With Pro/ENGINEER Wildfire 3.0 comes the introduction of shaded drawing views. These drawing views are also available with sheetmetal design. In the following example, we will walk through the process of creating a simple sheetmetal drawing with both the finished manufactured part and its flat state instance. We will touch on creating flat patterns as well as bend order tables.
To begin, we will start with a sheetmetal part that has already been designed and then create its associated flat state instance.
This can be achieved by clicking Edit > Setup > Sheetmetal > Flat State > Create (Figure 1)
Accept or rename the flat state instance, and then select the unbend operation. From this point, all you need to do is select the surface to remain fixed during the unbend operation (Figure 2)
Finally, click OK to complete the feature. The flat state instance is now displayed in a new Pro/ENGINEER window (Figure 3)
Notice that the flat state instance and name are displayed in the Pro/ENGINEER graphics window. From this point, the flat state instance window can be closed.
You can check the instances for the generic part by clicking Tools > Family Table (Figure 4)
Having created the flat state instance, attention can now be focused on the manufacturing aspect of the part. In particular, we will take a look at creating the bend order sequence.
This is also achieved by clicking Edit > Setup from the main menu, followed by Sheetmetal > Bend Order > Show/Edit from the Menu Manager
Selecting the same fixed surface as before (when creating the flat state) returns the sheetmetal part to its flat state
Click Add Bend to begin creating the bend order sequence (Figure 5)
Select the first feature for the bend order sequence and click OK (Figure 6)
Click Next and select the fixed surface (the same surface used to create the flat state) (Figure 7)
After selecting the fixed surface, hold the CTRL key and select the remaining bend locations (Figure 8)
Click OK > Done to finish creating the bend order sequence. The part returns to its finished state (Figure 9
Clicking Info from the Bend Order menu displays the information for the bend order sequence (Figure 10)
Now that the flat state and bend order sequence have been created, it is time to create the sheetmetal drawing.
Click New from the main toolbar to create a new drawing (set type to Drawing)
Clear the Use default template check box and click OK. Make sure that the Default Model for the drawing is the correct sheetmetal part and click OK (Figure 11)
When prompted, select the generic instance for the model
Right-click to insert a general view and click in the upper right-hand corner of the drawing window to place the view
Select OK from the Drawing View dialogue box to complete view placement
Right-click and select Lock View Movement to enable repositioning of the drawing view. Reposition and rescale the view as necessary (Figure 12)
Now we can add the flat state instance to the drawing.
Select File > Properties from the main menu
Click Drawing Models > Add Model to add the flat state instance
Select the sheetmetal part and click Open
Select the flat state instance from the menu and click Open
The active model will switch from the generic to the flat state instance. Click Done/Return
Create a drawing view of the flat state instance in the same fashion as the shaded model
Right-click and select Insert General View
Click anywhere in the drawing window to place the view. Use the View Display dialogue box to adjust the view display settings
Once finished, click OK (Figure 13)
To finalize the drawing, we will add bend lines and the bend table.
Select the Show/Erase icon
Click Show and select the options for Notes and Axes to be displayed
Click Show All > Yes to display the notes in the view
Click Accept All (Figure 14)
Click Erase > View and select the shaded view to remove the bend information from that view
Select Close from the Show / Erase dialogue box to complete the drawing (Figure 15)
Notice the bend table in the upper left-hand corner. Also note the bend axes and angles in the left-hand view. That completes the drawing. So by using both new sheetmetal and drawing enhancements in Pro/ENGINEER Wildfire 3.0, you can create detailed drawings for sheetmetal parts with relevant manufacturing information and shaded 3D drawing views.
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