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FreeCAD is excel­lent in that it can be used for design projects for all man­ner of fab­ri­ca­tion approach­es. A real­ly inter­est­ing fab­ri­ca­tion approach is cut­ting, bend­ing and join­ing sheet met­al. As such FreeCAD has a ded­i­cat­ed addon work­bench that’s incred­i­bly help­ful in design­ing for flat sheet mate­ri­als. Let’s run through some super sim­ple exam­ples to show off some of it’s fea­tures. Remem­ber that in these tuto­ri­als we always use the tooltip text name to describe a tool icon, so you can find tools men­tioned by hov­er­ing over tool icons and read­ing the tooltip, coin­ci­den­tal­ly this is a great way to dis­cov­er and learn about oth­er tools!

First of all you’ll have to open FreeCAD and install the work­bench. Click “Tools > Addon man­ag­er” and the list of avail­able addon work­bench­es should update. Use the search bar to search for Sheet­Met­al and then click the install but­ton. Wait for it to down­load and install and then you should be prompt­ed to restart FreeCAD.

With FreeCAD restart­ed on the start page click to start a new para­met­ric part project, or cre­ate an emp­ty project, move to the Part Design work­bench and then click to add an active body. As a first exam­ple let’s draw a sim­ple rec­tan­gle sketch and then extrude it to act as the first sheet of met­al in our project. Click to add a new sketch, select the XY plane and in the sketch use the rec­tan­gle tool to draw a rec­tan­gle. In an ide­al world we’d con­strain our sketch­es, but for this sim­ple exam­ple just close the sketch.

Next with the sketch high­light­ed use the Pad tool to pad the sketch, let’s imag­ine our real world mate­r­i­al is some 1.2mm alu­mini­um so we can pad to a height of 1.2mm. Once the rec­tan­gle is padded let’s move to the Sheet­Met­al work­bench. Click to select one of the edges of your padded rec­tan­gle and you should see some of the Sheet­Met­al tool icons become avail­able. Click the “Make Wall” tool. Auto­mat­i­cal­ly an extend­ed sec­tion of sheet­met­al is added with a fold sec­tion and a wall sec­tion at 90 degrees to your base object. Depend­ing on whether you select­ed an upper or low­er edge of your pad object will dic­tate the direc­tion in which the wall extends. You should see a new object “Bend” in the file tree view, feel free to delete it and then try with a dif­fer­ent edge to get the feel of how this works.

In the prop­er­ties dia­logue for a bend (dou­ble click on a bend object in the file tree to access) there are numer­ous set­tings to play with. Chang­ing the length of the new sec­tion and the angle at which it sits rel­a­tive to the base object are easy to adjust. The “Off­sets” tab offers some inter­est­ing func­tions. Often we might want to add a wall that is larg­er than our base object, we can increase the “Extend A” or “Extend B” options to make this pos­si­ble. We can also add “Gap” val­ues and these can be crit­i­cal to get­ting a good final design that works in met­al. On our exam­ple we have adjust­ed the gap A and B val­ues to 5 mm. This not only short­ens the added wall/bend object, but also places small cuts into the base object. The rea­son for this is that if you cre­ate a fold­ed part where the pro­trud­ing sec­tion is small­er than the base sec­tion you’ll cre­ate a dis­tor­tion in the met­al where the cor­ner of the fold meets. You can relieve/reduce this dis­tor­tion by adding a small relief cut into the base sec­tion. We can change the geom­e­try of these lit­tle cut out sec­tions to suit our pro­duc­tion meth­ods. If we are cut­ting the met­al by hand we might leave them quite small and the pro­file as “rec­tan­gle” as we could use a small file to bring the cor­ners square. If we plan to cut the design on a CNC milling machine though we might increase the size of the relief cut to accom­mo­date the tool­ing, and as milling cut­ters tend to be round, we might make the cut round­ed and large enough for the radius of our cut­ter with addi­tion­al clear­ance. This makes it pret­ty straight­for­ward to set up tool paths. 

Of course some­times you’ll want to cre­ate more com­plex fold­ed options. Anoth­er approach that enables more com­plex­i­ty is to draw a sketch of a more com­plex shape and then map anoth­er sketch to it with this sec­ond sketch con­tain­ing fold lines. As an exam­ple in a new project we cre­at­ed a part design body, and drew a sketch in the XY plane. Back in the Sheet­Met­al work­bench we select­ed the sketch and then used the “Make Base Wall” tool to cre­ate our base sheet object and set it to the thick­ness of our tar­get mate­r­i­al. Next we high­light­ed the upper face of the object and moved to the Part Design work­bench. We then cre­at­ed a sketch attached to this face. In this sketch we cre­at­ed a line across the angled sec­tion of the base object, note that we extend­ed this sketch line beyond the base geom­e­try as that’s impor­tant when we come to flat­ten and export our design. Clos­ing the sketch we can return to the Sheet­Met­al workbench.

We can now per­form a fold along the sketch line we just cre­at­ed. To do this we click to select the upper face of the object in the pre­view win­dow (note this won’t work if we select the whole object in the file tree) then we press the con­trol key to mul­ti­s­e­lect and click the sketch item we just made in the file tree view. With those both select­ed we can then click the “Fold a Wall” tool icon and cre­ate our fold at the sketch line position.

Ulti­mate­ly with a fold­ed sheet met­al design you will prob­a­bly want to flatten/unfold the design at some point to cre­ate some kind of out­put flat plan file. This could be for print­ing and then stick­ing the print onto the sheet stock for man­u­al cut­ting or indeed to cre­ate geom­e­try for fur­ther CAM pro­cess­ing for machin­ing. We can do this by first select­ing a ref­er­ence face that we want to flat­ten every­thing else rel­a­tive too. So with our angled fold we just made we select­ed the upper face of the orig­i­nal unfold­ed sec­tion of the design. We can then click the “Unfold” tool icon and imme­di­ate­ly we see a pre­view of the project flat­tened. In the “Unfold Prop­er­ties” dia­logue we can see a few options. We have some mate­r­i­al set­tings which includes a “K” fac­tor val­ue. These val­ues relate to the amount of mate­r­i­al need­ed to accu­rate­ly make the fold as at the fold point dif­fer­ent mate­ri­als will expand and com­press at dif­fer­ing rates. These K val­ues can be found in mate­r­i­al ref­er­ence books or online and you can adjust for your mate­r­i­al and design.

In the sec­tion below we find an “Unfold Sketch Gen­er­a­tion” area and if we check the “Gen­er­ate pro­jec­tion sketch” we can then direct­ly export either a DXF or an SVG from this prop­er­ties pan­el. DXF or SVG are per­fect for print or for poten­tial­ly using with a laser cut­ter or oth­er machines, or, of course, they can make great input items for the Tech­draw work­bench to cre­ate tech­ni­cal draw­ings. You can also apply the flat­ten­ing action and then you have the geom­e­try that you might then use in the CAM work­bench to set up for CNC machin­ing. Even with just these basic uses of the sheet met­al work­bench you can realise accu­rate designs, for exam­ple the author made this alu­mini­um body shelled robot rover some years ago using these methods!

As a final thought, whilst the work­bench is called the Sheet­Met­al work­bench, it real­ly can apply to any foldable/bendable sheet mate­r­i­al. It’s com­mon to see this work­bench used for card­stock cut on a vinyl cutting/dragknife machine or for design­ing for acrylic sheets that will be bent over a hot ele­ment. It’s an incred­i­bly use­ful workbench.