creating Additional Walls

(1) Select the Create Flat Wall No Radius icon from the tool bar at the right of the screen, as shown in Figure.

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(2) Select [Part Bend Tbl] from the menu manager, and then select [Done/Return].
(3) Select the white edge shown in Figure 9.6 as the reference for the new wall.
(4) Make sure the arrow is facing down, and select [Okay] from the menu manager.

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(5) Draw the profile of the new wall as shown in Figure 9.10 and dimension it as shown.

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(6) Click the check mark or select [Done] to exit Sketcher mode.
(7) Select [Okay] from the WALL Options menu. You should see the wall as shown in Figure.

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(8) You will now add a datum point to help define the next wall. Select the Datum Point icon from the tool bar at the right of the screen, as shown in Figure 9.9.
(9) Select the top right corner of the newly added wall, as shown in the figure, to define the datum point. Select [Okay] from the Datum Point window

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(10) Select the Create Extruded Wall No Radius icon from the tool bar at the right of the screen, as shown in Figure

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(11) Select [Part Bend Tbl] and then [Done/Return] from the menu manager. Select [One Side] and then [Done].
(12) Select the top edge of the newly created wall as the reference edge for the new wall, as shown in Figure

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(13) Select [By Point] from the SETUP SK PLANE menu, and click on the datum point that you created in step 9. A new datum plane will be automatically created.
(14) Make sure the arrow is facing to the left, along the path of the edge you selected as a reference, and select [Okay] from the DIRECTION menu.
(15) Draw the profile shown in Figure. You will need to add a line along the edge of the previously created wall as shown in the figure in order to create the necessary radius.

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(16) Delete the extra line you drew in the previous step, and click the check mark or select [Done].
(17) Select [Okay] from the WALL Options window. You should see the wall shown in Figure.

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Adding Holes and Cuts

(1) Holes can be added to sheet metal parts in basically the same way as they are added in solid parts. Select [Insert] -> [Hole] from the menu bar at the top of the screen.
(2) Select the top surface of one of the side flanges, shown in pink in Figure 9.14, as a reference for the hole.
(3) Drag the reference handles and adjust their values so that the hole is 20 from the side wall and 35 from the edge.
(4) Set the radius of the hole to be 15, and cut the hole through the part.

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(5) Repeat this process to create another hole 35 inches from the other side of the same flange. You should see two holes as shown in Figure .

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(6) Use the menu manager operations to mirror these two holes about the datum plane in the center of the part to create two holes on the opposite flange.
(7) You will now create a cut in the part. You will start by unbending the part, since the cut will be through several walls. Select the Create Unbend icon from the tool bar at the right of the screen, as shown in Figure.
(8) Select [Regular] from the Unbend Options menu, and then select [Done].
(9) Select the surface labeled A in Figure 9.16 as the plane to remain fixed.
(10) Select [Unbend Select] and then [Done] from the menu manager.
(11) Select Edge 1, hold down the control key, and select Edge 2 as the edges to unbend.

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(12) Select [Done Refs] from the menu manager, and select the Okay icon from the Regular Type window. The part should now be unbent at Edge 1 and Edge 2.
(13) Select [Insert] -> [Extrude] from the menu bar at the top of the screen.
(14) Select the Sketcher icon on the dashboard, and select the surface labeled as A in Figure as the reference plane.
(15) Select the Sketch icon from the Section menu.
(16) Sketch the profile shown in Figure , and click the check mark or select [Done] to exit Sketcher mode.

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(17) Select the Thru All option to cut through the part, and click the check mark. You should see the part shown in Figure.

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(18) Select the Create Bend Back icon from the tool bar at the right of the screen, as shown in Figure.

(19) Select the original part (labeled FIRST WALL in the model tree) as the part to unbend.

(20) Select the surface labeled A in Figure as the plane to remain fixed.

(21) Select [BendBack All] and then [Done] from the menu manager. Select the Okay icon from the Bend Back window. You should see the part as shown in Figure.

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(22) To create a flat pattern of the part which can be used to cut the sheet metal to the correct size, select the Create Flat Pattern icon from the tool bar at the right of the screen and click somewhere on the part. You should see the part as shown in Figure.

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(23) Select [File] -> [Save] from menu bar to save the part.