This guide is written for SOLIDWORKS 2015 Sheet Metal. If you are using an earlier version of SOLIDWORKS Sheet Metal, please download our earlier installation documents to correctly load and administer your version of SOLIDWORKS Sheet Metal.
This is not a troubleshooting guide. If you have any technical issues with SolidWorks, please contact Hawk Ridge Systems technical support.
This document is only to be distributed and used by Hawk Ridge Systems customers. Any other use is prohibited.
©2015 Hawk Ridge Systems
The sheet metal package is included in the base package of SOLIDWORKS. The power of this tool comes from its ability to quickly and accurately create flat or bent versions of a pressed or rolled sheet metal part. The goal of the sheet metal feature is to create a flat pattern that accurately represents the required dimensions and bend lines by accounting for the stretch, or bend allowance that occurs during manufacturing.
There are a few ways to create a sheet metal part within SOLIDWORKS:
- INITIAL BASE FLANGE- Using the sheet metal tool bar, parts can be developed as thin bent mental from their inception using the “Base Flange” tool,
- THICK SOLID- Create a ‘thick’ solid, and then convert it to sheet metal using the “Convert to Sheet Metal” tool.
- THIN SOLID- Parts can be developed, or imported, as ‘thin’ solids that have a constant thickness then converted to sheet metal parts using the Insert Bends tool.
- SURFACE MODEL- Create a surface model representing either the inside or outside surfaces of the model, then use the “Convert to Sheet Metal” tool to create the sheet metal model.
- LOFTED BEND- Create a complex sheet metal part using the “Lofted Bend” tool.
Parts can be initially created flat (or unfolded) using the construction method A mentioned above, with bend lines added later to accurately fold the part using the “Sketched Bend “ tool.
All methods of part creation will give the same result: a bent part with a suppressed flat pattern feature with true material length and bend lines. The particulars of part construction will be covered in the step-by-step examples later in this document.
With all methods of sheet metal development there is one common theme, the sheet metal feature. This isn’t a physical feature (i.e. it doesn’t create or edit geometry by itself) as much as it is a place SOLIDWORKS stores all the important data required for the creation of the folded and flat pattern part.
The fixed face is only asked for when inserting bends on to a solid part. The bend radius will be the default inside radius for all bends within the part. SOLIDWORKS does allow the user to manipulate the radii of individual bends. All sheet metal parts within SOLIDWORKS must have a uniform material thickness. When creating the part as sheet metal from the beginning, this value is entered during the creation of the first flange feature. When inserting bends on a solid, the part thickness is determined by part geometry.
When creating sheet metal geometry for SOLIDWORKS, the main rule is that complex surfaces created by forming or rolling will generally not unfold (see exceptions in the following sections). SOLIDWORKS mostly works under the assumption that all parts are created via a brake press.
When looking at parts using a brake press, the cross section profile will consist of a uniform thickness which contains flat and bend sections. If the part is manufactured by modifying the thickness, such as stamping, then the part may not flatten correctly.
Looking at the inside of outside of the model, the profile must not include any splines, and there must not be any complex surfaces. A complex surface will be defined as a surface with variable curvature, or a spherical surface. The exception here is when dealing with lofted bends which will be looked into later.
The example below shows a standard sheet metal part. Looking at the curvature (View menu > Display > Curvature), we can see there is a constant curvature for the bend faces, and for the flat faces.
Take a simple and common example below which generally fails to unfold. We have a part with excessive fillets. The bend faces contain non spherical constant curvature faces. However, the section where all the three fillets meet turns into a constant curvature spherical surface which will not be able to unfold without some manipulation.
Again, the part below shows a complex surface with a non-constant curvature which will fail to process as a sheet metal part. Using the curvature display again, the cursor’s location will display the curvature and radius of curvature (1/curvature).
Lofted Bends are not limited to the complex surface restriction.
One of the most common issues when dealing with the sheet metal parts is the excessive fillets. The cause for failure here is due to the spherical section where the three filets meet, as well as the actual number of fillets. This part should be made with two bends, not three. A quick and easy question is “Can this part actually be made using a standard tools?” (not including stamping methods)
Method 1: Remove the excessive filleted section.
- By using a cut-extrude, the excessive filleted section can be removed.
- Insert Bends or Convert to Sheet Metal to create a sheet metal part.
Method 2: Modify the excessive filleted section.
Modify the excessive filleted section. This method is much like method 1. Rather than removing the entire corner, we can remove just the spherical section.
- By using a cut-extrude, the excessive filleted corner can be removed.
- Use the Delete face feature to remove the excessive bend. (“delete and patch” for this example)
- Rip the corner to separate the two flanges.
- Use the Insert Bends or Convert to Sheet Metal feature to complete.
Method 3: Convert to sheet metal tool; ignore the corner section.
If using the Convert To Sheet Metal tool, the spherical section can be ignored automatically. The closed corner feature may be used to reduce the gap between the two flanges afterwards if desired.
Creating a flat pattern for a complex surface cannot be done in SOLIDWORKS unless the surface can be created using a lofted bend. However, if that is not possible, there is another possible workaround.
Again, lofted bend sheet metal parts do not conform to this restriction.
The flat pattern will be approximated. To approximate:
- Create a section which mimics the first curve of the part.
- Create a section which mimics the second curve of the part.
- Create the flat pattern of a linear approximation of one of the profiles.
- Unfold, and measure the unfold length then adjust unfolded flat width to accommodate the change.
Exceptions to double curved profiles
Other than lofted bends, edge flanges have the ability to follow a curved surface, however flanges cannot be created from these flanges.
Forming tools can be placed on parts via the design library. The flat patterns which are created using these design library parts will contain formed parts in their formed state, not their flat state. The flattened state of these formed shapes should follow the specifications for the tool(s) being used to create the forms.
Formed parts created using special forming tools, or in a stamp press can only be approximated in SOLIDWORKS if using the standard SOLIDWORKS tools. To flatten such a model, a third party solution such as BLANKWORKS would need to be used.
Below we can see a simple example of a formed part which can be approximated using standard features.
- Break the formed section into sections which can be unfolded using standard SOLIDWORKS tools. In this example, we can use miter flanges to replicate the formed sections.
- Remove sections which will cause overlap when unfolding the part. The sections can be removed using any method. A cut extrude in this case would works just fine.
- Flatten the part.
- Add in the removed sections using the extruded-boss features.
Helical shapes can be made a variety of ways. The factor determining which method to use depends on how the part will be made. Below are a variety of helical shapes which create a variety of flat patterns.
Method 1: Remove the excessive filleted section
- Create a cylindrical sheet metal part.
- Use the Unfold tool to unfold the part.
- Cut into a diagonal strip.
- Use the Fold tool to fold the form again to obtain the final formed part.
Method 2: Sketched Bend Technique
- Create a flat strip of sheet metal, and insert a sketch to be used for a sketched bend.
- Create the sketched bend with a 180 degree bend angle.
- Create as many sketched bends as needed moving through the strip to create the helix.
Method 3: Extrude and Flex
- Create an extruded flat section. The model does not need to be a sheet metal part.
- Use the flex feature to twist the sheet metal part. This will create a helical form; however will not create a flat pattern.
Method 4: Lofted Bend
- Create two helixes which represent the inner edges of the helical sheet part, and covert each helix into its own 3D sketch.
- Create a lofted bend using the two helixes as the profiles. Set the thickness as the width of the helix.
- The flat pattern is a flat strip.
Method 5: Helix From Disc
- Create two helixes representing the bottom edges of the helix, and convert each helix into its own 3D sketch.
- Create a lofted bend using the two profiles. The thickness in this case is the thicken of the sheet metal part.
- The flat pattern is then a 2D disc.
Sheet metal parts created using splines as a cross section profile cannot be used to create a sheet metal part. The spline profiles will need to be converted into sections of arcs and lines. The only exception to this is rule is that splines can be used for lofted bends.