Y-Axis Lathe

[rchipper]

Hello,

 

Still being fairly new to Mastercam, I have very limited experience with y-axis programming. I did receive feedback from the forums a couple of years ago regarding C and Y stuff. I have not done any Y axis work since then and I having a memory laps.  I did do a search for it but I did not find anything. Would someone out there be willing get me pointed in the right direction and refresh my memory. I have a solid model of a sample part should there be anyone up for it.

 

I tried a couple of tool paths but the code is not outputting moves. Am I in the wrong plane? wrong direction, wcs? I will keep working at it.

 

 

[The Cathedral]

The first thing I would do is make sure you have a post capable of outputting Y-axis. If you don't, you'll never get Y-axis code no matter how hard you try.

[MSL]

Hi,

Do you have a sample file to share?

[rchipper]

This is a sample part. I am not understanding the planes and views. What I was looking for is for the "top",(with hole config.) side to be C0, the "back" side to be C270 and the "front" side to be at C90. With the tool approaching from the back side, perpendicular to the Y axis, have I established the wrong position for the part to begin with? The code I am getting has the back as C0, top is C90 and front at C180.

 

I am using the generic C-Y axis slant bed lathe post as the custom Post I have for this machine is no longer working, had several programmers here before me. Another issue I need to deal with, EEEEESH.

LATHE Y AXIS 8-4-14.MCX-7

[The Cathedral]

It takes a second to wrap your head around the planes in lathe. Your standard tool travel on the lathe--which is X axis on the machine--is the Y-axis in mastercam. The z-axis on the machine is your x-axis in mastercam. C0 is always parallel to the y axis. So when you are in top view, what you would think of as the "top" of the part is perpendicular.

 

Basically, instead of like in Mill, where Top is as if your are looking down the centerline through the spindle and tool, in lathe it's as if you're standing in front of an actual machine.

 

If you want the hole to be C0, you're going to have to rotate your part.

[rchipper]

Ahhh.

 

Then what I had as the top would become the back, the back would be the bottom and the front is now the top plane. Right? So I rotated the part, and re chained  the geo and set the new planes, aside from the top reversing the tool path 180 deg. It looked ok. Question. Why is it when I set wcs's and go to views the part flips around 180 deg.? Oh boy.

[The Cathedral]

Your WCS should always be "TOP".  You change your T/C planes to the face you are trying to machine, but keep the WCS top. That way the post knows how to rotate the part properly.

[The Cathedral]

like this:

 

 

LATHE Y AXIS 8-4-14.MCX-7

[rchipper]

Thank you very much for the lesson. It is more clear to me now.

 

Respectfully,

rchipper

[Colin Gilchrist]

What you have to look at for programming any 4 Axis Lathe in Mastercam is the setup of the planes. The Back Plane (T/C Plane) is always read as the C Zero starting position. This is a function of the way MP is setup. There is a pre-defined variable in the post called 'rotaxtyp$' (rotary axis type). Depending on the setting of this variable, MP will process planes differently.

 

As long as you set Back to be your C Zero starting position, and create all the planes as a rotation of that starting plane, then your code will come out correctly. Enabling a Y axis is set in the Rotary Axis dialog of each operation type when using the standard Mill toolpaths. The secret to using the Mill toolpaths properly is making sure you set a correct T/C Plane before you begin creating the toolpath.

 

Mastercam Lathe also has "C-Axis" toolpaths available. These toolpaths are nice because they take care of setting the correct plane for you. Of those "C-Axis" toolpaths, the "Cross" toolpaths do no support Y axis machining. You'll need to use either Face Contour, C-Axis Contour, Face Drill, or C-Axis Drill, and set the option in the operation dialog to get Y axis output.

 

Also, keep in mind that your machine likely has limited Y axis travel. Sometimes it helps to use a Cylindrical or Polar Milling cycle instead of using XYZ, since you can get the C-Axis involved to substitute for the Y axis. Typically, in a Mastercam Post, the canned milling cycles are activated using MI4.

[rchipper]

Colin,

 

Thank you for taking the time to explain this. Aside from the post dialog I understand what you are saying. Now I need to practice, practice, practice.

 

Once again, thanks to all of you for the support.

 

rchipper