Machining a taper

[CNCMike]

Hi Guys,

I am having a hard time getting the tool path I want for machining a shallow taper. The part being programmed has two parallel surfaces with a height difference of about 1/4". The surfaces are connected by a angled surface several inches long. When trying to machine this angle the tool path generated is a back and forth motion (X-axis) with many passes. (I used parallel rough or finish rough tool paths).

 

The part in question was programmed long hand before we started using MCX2 and a 3" face mill was used in a single pass along the Y-axis. It would machine both flat surfaces and the taper in one 3D pass. Of course this left a slight curve on the part because of the curved cutting surface, but in this situation it is very acceptable.

 

The reason we can't (don't want to) just use the old program is because we are trying to standardize our programs to MCX2. If you have any suggestions I would appreciate it! BTW, the controller being used is a Fanuc OM.

 

Thanks, Mike

[Elmer Fudd]

Will a 3D contour work?

[CAM-mando]

If I understand correctly, you want a single pass Y axis motion then Y/Z ramp up then another Y axis move. You could simply use a contour (3D). And chain geometry that matches the numbers in your current program. In this case you have calculated the tool offset amount and are programming direct tool center. This would work since you already have the numbers in a program.

 

I think the best toolpath starting from scratch (ie with the 3 surfaces modeled) might be a curve 5axis with output set to 3 axis.

 

You would draw the cross section, copy it in top view and create a ruled surface between the two contours. Use that surface for the curve 5axis toolpath.

 

Use Tip Control "on projected curve" and Projection "normal to plane".

 

If you want to use one of the surface toolpaths you will have to change the cut direction and then play with the stepover / tolerances to force it to give you a single pass.

[Guest]

you could also project a straight line tool path down on the 3 surfaces as well.

[CAM-mando]

John's suggestion might be the simplest.

[CNCMike]

JParis,

Do you mean something like a center line (using create line)? I am not sure I totally understand, but I will give it a shot tomarrow. I might figure it out as I go.

 

Thanks everyone for the replies, Mike

[Hardmill]

Mike try changing the cut direction on the

parallel toolpath to 90degs and give it a

large step over.

 

 

PEACE

[Colin Gilchrist]

CNCMike,

 

That is exactly what John is referring to. Create a straight line above your part that you want the centerline of the tool to follow, then use the Surface Finish | Project toolpath.

 

Mastercam will project a toolpath down onto your surfaces that compensates for the tool/corner radius.

[CNCMike]

Thank you everyone for the suggestions. Everything worked out very well using the parallel rough/finish and also project tool path.

 

Mike

[heavychevy2155]

I use the Ruled wireframe toolpath to cut angles and tapers, but I only have level 1 so I do the best I can. You can copy and past that toolpath and add stock to leave, then use a trim toolpath using the front or side planes and create a surface rough and finish toolpath with Level 1.