Additive manufacturing is ideal for making parts with complex geometries at low production runs. But when making simpler parts, or parts that need to be produced at higher numbers, there are better methods.
And ultimately, when manufacturing, the goal is to move as much material as possible, in a shorter time as possible.
Take for example, the common angle bracket, as seen below.
To print such a part with an FDM machine may take an hour. This is acceptable if you are only making prototype parts. But if you want to make thousands of these things, laser cutting a piece of sheet metal, then bending it in a press brake is going to be way faster, and ultimately, more cost-effective.
The combined time of cutting and bending a piece like this drops to mere seconds when using the right machine for the job.
Luckily, from a design perspective, we can use the same CAD tools for designing sheet metal parts as we can for 3D printing them.
In this article, we are going to take a look at how to create basic sheet metal parts in Solidworks, using the Sheet Metal tab.
Getting Started
To start, open a new Part document in Solidworks. The Sheet Metal tab is only accessible in Part mode. You can not create Sheet Metal parts in Assembly mode (but you can assemble multiple sheet metal parts there after they are formed).
Once the Part document is open, you may need to activate the dedicated Sheet Metal tab.
To activate the Sheet Metal tab, move your mouse cursor to the CommandManager area at the top of the screen.
Right-click the mouse anywhere in this area, and a drop-down menu will appear. From the menu, simply select Tabs > Sheet Metal.
If you have done this, then you will see the Sheet Metal tab appear, as in the image below.
Now we can start bending metal.
You will notice that many of the functions are greyed out in the Sheet Metal tab at the moment. This is totally fine, and these will become active as we begin to design our part.
Sheet Metal Forming
There are multiple methods for making sheet metal parts in Solidworks using the Sheet Metal tab.
In this article, we will look at using the Sketched Bend feature and also the Edge Flange feature. Both of these features are used to create bends starting from a flat piece of metal.
Making a Flange
To make a sheet metal part entirely using the Sheet Metal tab, we need to start with a flange.
We can use a closed sketch to make a flat flange, or we can use an open sketch to make the profile of a flange with the bends already formed.
We will use a closed sketch in this case, because we want to start with a flattened flange.
First up, click the Base Flange / Tab button in the command manager, then select the plane that you wish to sketch on.
Clicking on the plane will open up the Sketch mode, where we can sketch the shape of our flange.
Let’s sketch a rectangular base flange.
Starting with the origin at the centre, sketch a centre rectangle measuring 50 mm x 150 mm.
This is the closed sketch.
When you have finished sketching, click Exit Sketch, and the outline flange will appear in the graphics area, like in the image below.
The flange options will appear in the Property Manager in the left-hand pane, where we can select the thickness of the flange.
You can select the thickness from the gauge tables, or you can enter the thickness manually. We have selected a manual thickness of 1.984 mm, which is equivalent to 14 gauge for stainless steel. In the Property Manager, we can also select a Bend Allowance (k-factor), and Auto Relief.
We will look at the k-factor and relief functions in a later article.
When you have selected the thickness, click OK in the Property Manager tab, and the solid flange will appear in the graphics area.
You will notice that a new feature, named Base Flange will appear in the Design Tree in the left-hand pane, and you will notice that the previously greyed out features in the Sheet Metal tab are now active.
Bending Metal – Sketched Bends
Now that the base flange is complete, we can start to bend it, and perform other sheet metal functions on the part.
Click the top face of the part, and start a new sketch on that face.
Sketch a line right through the origin, so it divides the part into 2 equal areas.
Exit the sketch, then move the mouse cursor to the Sheet Metal tab, and press the Sketched Bend feature button.
This will open up the Property Manager panel on the left hand side, and we can either select a face to sketch new bend lines on, or we can select a pre-existing sketch which we can use to form our bend. We have drawn the sketch already, so we go with the second option to use the pre-existing sketch.
You can see the Sketched Bend Property Manager panel and the preview of the bend in the image below.
From this panel we can select the face from which the bend will be applied, the position of the bend, and the angle of the bend. We can also select the bend radius, and bend allowance here.
Click the green check mark (the OK button) to complete the function and create the bent part.
There! You have created your first bend on a sheet metal part.
Let’s try some different features on the same part.
Now, we will try a bed in the different direction, and for this, we will use a different feature.
Edge Flange
Now we will use the Edge Flange feature in the Sheet Metal tab.
Go to the Sheet Metal tab, click Edge Flange, and select the topmost edge on the opposite face to the existing bend. A preview of the bend should appear, as below.
We can manually drag the Flange Length with the mouse cursor, or we can change it numerically in the Property Manager. Here, we will set it to 75mm.
Click OK, and the preview will disappear and the bent part will appear in the graphic area, as you can see in the screenshot below.
So there you go. There are two methods of creating a bend from a flat sheet, using the Sketched Bend and the Edge Flange feature.
There are other advanced features such as Mitre Flange, Jog, Hem which add other features to the base flange. We will examine these in a future article.
Next, let’s look at another important feature for basic sheet metal design.
Brackets and sheet metal often require fastening with bolts and other fasteners, and so the sheet metal requires holes.
Adding Holes
The section for making holes on sheet metal parts is found in the Sheet Metal tab, as seen in the image below. Making holes in sheet metal is simple. It’s the same as making holes or extruded cuts in the main 3D modelling section.
Take the existing bent part from the previous section and create a sketch on the horizontal face for reference. We have used the midpoint of the longest edge of the top face, and sketched two lines measuring 12.5mm each.
These will serve as reference for the centre of our holes.
Now we can use either the Extruded Cut feature if we wish to create holes that go through multiple faces / surfaces, or we can use the Simle Hole feature if we are just going through one section.
We will go through the one section only, so we can use the simple hole.
Select the Simple Hole feature, and click on the top face where our reference sketches are.
A preview of the hole will appear, as below.
If the hole preview is not perfectly aligned with the reference line, then don’t worry. Simply click the centre of the hole preview, and drag the hole so it is coincident with the point at the end of the reference line.
Now repeat for the other side, using the other line for reference.
Note that this step must be repeated for each hole when using the Simple Hole function.
If we wish to create multiple holes at once, we can use the Extruded Cut feature, as per the main modelling process.
In the image below, we have sketched 2 holes (in blue) in the lower horizontal flange.
We can now select the Extruded Cut feature, and create two holes in one move rather than having to repeat the Simple Hole function twice.
Fillets and Corners
Finally, let’s briefly look at adding fillets and corners. In real life, you may wish to get rid of those sharp corners for safety and handling reasons.
On the Sheet Metal tab, you will see the Corners section, along with a little arrow beneath it.
Clicking the Corners button will open up a drop-down menu showing Closed Corner, Welded Corner, Break Corner/Corner Trim, and Corner Relief.
Click on the Break Corner/Corner Trim feature and you will see the panel open up on the left, as in the image below. This is where we can add a chamfer / fillet, and remove the sharp corner.
This feature works just like the chamfer/fillet feature in the main modelling section of Solidworks. You simply select Chamfer or Fillet from the Break Type section in the Properties Manager, select the length of the chamfer or radius of the fillet, and click the corners in the graphics area.
You can see this in the image below.
When you are happy with the size and type of the corner break, simply press OK, and you are done.
If you have followed the steps, the final part should look like the image below.
Conclusion
Congratulations. You have made a bracket using the sheet metal features in Solidworks.
In future articles, we will look at the more advanced sheet metal features, and we will also look at how to flatten the part so it can be added to a drawing suitable for manufacturing.
Until then, feel free to play around with the other advanced features on the existing bracket that you just created. Experimentation is a great way to learn!