One of the special types of documents that can be created with SolidWorks 3D mechanical design software is a sheetmetal part. SolidWorks has special features and functions that are specifically geared to this type of design.
A sheet metal part starts as a flat sheet of metal and is cut and bent to form a part. While you may design the part in its finished, bent state, the part will start out as a flat piece of metal. A sheet of metal allows the designer to model the part and automatically produce a flat pattern that can be used to create the blank. The blank is then bent to create the final part.
The example shown in Figure 1 shows some of the different features that can be created with a sheet metal part. Figure 2 shows the sheet metal toolbar. This toolbar displays all the sheet-metal-specific functions.
Figure 1 – Example sheet metal part
Figure 2 – Sheet metal toolbar
There are two ways in which you can start a sheet metal part, Sheet-Metal2 is described in Method 1, and the newer Sheet-Metal1 is described in Method 2. Sheet-Metal1 can be easier and quicker to create. The Sheet-Metal2 method has additional rules (i.e., link to thickness) that need to be defined to create a valid sheet metal part.
Method 1 (Convert to Sheet Metal)
- Create the part using thin extrusion and cuts. These features should be linked to the same thickness.
- Make it a sheet metal part by using the Insert Bends feature.
- Create additional sheet metal features.
Figure 3 – Part defined as sheet metal after design of several features
Method 2 (Direct Sheet Metal)
- Create the sketch profile.
- Insert a Base-Flange feature.
- The base-flange feature is created, using Sketch1.
- Create additional sheet metal features.
Figure 4 – Base-Flange defines part as sheet metal from the start
Setting up the Part
When starting a sheet metal part, the following attributes should be defined:
- Thickness. A sheet metal part only has one thickness. This is defined in the Base-Flange feature (Sheet-Metal1) or defined in the features for Sheet-Metal2.
- Bend Allowance. The default radius used for all bends.
- Auto Relief type.
- Default Bend Radius. This can be changed if a bend uses a different radius. This is defined in the Base-Flange (Sheet-Metal1) feature.
There are different methods that can be used to calculate bend allowances (Bend Table, K-Factor, Bend Allowance, and Bend Deduction) within a sheet metal part. The method within the Sheet-Metal1 and Sheet-Metal2 features. This defines the default method for the part. This method can be changed on a bend-by-bend basis if so desired. When sheet metal is bent, the inside compresses and the outside stretches. The centerline between the inside and outside is referred to as the neutral axis. The neutral axis is R as shown in Figure 5. SolidWorks automatically calculates the flat pattern based upon the material thickness, bend angle, and bend allowance method.
Figure 5 – Bend length
To calculate the flat pattern for manufacturing purposes, the length of the bend needs to be calculated. The total bend length = A + B + C. To calculate C, a bend allowance needs to be determined. This is the value that needs to be added to the flat pattern to account for the bending process.
Sheet Metal Features
The following features are specific to sheet metal parts.
This feature will unfold the sheet metal part into the state used by manufacturing. The important aspects here are insuring the bend radius and bend allowances used are correct for the manufacturing process. The flat pattern feature is suppressed while the part is in the bent state. To see the part in the flat state, unsuppress the feature.
Adds a flange to a selected edge of the sheet metal part. The edge profile, angle, length, position, bend allowance, and relief types can be defined for each bend type.
Add a sheet metal hem to the part. The size, position, and type can be defined for this feature.
A jog creates two bends offset from one another.
Corner treatments can be used to add fillets or chamfers to a sheet metal part to break the sharp corners.
A miter flange is a different flange type due to the profile which must not be tangent to the sheetmetal edge. The flange may be complete or partial based on an offset from the start and end of the selected edge.
A sketched bend is a single line used to define an additional bend line.
Used to quickly suppress the sheet metal features in a Sheet-Metal2 part.
Fold and Unfold
A sheet metal part can be unfolded to create a cut that crosses bend lines. This is the only way to easily model the type of feature shown on the right. The feature is unbent, cut with the same true punch size, and then refolded.
Palette Forming Tools
The Feature Palette™ can be used to drag and drop common sheet metal forms (i.e., dimples, louvers, embosses, lances, ribs, and extruded flanges) into a design. Custom sheet-metal forming tools can also be added to the Feature Palette. The features can be sized and located by editing the feature or sketch.
A cross break is a sheet metal feature new in SolidWorks 2009. A cross break does not modify the geometry of the part and can be placed on any flat face of a sheet metal part.
To insure that all sheet metal parts are defined consistently, a template should be used and shared with others so that the setup is the same for all users.
Either method can be used to define a sheet metal part. It is a matter of preference. Sheet metal features help simplify the process of creating this type of part and make you more productive.
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