After own a cnc router, we must know how to create toolpath via ArtCAM program so we can make the cnc machine work the jobs. To output the tool path for repief, first we should have a model of relief, that is, what is commonly known as BMP file. In this post, we are looking at how to creat toolpath after you own the BMP relief files. Please see details below.
Want to create your own style unique BMP model file? Please use industrial scanner model creator. Or, you can buy cnc design files directly from EagleTec. 

Detailed steps to generate relief tool path is here. (ArtCAM Pro.8.1)

1. In ArtCAM interface, click “Create Model From Image”- “Set Model Size” dialog box appears- No set here- Click “OK” icon directly.

2. Set model size in ArtCAM software

(1) Set the width and height of relief: Top Manual Bar—Click “Set Size”, here the width (X axis) and height (Y axis) is zooming in equal scale; also, we can get another alternative- Set Size Asymmetric, here the width and height can change any way as you like. But considering the relief appearance, normally we only do a little adjustment, do not change too much. Steps: click "Set Asymmetric Size" - input "width" and "height" size – click “Apply”, and then click "OK".

(2) Set the depth of relief: Top Manual Bar – Relief – Scale, input new height, then click “OK” icon.

3. Create tool path in ArtCAM program Pro.8.1: 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 "Machine Relief" in 3D Tool Path tag, and "Machine Relief" dialog box appears, set the parameters as follows:

(1) Area to machine

Whole Model: means all parts of relief have to be machined.

Selected Vector: we can draw 2D vector in the relief model, and choose this option means only part of the vector we selected will be processed, the other part not processed.

(2) Strategy

A. Generally we select “Raster In X”, machining speed based on it is fast; if “Spiral” strategy, the working speed is relatively slow.

B. Raster Angle, generally set value “0” here. If we input 45 here, the tool path is rotated by 45 degree, machining also will be in this direction.

C. Allowance - normally set value 0 here

D. Tolerance – normally set value 0.01 here

(3) 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.

(4) Tool: Click "Select" button, we can select tool

End Mill: The tool which is same size up and down; end mill 6mm means the tool with 6mm blade diameter.

Ball Nose: means ball nose router bits. Ball nose 6mm means ball nose tool with 6mm blade diameter.

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".

(5) Do multiple Z passes: If we do not choose this option, the engraving are not layered and finish in one step down no matter what is the step down value you have set in the tool parameter. If this option is selected, multiple z passes will be made. Start at the value entered in the Z height of first pass field and finish at the value in the z height of last pass field. The step down between these two values is controlled by the step down field in the selected tool. For example, the relief depth is 10mm, step down is 2.5mm, first pass of z is -2.5 and the last pass of z is -10.

(6) Material: click “Setup”, pop up dialog box of material setup; the value entered in material thickness should be bigger than the engraving depth; material Z zero, select the top; model position in material, select top offset and set value is 0; finially, click “OK”.

(7) Switch to 3D view, and then click “Now” icon. The tool path start calculating (red lines)

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

(9) Save Toolpath (Output toolpath file from ArtCAM): select “Save Toolpath” in the left side column “Toolpath Operations”; dialog box pop up, click the arrow rightward, pull the “calculated toolpath” to the right; select “Model Master 3 Axis Flat(*mmg)” in lower right conner; name the toolpath and click “Save” icon.

Free ArtCAM training course can be provided to you if you contact us.
Other suggested course: ArtCAM Pro 8.1- Program Character Engraving Toolpath

To purchase the software of ArtCAM, please contact us. 

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