PTC Creo 3.0Posted by Ing. Vladimir Palffy Mon, February 27, 2017 10:02PM When you create a cut in Sheetmetal mode, you can create a solid cut or a sheet metal cut. In this video tutorial you can learn more about Sheetmetal cuts:
A solid cut is created the exact same way and with the same options as in Part mode.
A sheet metal cut can be created as Thin or Solid. A sheet metal cut can only be extruded. You can use a Blind, Through Next, or Through All as depth.
One difference between the solid and the sheet metal cut is that the solid cut is extruded through the material in a direction normal to the sketch plane. In the sheet metal cut is first projected onto the surface (green or white) selected as the driving or offset surface, and extruded normal to that surface.
If the cut is a sheet metal extruded cut with the selected "Driving surface": the cut is projected onto the green surface and extruded normal to the green surface.
If the cut is a sheet metal extruded cut with the selected "Offset surface": the cut is projected onto the white surface and extruded normal to the white surface.
Depending on the types of parts that you design, you may have to create additional features (Rip, Corner Relief, Conversion features, etc.) in order to unbend a model.
Most sheet metal parts are created with open edges; however, some parts will have closed profiles. These closed profile parts cannot be flattened without the use of a rip feature.
When creating a rip feature, Creo Parametric creates a tear in the sheet metal geometry, similar to rip relief.
You can create four types of rips:Edge Rip, Surface Rip, Sketched Rip and Rip Connect
The Edge Rip element creates rip geometry along an existing edge, similar to the rip feature. The edge is then converted from a sharp edge to two adjacent walls that meet at their inside surfaces.
By default, the edge rip is created using an Open corner type. You can change this to either a entered value or an Overlap.
If you create Surface rip, select a surface. The system creates a cut by removing an entire surface patch.
For a Sketched rip, you need to sketch a section to define the rip line.
The Rip Connect element is similar to the edge rip; however, instead of selecting an existing edge, you select two points or vertices between which to create the rip.
The Corner Relief creates relief at specific corners. Similar to the corner relief option when creating walls, selected vertices are highlighted with specific symbols that indicate the particular relief or conversion feature that has been applied.
One of the primary methods for manipulating sheet metal is bending.
You can create two types of bends:Angle and Roll.
Angle bends - bend the material adjacent to a sketched bend line through a specified radius and angle. The angle refers to the angle of the wall segment travels as it is bent. System automaticaly specify which portion of the wall to remain fixed during the bend operation and specify the side of the bend line the feature is created on. You can change the direction of the bend using the "Flip options".
Roll bends - bend the material adjacent to the sketched bend line through a specified radius. The included angle of the bend is defined by the amount of material available to bend.
In certain cases you will need to add bend relief when bending a part. The 'Relief option" creates bend relief at the endpoints of a bend feature. Select the desired relief option after you created the bend line (No Relief, Rip relief, StrtchRelief, RecRelief, and ObrndRelief).
The following Creo Sheetmetal tutorial describe common type of secondary wall option or How to create Flange Wall feature with Creo Parametric 3.0: Notes:
To create Flange Wall feature (secondary walls), select the appropriate button from the model tab.
A flange wall is created by sweeping a cross section along an attachment edge.
To create a flange wall feature you can sketch the profile or select from a pre-defined profiles. The pre-defined profiles can also be used as a starting point for sketching and you can customize it further by selecting the "Sketch..." button in the Shape panel.