CNC West Oct Nov Web

CNC WEST October/November 2018 www.CNC-West.com 57 the machine control would be .001”. Most shops that strictly use CAM software to generate toolpaths use “Wear” compensation as it gives more flexibility with smaller lead in and lead outs. If your ¼” diameter tool measured .251” and your tool offset table had a .001” diameter you would only need a .0006” lead in/out to turn on/off your cutter comp. This allows you to get into smaller pockets and other confined areas. Adjusting the part feature size is done the same way “In control” is done as explained earlier. A common work flow to set up your tool for wear comp is to probe the length and diameter of your tool and then back out the programmed tool diameter from the offset table in the control, leaving only the differ- ence between the programmed tool diameter and the measured diameter. With a well calibrated tool probe it’s common to get very accurate parts with no compensation needed. One trick that is nice for people who have tool probes in their machines is to edit the tool probe macros to back out the tool diameter automatically. This requires a fairly good understanding of Macro programming and editing. method saved a lot of time in having to manually calculate offset tool paths. It makes sense for shops to still use this method when they use both CAM software and manually write G-Code programs. Remember that the line move to turn on/off cutter comp needs to be at least the radius of the tool. This means that the lead in/out lines need to be at least .1251” for a ¼” dia tool. To adjust the part feature size for a boss or a bore you would incrementally change the diameter offset table by the positive or negative amount you want to adjust the size. Exam- ple: A target of boss of 1.000” measured at 1.001” would require an incremental adjustment of -.001”. W ear - The toolpath centerline is output to be off- set from the feature geometry by the radius of the selected tool in the CAM software. Just like with “In control” compensation type the output code for “Wear” comp includes a G41 (right comp), or a G42 (left comp) to offset the tool by the tool radius pulled from the diameter offset table in the machine con- trol. The output code also includes a G40 to cancel the compensation when the tool path is complete. The difference is that the diameter in the offset table in the machine control is typically set to zero or the small difference between the programmed tool diameter and the actual measured diameter. Offset table example: a ¼” diameter tool could measure .251” and the diameter listed in the offset table in Years ago, Henry Llere from Selway helped me edit my macros to automatically do this. It’s a small thing that has saved me hours over the years. This is a great example of why you should have a good rela- tionship with your machine tool partner. I nverse wear - This is identical to “Wear”, except that the wear adjustment is entered opposite of wear. Example: If you needed to make a boss .001” smaller you would change the diameter offset table incrementally +.001. This is driven by settings in the machine control and is less common than standard wear comp. O ff - The tool path centerline follows the feature geometry on center. The output code has no compensation codes. This is commonly used for things like tracing text with an engraving tool. N othing I’m writing here is revolutionary or hasn’t been written about countless times. My hope is to get people that aren’t using cutter comp, or don’t have a solid understanding to learn more about it and consider using it. Beyond cutter comp, we all have details about our trade that we could and should learn more about. Figure 2

RkJQdWJsaXNoZXIy NTUxNTc=