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Some­times we might need to share a 3D design in the form of a 2D tech­ni­cal draw­ing. FreeCAD has an entire work­bench, Tech­Draw, with a col­lec­tion of tools to help you do this.

To explore Tech­Draw we need to have an object that we want to make a tech­ni­cal draw­ing of. Let’s just quick­ly cre­ate an object. On the FreeCAD start page click the “Para­met­ric Part” option from the “New File” win­dow. This cre­ates a new file and jumps to the Part Design work­bench and cre­ates an active body. Click the “tasks” tab and select to “Cre­ate sketch” or click the “Cre­ate sketch icon”. Let’s select to draw our sketch in the XY plane.

Draw a sketch sim­i­lar to the one in our image. We sim­ply used the “Cre­ate poly­line” tool to draw the out­side line using the “M” key to tog­gle to change to an arc line for the curved cor­ner. Don’t wor­ry too much about your design. We drew a cir­cle inside our perime­ter poly­line to help show some Tech Draw fea­tures lat­er on. We don’t need to con­strain our sketch ful­ly for this exam­ple, but let’s give the base line of the sketch a length con­straint and set a diam­e­ter for the inter­nal cir­cle. We just con­strained these to the sizes they are as drawn. Close the sketch and let’s pad the sketch to the default 10mm.

Next let’s left click the work­bench drop down menu and select to move to Tech­Draw. On first launch in a new project there will only be two tool icons that are selec­table. “Insert Default Page” and “Insert Page using Tem­plate”. First let’s left click on “Insert Default Page”. You’ll notice a new object “Page” appear in the file tree and you should see a blank white page launched in a new tab in the pre­view area. For the sake of explo­ration, sin­gle left click on the “Page” object and let’s delete it. In turn click the “Insert Page using Tem­plate” option. You should see a “Select a Tem­plate File” win­dow appear con­tain­ing lots of dif­fer­ent tem­plate options. These are list­ed with paper sizes so “A4” or “A3” and more, and also dif­fer­ent stan­dards such as ANSI A, ANSI B, ISO5457 and more. Let’s select “A3_Landscape_ISO5457_minimal.svg” and click “open”. This again cre­ates a “Page” item in the tree and launch­es the blank tem­plate in a new tab. This tem­plate has some stan­dard fields added in the low­er right hand cor­ner which, of course, can be edit­ed with your project draw­ings details. Dou­ble left click­ing on an editable field launch­es a small dia­logue where you can edit the field with your details.

Left click back onto the tab con­tain­ing our padded part. In the file tree left click to high­light the “Pad” part and then left click the “Insert View” tool icon. You should now see, irre­gard­less of the ori­en­ta­tion of the part in the pre­view win­dow, a front view cre­at­ed in the tech­ni­cal draw­ing page. In the task tab a dia­logue titled “Pro­jec­tion Group” appears. In this dia­logue you can per­form numer­ous adjust­ments to your insert­ed views. You should see a clus­ter of tick box­es and you can tick these box­es to add cor­re­spond­ing views into your tech­ni­cal draw­ing. If you leave the “auto dis­trib­ute” box ticked then you can use the X Spac­ing and Y Spac­ing inputs to increase or reduce spac­ing between the view. Like­wise you can adjust the scale of the draw­ing by set­ting the “Scale” drop down to “Cus­tom” and then adjust­ing the ratio. You can also flip the axis of the pro­ject­ed group to cre­ate cus­tom lay­outs. Notice you can also switch between first angle pro­jec­tion and third angle pro­jec­tion. A good primer on ortho­graph­ic views, first angle and third angle pro­jec­tion can be found on Wikipedia here.

Note that if you manip­u­late the scale, or the pro­jec­tion angle those fields in the tem­plate page will not update auto­mat­i­cal­ly. We can edit the scale fields but we can’t eas­i­ly edit the angle pro­jec­tion sym­bol as these are set as part of the spe­cif­ic template.

Select some views, and then click OK to close the “Pro­jec­tion Group” dia­logue. You’ll notice that the indi­vid­ual views insert­ed into the page are labelled with a view descrip­tion “front left” “Bot­tom” etc and that they are sur­round­ed by a dashed line. Whilst this view is enabled we can move the entire clus­ter of pro­jec­tion views by mov­ing the main “Front” view. Left click on the “Front” view frame and drag to move the entire group. If we click and drag an indi­vid­ual view frame we can move it lim­it­ed to the axis the view is pro­ject­ed on. For exam­ple if we click and drag the “Left001” view we can only drag it left and right in the page. This is because it would be easy to place a view in an incor­rect pro­jec­tion area oth­er­wise, lead­ing to errors when read­ing the tech­ni­cal draw­ing. A note on view place­ment is that if you dou­ble click to reopen the “Pro­j­Group” item and you keep the “Auto Dis­trib­ute” option ticked then when­ev­er you click “OK” or “Apply” any views you have moved in the page will reset to there orig­i­nal positions.

We can tog­gle the view frames on and off using the “Turn View Frames On/Off” tool icon which also then tends to act as a posi­tion­al lock for the views. We can now begin to add some dimen­sions and oth­er infor­ma­tion to our tech­ni­cal draw­ing. Left click on the base line of the “Front” view object and then click the “Insert Dimen­sion” tool. This tool should look famil­iar to you as it uses the style and nam­ing con­ven­tions used by the equiv­a­lent tool in the sketch­er work­bench. The “Insert Dimen­sion” tool should cor­rect­ly guess you are want­i­ng to add a length dimen­sion and should insert and allow you to place this dimension.

Rather nice­ly now you can exper­i­ment with going back to the sketch of the orig­i­nal item and chang­ing the length con­straint for the base of the item, changes should be pushed auto­mat­i­cal­ly through to the dimen­sions in your tech­ni­cal draw­ing. Chang­ing our, as drawn, 72.36mm length con­straint to 78mm, we can see that this val­ue is updat­ed in the tech­ni­cal draw­ing. Next lets click the “Insert Dimen­sion” tool and select the circle/hole in the front view. This should auto­mat­i­cal­ly add a diam­e­ter dimen­sion that can be placed attached to the cir­cle. How­ev­er unlike in a sketch, you may notice that we don’t have a cir­cle cen­tre mark we can use as a ref­er­ence for the posi­tion of the cir­cle cen­tre. Click the Front View and in the “View” tab under the “Dec­o­ra­tion” head­ing, tog­gle the “Arc Cen­tre Marks” val­ue to “True”. You should now have a cen­tre mark in both the cir­cle and for the arc made as part of the part out­line. You can then select the cen­tre mark, and anoth­er point and cre­ate length dimen­sions to describe the posi­tion of the cen­tre of your hole.

Some­times in tech­ni­cal draw­ings it can be use­ful to add labels and text descrip­tions that aren’t par­tic­u­lar­ly a dimen­sion or oth­er import­ed linked val­ue, a good option for this is to use the “Insert Bal­loon Anno­ta­tion”. Left click on the tool and then click on the tech­ni­cal draw­ing where you would like the point­er attached to the anno­ta­tion to be. A sim­ple point­er line and cir­cu­lar text bal­loon will appear. We can then dou­ble click on this and the “Bal­loon” dia­logue will appear. In this dia­logue we can add our text, and also manip­u­late oth­er set­tings, bal­loon shape, font, colour and more to meet our need.

There’s lot’s left to explore on the Tech­Draw work­bench, but you prob­a­bly know enough now to explore fur­ther fea­tures, it’s also def­i­nite­ly worth look­ing at the offi­cial Tech­Draw doc­u­men­ta­tion which has lot’s of infor­ma­tion on all the Tech­Draw tool­ing. Final­ly you can export your tech­ni­cal draw­ing at any time by click­ing either the “Export Page as SVG” or “Export Page as DXF” tool icons.