[ANorwood]

I am currently having to make a piece of tooling that has an ellipse slot that is .079 deep by .158 wide. I am using a .158 Ball Mill and have used master cam to write a contour program to ramp it in at .01 per step. That has been successful, but I am trying to avoid a gouge at the end where it makes its final pass and come up out of the work when finished. Is there any way I can have it ramp in like I have it currently, make a pass as final depth then ramp out along the same chain? Very much hoping someone understands what I am getting at haha.

Also attached a pic of the finished part to give an idea.

[qnet2]

Like this?
check the settings on the lead in

[ANorwood]

Like this?
check the settings on the lead in

Guess I should have mentioned I am running MCX4. I have played with the lead in/outs, however they do not follow along the same chain so I turned them off on the original.

[qnet2]

use the leadin /out specify the height of ramp in the box there, and make sure you are selecting tangent . then it will ramp down and up.

you do have cut parameters set to off , right? so the center of your tool is centered over the chain

[ANorwood]

use the leadin /out specify the height of ramp in the box there, and make sure you are selecting tangent . then it will ramp down and up.

you do have cut parameters set to off , right? so the center of your tool is centered over the chain

I do have cutter comp off. When I set a lead out even with a ramp it still wants to come off the chain resulting in a gouge. When I set and arc radius of 0 and keep the line on tangent with 200% length it stays in the chain, but still just comes straight up, no ramp. I added a screen cap here.

[qnet2]

post your mastercam file here and i'll see if i can fix it, zip it first

[txcncman]

Draw in geometry yourself to drive the center line of the tool and then contour 3D. I just did that today on a part where any combination of lead in and lead out would have gouged the part.

[qnet2]

A few times ive not been able to get MC to do what it should. and i had to restart the project with a fresh new file, then it worked. dont know why

Txcncman did you look at the mc file i posted? did it look right to you?

[txcncman]

No, I did not look at your file. I am not at the office and do not have MasterCam at home.

[ANorwood]

Draw in geometry yourself to drive the center line of the tool and then contour 3D. I just did that today on a part where any combination of lead in and lead out would have gouged the part.

Ahh ok, I'll try that and see how that goes. Guess that makes sense. I don't do much work in 3D except a project that I had to do a Flowline on a couple weeks back.

[Superman]

"ellipse slot that is .079 deep by .158 wide. I am using a .158 Ball Mill "

ahhh.... isn't this just a normal slot, done to the depth of the radius of the ballnose cutter


OK....the geometry to select is the centre of the actual slot
- tool comp = OFF
- XY offset = zero
- lead in/out = OFF
- Ramp pitch stepdown = 0.010"

toolpath created is a helix down to depth, then a final cleaning pass at full depth
---- as soon as the tool has lifted off the part ie 0.001", it can then rapid back to the clearance plane - if you need it to feed out of the cut, then uncheck the rapid retract on the tool parameter page