From Shopbot Wiki

3D Machining:

These are some ShopBot-specific suggestions for setting up toolpaths for machining 3d parts from wood and other materials with similar cutting properties. Refer to the Chipload Calculator under Tools in the ShopBot control software to set appropriate cutter RPMs and Tool movement speeds and try to use the lowest rpms that gives you good router power and edge finish.


For most projects that involve wood that is thicker than ½” you will need to do a Z level roughing toolpath. A Z level roughing toolpath will cut away the bulk of the material around where your finished project will be and prevent the finishing tool from being damaged by excessive cutting loads.

For a Z level roughing toolpath, it is important that the tool you choose can reach into the crevices of your part like the space between letters or something of that nature. Generally a 1/4" end mill works well for roughing, though a 3/8" will be quicker if the project allows. You will want your stepover to be large so that the tool does not waste time recutting area it has already been to – 80-85% works well for for all area clearance and Z level roughing operations. I general you will want the largest mill that will rough thoroughly, with the largest stepdown value that your finishing tool can handle.

You will want your stepdown value to be relatively low since you will be creating terraces with your roughing operation, pockets at progressive depths and you do not want to risk damaging your finishing tool as it climbs or descends the part and encounters the full height of your roughed “terraces.”

 For a 1/16” diameter finishing tool, step down .125. 
 For a 1/8” diameter finishing tool, step down .3
 For a .25” diameter finishing tool, step down .5

A good starting point for feed speed for a 1/4" or 3/8" end mill is 4"/sec in XY and 1" in Z on an alpha, 2-2.5" XY and 1" in Z on a PRT.

Also it's a good idea to leave some material allowance - .02 or .03 is fine, to guarantee that your finishing tool will cut virgin material everywhere and that none of the cuts from the roughing tool will be visible on the finished part.


Your finishing tool will invariably be a ball nose. Typical sizes include 1/4", 1/8" and 1/16", with 1/8" being the most common. If your part has no crevices and only external features it may be that you can use larger tools – 1/2" cutters and larger are common for shaping surfboards. Stepdown is not relevant for 3d operations – multiple passes are not used because it is assumed you have pre-roughed the area to be machined. You will want the largest ball nose that will fully describe your project’s details and the largest bit stepover that provides an acceptable surface finish.

 For a 1/16” ball nose, step over .01”. 
 For a 1/8” ball nose, step over .012-.02” 
 For a ¼” ball nose, step over .02-.032” 

For finishing passes try moving at 2.5”/sec in XY and Z on an alpha machine, 2” in XY and 1” in Z on a PRT.

Remember that these are just suggestions and provide a good starting point...ultimately you're looking for settings that will give you the shortest machining time and good part quality.

Personal tools