Sheet Metal Part Design in PTC Pro/ENGINEER

To start creating sheet metal layout, go to the right hand side toolbar and click on the sketch button. This will open a menu similar to the image shown here. Select the plane in which you switch to use to sketch in. For simplicity, we will be using the front plane. Select the front plane and click okay. This will now reorientate your screen to have the front plane facing you, ready to sketch the design.

Ensure that you have your design in the right shape and form, use the centreline tool located in the line tool button. Click the centreline tool to orientate on top of the axis in the front plane. This will help when apply constrains to the model later in this tutorial. To start sketching, simply use the toolbar to the right to access any of the drawing tools. Once the rough drawing of the sketch has been made, the design can now give it specific dimensions as well as constraints. To show the dimensions of the sketch, click the Normal (dimensions tool) button on the right hand side and the workspace should showup with grey dimension lines on your sketch. When completed click okay and double click on a dimension to edit the dimension. Now click the “constrain” button to add constrains to the model as required.

Once the sketch is completed, click the tick box on the middle of the right hard toolbar to complete the sketch and switch back to the sheet metal workspace. Now to create the base of the sheet metal design in which the sketch will be based off, select the flat (create unattached wall) button and a preview of the sheet metal will appear in the workspace. On the top under the main toolbars, the opinions for the sheet metal thickness as well as the name of the feature can be changed here (this is known as the flat wall Dashboard). Once completed, click the green tick icon to confirm the changes which is located on the far top right of the workspace window.

This is the base of which the rest of sheet metal design will come from. The additional features which can be added such as walls, flanges, S bends, holes, punching, pressing and etc will be attached to this main piece. Note also the information in which can be tracked on the Design Tree with each additional part can be rolled back and copied form here. Editing of a particular part can be done by right clicking the mouse on the part and selecting edit definition. This will bring up the window in which you initially designed the add-on feature to the design allow you to change the necessary parameters to meet the specification required.

There are multiple functions which can be added to the sheet metal designs in wildfire4.0. Creating attached flat or flange walls with reliefs ranging from Point, corner reliefs to edge rips and bends. To attach a new wall to the sheet metal design, select either create flat wall or create flange wall and the dashboard for either one of the two opinions will appear. There are various opinions in which are available to customise and edit the attachment of the wall. The placement tab will highlight red if the wall creation was selected without highlighting an edge to attach it to. The shape tab allows for the creation of custom walls with specific features that might be needed that is accessed by the sketch button. Also the Shape tab allows for the user to define the height of the wall as well to define offsets from the attachment edge of the wall.

Note: It is important to note that different profiles are available for the user to use in their creation of the flat wall. Theses are Rectangle, Trapezoid, L, T and user defined. Flange wall creation has similar feature where there are list of profiles available for the user to decide on.  These are found above the placement and shape tabs.

Demonstration 1:

Now through out this tutorial, there will be a design model which will be designed in Pro Engineer wildfire 4.0. This is done to demonstrate on how each part can be done with a few tricks and tips along the way. Also through this tutorial, there will be features and options that will be discuss to explain why such functions need to be applied in a certain order. Now, to start up, we will be looking at this design here:

As shown here, we can see that there are two symmetrical lines which are used in this sketch which run along the x and y axis. These are known as centrelines which can be selected during sketch mode and found in the line toolbar. The centrelines are important in sketches as they will allow for careful manipulation of the distance as well as the symmetry of the model part. This will become important later on during the assembly as each part will be constraint based on the planes created. Also note that dimensions are added in and then constrained based on equal lengths as shown by the Letter with subscripted numbers.  Notice how there is an additional dimension to the x-axis centreline to the highlighted line of 18.75inchs of L1, this is another benefit of using the centreline since you can create an offset for the design which you can adjust without altering the entire design.

Points to take:

1. Ensure with any sheetmetal design of parts in ProE to use the centreline function to provide additional constrains, to make sure that the design stays symmetrical through the design process and assembly and provide easy adjustments for offsetting of parts.

2. Use the constraints in sketch mode and they are represented by the appropriate Letters with Subscripted numbers. Make good use of this.

Now that we are completed with the design, click confirm and create an unattached wall. Add the design thickness required in as well as a suitable name. Click confirm and we have a starting platform for the additional features required for this part. Now we will attach a small 5.0 inch wall. Proceed through the steps and confirm after the required parameters have been met. Next we will copy this feature from the Design Tree, by simply using the keyboard shortcuts [Ctrl+X] and paste it accordingly to the necessary edges as you can see in the series of pictures below. This is a very powerful and efficient way of duplicating features on a specific model without having to repeat the required step to attach it from the toolbar. Once completed, there are two additional tabs which need to be added on one of the larger lengths on the sheetmetal design. By repeating the steps with the attaching walls, but this time creating a offset on either side will allow us to create the tabs required. Once completed, Save the design and flatten the design with the flatten pattern button. This is an important step in which needs to be done to be able to use the nesting function later. Save the file under a different name as well since that in assembly, the designs will be assembled in their flattened forms. Here is a small overview on the designing process:

Figure 1.1 - Designing Stages form left to right- 1) Creating the unattached flat wall 2) Creating the 4 flat walls using Cut and paste function from design tree 3) repeated once again on the far outer edges. 4) Creating the necessary tabs for anchoring. 5) completing the design, save, flatten and save under a different name for nesting.

Die Press, "Stamping" Form Features in NC Sheetmetal:

Although this particular design demostration does not use any die features, it is still relevant to mention how these would be defined in Pro/ENGINEER NC Sheetmetal. Note Pro/ENGINEER offers both die-stamp and punch-tool form feature definitions (one does not require the other). Here is a brief overview of die-stamping in Pro/E NC Sheetmetal..

Start by creating a die cast in wildfire 4.0. Now the only requirements for the die-cast is that it is a extruded design with the design pattern on a single surface. Once you have created that save the die with appropriate name. Next open up the sheetmetal design that you want to create the feature with the die imprint on. Select the press form button and select create from die, reference and then done.A window will ask you to select the die .prt and click okay. Two new windows should open with preview window of the die cast as well as form dialogue box asking you to setup the constrains similar to the one shown here:

Now you will need to apply three constrains for the die to be full constrained to the sheetmetal design. Now in this example, we have used the mating constrain with the two surfaces in which the die is going to be pressed to the sheetmetal design. The other two constrains we have aligned the datum planes of the top and front planes of the respective parts.Once completed, click okay and select the seeding surface and the bounding surface on the die to imprint on to the sheetmetal design.

Figure 1.2 - The area required for the pressing feature in ProE. Left) The bounding surface. Middle) The Seeding surface. Right) The Excluding surface.

At this point you can preview the design on what it looks like by selecting the preview button. Now to make the necessary cuts in certain die-casts, you will need to select the exclude surface opinion. To do this click in the dialogue box - exclude surface and select define. Now in the Die cast.prt, select the areas in which you want to exclude from the feature for the sheetmetal design. Note to hold down [Crtl] to select multiple surfaces. Once completed click done and your Feature should look similar to one of the two features here. The one left is the feature without the exclude surface and the one on the right is with the exclude surfaces. Here is an image of what including and excluding the surface option will looking like in a design:

Figure 1.3 - Two representations of the including and excluding feature option in die pressing in ProE. 1) Resulting Image of including feature option for the press design. 2) Resulting Image of the excluding feature option for the press design.

Note: Pro/ENGINEER NC Sheetmetal die press feature only requires the "die side" to create the press feature.  To calculate deflection from the die press, you will require PTC Pro/MECHANICA option.