Lower Z axis in both directions when machining a single slot

[ngr1]

Hello, I am machining a single slot to a depth of .25". The Z axis is lower only in one direction, how do I program the slot operation to lower the Z axis in both directions.

I could modify the g-code my self but I would like to accomplish this task in Mastercam.

Thanks...Norman

[psychomill]

Are you programming in 2D or 3D? Maybe the slot got rotated in the drawing by accident? Or you cut using 'Ramp Contour' without a finish pass?.......

There's a few things that could've happened here. (hopefully not a butchered post)

[ngr1]

Sorry,I should have been more descriptive.

Just imagine a single line as my drawing which I would like to machine to a depth of -.25" using a 3/16" flat end mill. I would simply like to go back and forth on that line dropping each time by .02" until I reach .25".

My current configuration is using a contour which only drops the z axis in one direction taking twice as long to complete in comparison to cutting in both directions.

I tried an open pocket but it needs an overlap % which when set to 0 produces no tool path.

Any ideas... Thanks!

[ObrienDave]

Greetings,

As with anything else in MasterCam, there is more than one way to accomplish this.

1. Physically create geometry to represent the center line of the exact
toolpath you need.
This way you can run it as a simple 3D contour with the "compensation type"
set to off and when you chain the geometry, you turn the "plane mask" off.

2. Create a vertical line at each end of the slot to represent the CENTER of your
cutter and use the WIREFRAME, RULED toolpath. Once again, turn the
"compensation type" to off.

3. Create a vertical surface to represent the CENTER LINE of your cutter.
Then FAKE it by creating a tool that is EXTREMELY small, such as .00001 diameter

With example 1, you have to change the geometry to change the pass depth.
With examples 2 and 3, you can easily modify the individual pass depths by changing
the stepover value.

The bad thing about these examples is, there is no easy way to change the
plunge feedrate without doing it through the NCI file editor.

I am sure other people will have other ways to do the same thing.

[post_guy]

Just do a regular contour toolpath. Turn off cutter compensation, make sure lead in/out is off. Set the depth to -.25 (abs.) (I am assuming your geometry is drawn at Z0, if it is actually drawn at z-.25, set depth to 0 Incremental). Set your contour type to ramp and click the Ramp button. Now set Ramp Motion to depth and set the depth to .02. You'll most likely want to Make a pass at final depth.

[ObrienDave]

Greetings,

Like I said, I am sure other people will have other ways to do the same thing.

One of my favorite sayings is:

Take 20 programmers and you're going to get 20 different ways to do the same thing.
What counts is the end result and doing it in the least amount of TOTAL time.

I added your example to the ZIP file.

On a side note, I am honestly impressed with the quality of the help that the
members of these forums provide without being rude or condescending.

Proud to be a member.

THANX!

[ngr1]

Thank you!

[ObrienDave]

Your welcome!

[Rekd]

Originally Posted by ObrienDave Greetings, Like I said, I am sure other people will have other ways to do the same thing. ... Take 20 programmers and you're going to get 20 different ways to do the same thing. ...

True, and Mastercam can usually give you as many different ways of doing the same thing.

... On a side note, I am honestly impressed with the quality of the help that the members of these forums provide without being rude or condescending. Proud to be a member. THANX!

This is by far one of the most professional boards I frequent. (And not just cuz I work here.)