What are the sheet metal operations

Self-study materials: sheet metal modeling with ProE


1 Self-Study Documents: Sheet Metal Modeling with ProE These instructions are intended to provide a quick introduction to sheet metal modeling with ProE and cannot explain all functions due to the diverse possibilities of the sheet metal module. However, these can be acquired individually after this introduction. A case cover that can be found in many PC cases is used as an example. Further modeling options are then explained. Table of contents Introduction to sheet metal modeling: Example housing cover ... 2 Drawing up: Creating developments: Flattening of beads: Deriving drawings: Other useful sheet metal operations: Inclined bending lines: Reliefs: GSO-FH, CAD Labor, Christian Daut

2 Introduction to sheet metal modeling: Example housing cover GSO-FH, CAD laboratory, Christian Daut

3 We first create a sheet metal starting model. To create a sheet metal model, you have to select the sheet metal subtype when creating a new part. The first model is named Housing Cover. When using the student version, an error message appears first. This can be easily confirmed: After the error message, you may have to select the desired start model, if this is not set in the default setting in the config.pro file, the template mmns_part_sheetmetal is selected. This contains the information about the units used, etc. Under Edit Settings Sheet Metal, these default settings can be checked and, if necessary, adjusted. After the selection you can confirm with OK. GSO-FH, CAD laboratory, Christian Daut

4 You can now see the usual start model with the three levels. So-called tabs are used in sheet metal modeling. The first tab is called the primary tab. For the housing we need a square primary bracket with an edge length of 400mm. First we choose the Flat tool: create a free flat flap. The further procedure corresponds to the usual generation of a volume model. We select the TOP plane as the sketch plane, and then sketch a square with a side length of 300mm in sketch mode. After exiting the sketching mode, we select the sheet thickness 1.00 mm and confirm. The first tab has now been created. All other tabs are now attached to this tab. Before we continue, the 3D model must be rotated with the key combination CTRL + D. GSO-FH, CAD laboratory, Christian Daut

5 We put the next flap at the point marked in the picture. After creating the first tab, all buttons are now active in the selection menu. To create an angled tab, we select the option: create. Flat: flat flap First, one edge of the primary flap must be selected. We take the upper edge for this and click on it. In the control menu we select the Form tab and then click on Sketch: GSO-FH, CAD Labor, Christian Daut

6 In the sketch mode you can first see the two corner points of the primary flange. The shape of the tab can now be sketched as usual or a predefined sketch can be parameterized: Important: The edge around which it is to be bent must not be drawn. The cut must be open. After exiting the sketch, you can now see a preview of the tab. If necessary, the angle and the bending radius can be changed. However, we keep the suggested values ​​of 90 bending angle and inner radius 1mm and end the bracket. Now we want to drill two more holes so that the cover can be screwed onto the housing later: We use the extrusion tool for this. We use the tab we just created as the sketching surface: The TOP and FRONT levels serve as sketching references. The distance to the front level is 100mm Ø5mm distance to the top 5mm. The hole can be mirrored directly in the Sketcher on the front plane or a center line lying on it. GSO-FH, CAD laboratory, Christian Daut

7 The sketch maker can then be ended and the creation of the hole can be completed after specifying a reasonable depth (to selected). Since ProE is set to Remove material in sheet metal mode, no further settings need to be changed. The next step is to prepare the remaining flaps. In the next step we process the opposite edge. This is first cut at the corners. This is done again with the extrusion tool: The corners are processed as follows: 45⁰20mm depth to the bottom. If you are working with an open section, this cannot be mirrored in Sketcher mode but only as a finished construction element. The sheet should now look like this. GSO-FH, CAD laboratory, Christian Daut

8 Now we want to punch another guide plate. To do this, we first have to create a so-called deep-drawing mold. So we create a new volume model (not a sheet metal model!) With the designation deep-drawn mold and create a base body with the dimensions 60x20x5: A negative of the later shape is now created on this base body: First, another rectangular body (20 mm x 8 mm) is created applied to the base body. It should have a height of 2.5 mm. GSO-FH, CAD laboratory, Christian Daut

9 Then two long edges are rounded (radius 1.00): The shape is now finished. The model can now be saved and closed. We now switch back to the sheet metal model: With the Create bead option, we can now create the guide: We then select the Deep-drawing form option in the selection menu. Another window will now open. Here we select the shape we just created. GSO-FH, CAD laboratory, Christian Daut

10 The rest of the process is similar to installing a part in an assembly. The first condition defines the boundary surface. Here the area of ​​the stamp base should be placed on the inside (to which the fold is also directed) of the primary flap. (Tip: select the glasses. This makes installation easier) The other conditions should now be selected so that the stamp is aligned as shown on the left. GSO-FH, CAD laboratory, Christian Daut

11 The next step is to select the boundary surface. This is the marked area of ​​the main body, the stamp base. The core area, on the other hand, is the top of the actual shape. GSO-FH, CAD laboratory, Christian Daut

12 Now we have to exclude areas. This option causes the sheet metal to be cut off at this point. The three marked areas are selected and confirmed as areas to be excluded. With the preview option you can check again whether everything fits. When you confirm, the shape is created. The deep-drawing tool is also suitable for stamping. For this, however, one does not choose any areas to be excluded. Then no cuts are made, but the sheet metal is deformed. GSO-FH, CAD laboratory, Christian Daut

13 The next step is to bend the sheet metal. This is done with the bend tool. Done Inner radius is selected as the radius type. The sketch area for the bending line is now defined. This is placed on the primary tab. The following queries can all be confirmed until the sketch mode is reached. The corner points of the previously created sections were chosen as references. The red line represents the sketched bending line. GSO-FH, CAD Labor, Christian Daut

14 After sketching the bending line, the bending side must still be defined. This should point inwards. This determines which side will be bent. If you have chosen the wrong direction, this can be corrected at any time. Discharge elected. In the next menu the option none will be selected as bending angle 180 and as bending radius 0.1 mm. Then use the Preview option to check whether the bending angle is correct. If it points in the wrong direction, you can define it again and switch the direction. Now another guide rail is to be created. For this we use one of the two previously unprocessed edges. We are now using the Flange Tab Tool. First, an edge is again selected for placement. We use the inner edge again. In the Profile tab, we select Sketch and sketch a plate cross-section as follows: GSO-FH, CAD Labor, Christian Daut

15 Radius 2.0 mm and 0.5 mm distance 10 mm, possibly delete sketch elements specified by the system. Now confirm and the flange bracket is ready. By adding the flange bracket, an overhang is now visible. This should be removed with the help of the lengthen tab. GSO-FH, CAD laboratory, Christian Daut

16 We take the inner edge again as the edge. As the extension distance we select value input and then input. The value should be 3 mm. After setting, you can complete the generation. The construction of the housing part is now complete. GSO-FH, CAD laboratory, Christian Daut

17 Drawing up: Creating developments: For the drawing we still need the development of the sheet metal part. This can easily be done automatically by ProE: Edit Setup GSO-FH, CAD Labor, Christian Daut

18 Now select the following in the menu manager: Create sheet unwinding condition Now the unwinding name is assigned. For the sake of clarity, we choose the following designation: Now we select the option Shaped. The following is selected: Fixed Geom Define sheet metal part Select and confirm GSO-FH, CAD Labor, Christian Daut

19 Now you can open the development as follows: Setup sheet metal Unwinding State Show Select the development Flattening of beads: When the development is created, beads and embossings are not developed. This can be done easily by hand: (Note: The following steps are carried out in the development) To do this, select the tool Create bead flattening. In the following menu, choose Define Bead. Now you select the area of ​​the bead: GSO-FH, CAD Labor, Christian Daut

Derive 20 drawings: Now the creation of drawings can begin. For this we choose a DIN A3 drawing template. You should be asked which part should be loaded. Here we first choose the generic part. We set the scale to 0.5. The now visible sheet metal model is reduced to a scale of 0.25 and moved to a drawing corner. It's just for the sake of clarity. GSO-FH, CAD laboratory, Christian Daut

21 The development is now inserted. For this we first have to load the development as a model: Right mouse button on the free drawing area The following window opens. Here you select: Drawing models Add model Drawing models Add model Select the development Done! Now you can insert a basic view and select the development as part of it. The views can now be aligned as follows. GSO-FH, CAD laboratory, Christian Daut

22 Bending Line Bending Angle To show the bending angles and bending lines, you can select the Show Notes and Axes option in the Show / Remove Tool. GSO-FH, CAD laboratory, Christian Daut

23 Other useful sheet metal operations: The same model (200 mm x 150 mm) is always selected for the following operations. Therefore, a new sheet metal model with the designation test model is first created: Inclined bending lines: To create inclined bends, you need the bending tool again. ==> Parts bending table inside radius Now you select the sketching plane for the bending line (note: choose sensible) the following messages can be confirmed until the sketcher is activated. GSO-FH, CAD laboratory, Christian Daut

24 The following line is sketched as a bending line: After sketching, confirm with the tick. The following two queries determine which section will be bent. If you have chosen the wrong side here, you can define it again. In the case of relief, it should be set without relief. What this means will be explained later. The following query specifies the bending angle. We choose an angle of 60. (Note: any angle can be entered using the Enter Value button) Thickness is also selected as the bending radius. Finished! GSO-FH, CAD laboratory, Christian Daut

25 If you choose the roll option instead of the angle at the beginning and set the radius to 100, you get such a result: Relief cuts: Relief cuts are often necessary to avoid undesirable deformations during bending operations: For this we use the test model again: We want a tab can be generated, which has a distance of 30mm from both sides. (Note: The sketch is on the next page) GSO-FH, CAD Labor, Christian Daut

26 After sketching, you can set the shape of the relief under the item Relief. Rectangular is selected first. The result then looks like this: If you select the Round-Oblong option, you get such a relief: GSO-FH, CAD Labor, Christian Daut