Character engraving is one of the most common functions of cnc router machines. In ArtCAM Pro 8.1, there are many machining strategies which can do this job. Here, we would like to introduce the strategy of smart engraving; below are the detailed steps of using this strategy to program character engraving toolpath via ArtCAM. 

For your information, we also provides cnc furniture design files which contains minimalist stype wood door designs, 3D wood door designs, and European style furniture design cnc stl files. 

Step One. Create New Model

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 three sizes here, Height(Y), Width(X), Origin point and Unit (mm or inches). Height and width is set as per the actual size of 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”.

Step Two. Write the Character (Vector Editing)

Find “Vector Editing” icon in the left side of ArtCAM interface, please select the number five icon “T”; and it appears TEXT TOOL dialog box on the screen.

(1) Font Setup: please select the right font for your characters. We select “Arial” as example here.

(2) Size: please set the right size for your characters. We select “18” as example here.

(3) Type the characters in the blank.

(4) Create: please click button “Done”.

(5) Position the vector: find column “Position Size Align Vectors”, please click the second icon in second line “middle the vector”, the character becomes centered.

(6) Change character size: find vector editing column, please click the third icon in first line, “Transform Vector” dialog box appears; Input the “New Width” or “New Height”, please noted because the width and height are scaled, we just need set one of both. Here, we set “New Width” 80. Click “Apply” and “Close”.

Step Three. Program Character Engraving 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 icon "Engraving" in 2D Toolpaths tag, and "Smart Engraving" dialog box appears, set the parameters as follows:

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

(2) Finish Depth: the depth of engraved characters. If you want the engraving depth to be 2mm, then write 2 here; if want 3, then set 3. Here, we set 5 as example.

(3) Tolerance: keep 0.01.

(4) Option “Vectors are on surface”, checked.

(5) Option “Outer vectors are boundary”, unchecked.

(6) Option “Offset end mills for engraving tools”, unchecked.

(7) Machine safe Z: The value should be large enough to clear any clamps used to hold the job. Click on the small black triangle behind, pop-up "safe Z" and “Home position” dialog box, the home position specifies the starting and ending position for the tool before and after processing; here we set safe Z to be 100, and Home position be X0 Y0 Z100.

(8) Tools List: please click “Add”, “Tool Groups Database” appears, select the proper tool you will use. The tool quantity can be one or multi pieces. Here, we take “small V bit 6mm” as example. Click “Edit”, set step down to be 5mm, the same value as finish depth.  Click “OK” and “Select” button.

(9) Allowance: we set 0.

(10) Tool Clearance Strategy: “Offset” and “Climb Mill”, no change. 

(11) Option “Do corner sharpening”, checked.

(12) Option “Only Smart Engrave Profile”, unchecked.

(13) Option “Profile Only”, unchecked.

(14) Option “Independent Finish Depth”, unchecked.  

(15) 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; finally, click “OK”.

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

(17) After the calculation is completed, click on tool path icon in the lower left corner of ArtCAM page; 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.

(18) Save Toolpath: 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.

Until now, the full steps of programming of character engraving toolpath in ArtCAM are finished.

Any question, please feel free to contact. Free ArtCAM user guide can be provided to you as your request.
Another suggested course: 2D profiling toolpath creation


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