Cheating Mastercam to get a good toolpath with an undercut tool

[crazy^millman]

I have a 11" deep chamfer in a tight area. I have a 100mm dia tool cutting the 1" tall undercut. I have a chamfer above it I need to cut. I roughed the undercut using Dynamic Contour toolpaths and then steeped up in 2 increments to get most of the meat out of there using the same process. Now I want to semi finish in this roughing stage with .025 step up increments. I went through all my bag of tricks to get a good toolpath using this undercut tool and got flowline to get me motion, but it kept wanting to retract through the part. Not good. I need to keep the tool coming back to center to flush the chips then go back to each cut. I was thinking okay really old school way I would do this with pencil and paper is G0 to center then G1 to start of Arc Swing arc then back to center then move up rinse and repeat. I know my tool diameter and such and could make code by hand in maybe 10-15 minutes. Flowline is close so I just turned up the arc tolerances and made it give me good arcs. I then saved the toolpath to a level and deleted all the retract moves. Now I have a bunch of circle that represent the center line of the tool. I need to get it to the center and back at each .025 cut. I remember someone putting up about points and then using the lead in/out with no values, but tell it use entry and exit points. I have a toolpath that goes down the center of the hole to the 1st point. Then moves out to center line and swings the arc. I then move back to the same center point and then move up .025 to the next center point and finish and repeat. Now I have 25 chains and 25 points to work from and a chain manager that is full of stuff, but start to finish motion that I can be confident will give me what I want. I have one point toolpath in to use my 1st dynamic undercut roughing, then my 2 step up to rough the chamfer and then my semi finish chamfer and then my one point toolpath out. Nice clean motion that will do everything I need. Yes a lot of work getting to this point, but now I bent Mastercam to my will and got exactly what I wanted to make a good toolpath that is safe and efficient.

Just wanted to share a way to use Mastercam that will hopefully be helpful to others. Have a good weekend.

[crazy^millman]

Got to the next chamfer and nothing was working. I did however have a lower chamfer that is the mirror of the upper chamfer on the middle section. I got to thinking if I could mirror that toolpath and then offset it the difference of the 17.5mm thick X 100mm diameter then I could use it to drive the toolpath. Nope mirror was haing a fit and wanting to flip it into the part. I have motion that works, just need to get it into place then drive it correctly. I back plotted that toolpath then saved that to a level. I then Dynamically moved it and spun it like I wanted. I then had to use make spline with the 2 chains that were over lapping in the start and end of my spiral, but now I have a Flowline Spiral cutting top to bottom to the bottom chamfer and a bottom to top spiral cutting the top chamfer. Geometry is just that and if you use it the correct way you get cut just about anything.

[?Mark]

Using undercutting tools in some tight spaces has been my bread an butter for the last several years. It's always a battle, but a best lesson here is to get creative and try new things. There is always a way to "skin that cat"