FreeCAD News

The Path work­bench in FreeCAD can help you cre­ate tool paths for CAM for a wide vari­ety of CNC machines and G‑code fam­i­lies. Let’s walk through how to begin using this work­bench in this first part cre­at­ing and curat­ing cus­tom tool bits. In part two we’ll con­tin­ue set­ting up cut­ting oper­a­tions and look at export­ing G‑codes for our machines.

As a sim­ple exam­ple object to work with, in a new project, move to the Part work­bench and cre­ate a 30mm diam­e­ter cylin­der that is 10mm tall. Cre­ate a sec­ond small­er diam­e­ter cylin­der, say 15mm diam­e­ter and right click, select trans­form and move the small­er cylin­der upwards a lit­tle so that when we cut it out of the larg­er cylin­der it leaves a small pock­et­ed area. Final­ly select the larg­er cylin­der in the com­bo view, then use con­trol and select the small­er cylin­der and then click the boolean cut tool. You should now have a flat cylin­der with a cir­cu­lar hole or pock­et cut part way through.

Next, let’s move to the Path Work­bench. As a note about how this tuto­r­i­al is writ­ten, when­ev­er we say to click on a “Tool Icon” we use the name of the tool icon as it appears when you hover/rollover the tool icon and the descrip­tion appears. This means you’ll need to hov­er over lots of tool icons to find your way around a new work­bench; an excel­lent way to dis­cov­er the tools! We’ve used FreeCAD ver­sion 0.21.1 for this tutorial. 

If it is the first time you have run the Path work­bench, when you select it from the drop down work­bench menu you will see a dia­logue request­ing that you change the unit sys­tem to “Met­ric Small Parts/CNC(mm, mm/min)”. This is used because when we set the fee­drates for indi­vid­ual tools and oper­a­tions you will set how fast the tool moves in mil­lime­tres per minute. To make this change click “Pref­er­ences” and on the “Gen­er­al” tab set the unit sys­tem to “Met­ric Small Parts/CNC(mm, mm/min)”.

In the Path work­bench we will need to cre­ate a “Job” item. The “Job” item in the com­bo view con­tains all the dif­fer­ent infor­ma­tion need­ed for an entire CAM job. It can con­tain one or more tool paths or cut­ting oper­a­tions as well as the infor­ma­tion about which tools are being used and how fast those tools are trav­el­ling and more. To cre­ate a Job, select the “Cut” object in the com­bo view and then click the “Job” tool icon. We’ll skip over the “Cre­ate Job” dia­logue for now but it should have the “Cut” item checked in a check­list, sim­ply click “OK” to cre­ate the “Job” object. You should now see that the pre­view win­dow looks a lit­tle dif­fer­ent with a grey ver­sion of our “Cut” object sur­round­ed by a set of lines form­ing a box, the greyed ver­sion of our tar­get object is a clone of the orig­i­nal which is held inside the “Job” drop down. Also the com­bo view should now con­tain the “Job Edit” dia­logue. At the top of this dia­logue you should see the “Stock” pan­el. In this you can change the size of the bound­ing box of lines around our clone “Cut” object. This rep­re­sents the size of the stock mate­r­i­al we would fit to our CNC machine so you can adjust this to match what you need. For exam­ple if we were cut­ting out this 10mm high cylin­der object on a CNC router we might actu­al­ly use 10mm thick stock mate­r­i­al and not face cut the upper and low­er sur­faces to size, there­fore we could change our stock bound­ing box Z axis val­ues to 0 and 0, this would then make the bound­ing box the exact thick­ness of our “Cut” object. 

The Path work­bench has a small col­lec­tion of built in tools, in this instance the tools refer to the actu­al cut­ter that would be placed into the CNC machine to do the work. There is a huge range of tools avail­able in real­i­ty so it’s impor­tant to be able to cre­ate tool pro­files to match what we have avail­able for our machines. Click­ing the “Tool­Bit Dock” tool icon for the first time you will be asked to set up a loca­tion on your sys­tem to store your per­son­al tool library. You can set this up at the sug­gest­ed path, or you can set a cus­tom path. If you set up a cus­tom path out­side of your FreeCAD instal­la­tion you can then eas­i­ly migrate your tool col­lec­tion to new ver­sions of FreeCAD. Once cre­at­ed it will ask if you want to copy over the exam­ple default tool geom­e­try files, this is worth doing as it sim­pli­fies cre­at­ing a com­mon range of new tools.

To add a new tool click the Path drop down menu and select the “Tool­Bit Library Edi­tor.” It’s worth iden­ti­fy­ing a tool in your col­lec­tion you want to use and per­haps grab­bing a set of calipers to mea­sure the var­i­ous aspects of the tool we need to cre­ate the Tool­bit item. As an exam­ple we can add a 3mm end­mill. In the Tool­Bit Library Edi­tor dia­logue click the “Cre­ate Tool­bit” but­ton. As we want to cre­ate an end­mill select the “end­mill” file in the “Select Tool Shape” win­dow. After select­ing the shape of the tool the next win­dow requires you to give your tool a name. We named our exam­ple “3mm_2Flute_endmill”.

You should now see the new tool entry in the Tool­Bit Library Edi­tor or the dock tool­bit area. Dou­ble click on the new tool and this will open the “Shape” and “Attrib­ut­es” tab. In the shape tab you add the dimen­sions of the tool. So for exam­ple our 3mm end­mill was in total 55mm long with a 25mm long cut­ting edge, the diam­e­ter was 3mm. Mov­ing to the “Attrib­ut­es” tab you can set var­i­ous things includ­ing the num­ber of flutes (which we set to 2 to match our end­mill) and the tool mate­r­i­al between HSS tool­ing and Car­bide tooling.

Unlike some oth­er CAM pro­grams the FreeCAD Path work­bench doesn’t attach speed and fee­drates to each tool in the library, when we add a tool to a job we will auto­mat­i­cal­ly cre­ate a tool con­troller object into which we can add speeds and fee­drates. This makes sense as our speeds and feeds for the same tool bit might be wild­ly dif­fer­ent in use on dif­fer­ent mate­ri­als and or dif­fer­ent machines. We’ll look at this and fin­ish off mak­ing some sim­ple paths and export­ing G‑code in the sec­ond part of this intro­duc­tion to the Path Workbench.