2D profiling is one of the main applications of cnc router. To machine 2D profiling, we should have a toolpath file for that. How to create 2D profiling tool path? Briefly speaking, three steps total, create new model, edit vector and create tool path. Full details of using ArtCAM software to create 2D profiling tool path is as follows. EagleTec is experienced china cnc router manufacturer. We also provides design file library which contains minimalist stype 2D wood door designs, 3D door designs, and European style furniture cnc stl files.

Here is the guide step by step. (ArtCAM Pro 8.1)

1. Create New Model in ArtCAM Pro 8.1

Click “Create New Model” icon in ArtCAM software, appears “Size for New Model” dialog box. The size here means the block size (material size). We need set four items here, Height(Y), Width(X), Origin point and Unit (mm or inches). Height and width is set as per the actual size of your block; Unit is selected as per your habit; the origin point here means the material origin point, it is also called zero point; origin point normally choose left bottom corner. After parameter set, please click “OK”. As example, the size we set “100, 100” here, unit we select “mm”.

2. Edit Vector

Find “Vector Editing” icon in the left side of ArtCAM software interface, choose the right vector shape you need, we take circle as example here. Click “circle” icon, appears “Circle Creation” dialog box

(1) Circle Center Setup: input the coordinate value of circle center here. The coordinate point here is relative to the zero of the work piece. We set “50, 50” as example here.

(2) Circle Size Setup: we can do in two ways: radius or diameter. As example, we set radius value 30 here.

(3) Preview: click button “Preview”, we will see the shape we are going to create.

(4) Create: if everything is ok, then we click the “Create” button and then “Close” button.

3. Create Toolpath

Click the “Tool Path” tag in the lower left corner of the ArtCAM page, and the toolbar concerning tool path will appear on the left side of the page. Click the first icon "2D Profiling" in 2D Toolpaths tag, and "2D Profiling" dialog box appears, set the parameters as follows:

(1) Profile Side: we can choose outside or inside. The difference between them is that, “outside” refers to machining along the outside of the vector; “inside” refers to machining along the inside of the vector. Here we set “inside” as example here.

(2) Start Depth: from where the material being machined. Normally, we set 0.

(3) Finish Depth: final depth you need. If you want cut down 5mm, then write -5; if want 10, then set -10. Here, we set -5 as example. Please noted that the value here must be minus.

(4) Allowance: we set 0.

(5) Tolerance: keep 0.01.

(6) Machine safe Z: specifies the height above the surface of material at which it is safe to move the tool at rapid speeds between tool path segments. The value should be large enough to clear any clamps used to hold the job. Click on the small black triangle behind, pop-up "Home" position setting dialog box, the home position specifies the starting and ending position for the tool before and after processing, such as X0 Y0 Z15.

(7) Tool: Click "Select" button, tool groups database appears. We can select the tools we needed in the list here; if the tools in the list do not have what you need, we can add tool. For example, we want to add 6mm round bottom engraving tool, we can set this way: click “Add Tool” icon - “Tool Edit” dialog box appears: 1. Description: name the new tool 2. Tool Type: select “Radiused Engraving”, and edit the tool in right side: diameter 6, half angle 18, tip radius 1.5, step down 3, flute length no need set, step over 0.6, spindle speed 15000, feed rate 70, plunge rate 30. Two nouns are explained here: 1. Step down: the engraving depth of each layer during engraving; 2. Step over: the distance between two adjacent tool paths, which determines the fine degree of the finish: general settings is from 0.2 – 1.0; the smaller the value, the higher the fineness. To modify the tool parameters, select the tool, click Edit, modify, and click “OK".

Here as example, we select “Endmill 3mm”; make step down 3.0 mm; click “OK” and then click “select”.

(8) Material: click “Setup”, pop up dialog box of material setup; the value entered in material thickness should be no less than the absolute value of finish depth; material Z zero, select the top; model position in material, select top offset and set value is 0; finially, click “OK”.

(9) Click “Now” icon. The tool path start calculating (red lines)

(10) After the calculation is completed, click on tool path icon in the lower left corner of ArtCAM; select the first icon “Simulate Toolpath” in the Toolpath Simulation column; dialog box pop up, select “standard” option; next click “Simulate Toolpath” icon and simulation starting; check the effect after simulation finished; if it is satisfied, then save the tool path.

(11) Save Toolpath (output toolpath file from ArtCAM software): select “Save Toolpath” in the left side column “Toolpath Operations”; dialog box pop up; select “Model Master 3 Axis Flat(*mmg)” in lower right conner and click “save”; name the toolpath and click “Save” icon.

Free ArtCAM training course can be provided to you after your contact.
Suggested course: ArtCAM Tutorials: How to Make 3D Relief Toolpath

To buy ArtCAM software, please inquire now. 

                                                                                                                     Origin article from Jinan EagleTec CNC Machinery Co.,Ltd. 
                                                                                                                     Repost please indicate the source.