Facing to OD transition, and Partoff paths

[Terminus-Est]

Hey,

Mastercam rookie here hoping to get some help. I am encountering a specific challenge in Mastercam 2024 while programming for CNC lathe operations, particularly when transitioning from a facing operation to outer diameter (OD) turning. My background is largely hand programming swiss lathes. My typical approach with facing and OD  work involves maintaining continuous part and tool contact throughout both operations. I recently made the jump to a new company, and am learning Mastercam for lathes, none of which are swiss.

Up to now I’ve always faced down to a specific diameter (e.g., X0 or X-.016), and then, without retracting or losing face contact, directly transition to OD turn. 

When setting up the toolpath in Mastercam 2024, I’m struggling to replicate this method. The software seems to automatically include a retraction (X+ Z+, then Z-X- to diameter X) or repositioning move after facing, before starting the OD turning. Could anyone advise on how to configure Mastercam 2024 to achieve this specific toolpath strategy? Are there specific settings/ tool path types or a particular approach that would allow for this seamless and continuous operation? 

I’m not at all implying this is best practice, it’s just what I was shown early on and have stuck with. Attached is a code snippet to illustrate my goal. Bar stock would be .250 diameter and part would be a .125 diameter 2.0 inch rod

(--- Facing and OD Roughing ---)

G0 X0.5 Z0.015

G0 X0.275

G01 X.260 F.005;

G01 X-0.016 F0.002 (Face with 0.008 inch radius on tool);

G01 X0.150 (Don’t move Z, go positive X to desired OD diameter);

G01 Z-1.990 (OD Roughing along Z axis);

G01 X0.255 (Turn up past stock diameter);

G00 X0.5 Z0.0 (Retract)

 

If Doing bore work I might face, move to ID work, then finish face and OD as described.

Sometimes the following finish pass would be done with another tool if needed or desired for tool life/geometry/radius, but often I use the same tool and transition directly from OD rough to finish face as continuation of that tool path:

(--- Finish Face and OD ---)

G0 X0.160

G01 X-0.016 F0.001 

G01 X0.125 

G01 Z-2.080(extra material for .079 wide partoff)

G01 X0.260 

G0 X[Retract Position] (Retract to Safe Position)

 

Additionally I have been trying to get the software to do relief cuts past the parts finish length and then come up, chamfer the back side and at the end of the chamfer move straight down in X. Using the same .250 barstock and a finished .125 diameter 2.000 long cylinder/rod. The relief operation begins just beyond the 2-inch finished part length, at Z-2.005. The tool(relieving and cutting off with same tool) relieves down to an X diameter of 0.100 inches. It then retracts to clear the 0.125 inch diameter of the part before positioning to cut the chamfer. The part-off is completed at the end of chamfer. Quick code might look something like: 

(T1 M06) (Partoff tool)

G20

G28 G91 Z0

G0 G17 G40 G49 G80 G90

(--- Part-Off Relief Operation ---)

G0 X0.260 Z2.010

M03 S500

G97 S1500 M03

(Relief)

G1 Z-2.005 F0.008

G1 X0.100 

G0 X0.150(retract and reposition)

G0 Z-1.975

G1 X.130 F.002(prep point)

G1 X0.125 Z-1.985 F0.001(Lead in)

G1 X.095 Z-2.00 (chamfer)

G1 X0. Or X-.[Tool nose radius](Cutoff)

Then sub spindle retract and turret home.

 

I appreciate any guidance or suggestions you might have even if it’s to tell me not to do things this way. I’m open to any and all guidance at this stage. 

Thank you!

[TFarrell9]

What's the reason you want to stick with dragging the tool across the face rather than retracting? You should be able to get the results you're looking for by modifying lead-in/lead-out settings with a finish path, rather than face path. You would have to do the same thing with same thing with the roughing path for the o.d., but it's likely the roughing path will want to face a retract of some sort. If you can one-shot the face and the o.d., then using two separate finish paths with modified lead-in/lead-out settings will be your best bet to not force retracts.

As far as parting-off with a chamfer/radius following a relief cut, those options exist in the cut-off toolpath parameters. 

[Aaron Eberhard]

Agreed with TFarrell9.  It sounds like you want a Finish toolpath, not a Facing toolpath.   Facing is for exactly what it says.  If you're trying to follow a contour around the corner, you should use a Finish toolpath.

[Terminus-Est]

Thank you for taking the time to respond.

I don't have a particular "need" so much as its all I've ever seen done. Prior to the purely swiss shop I was running standard 3&4 axis lathes at another shop and they did it the way I described. To be clear I'm by no means indicating this is how it "should" be done, rather it's all I've ever seen. Very different shops with the exception of both having a few swiss machines, and both using Esprit Cam so perhaps it's just the default method in esprit? It always worked very well on the micro machining we were doing with tight tolerances and surface smooth surface finishes. so many of the parts I was doing being a rough face, bore work and then a combined finish face to finish OD pass. I think the idea was to reduce strange blends and tool wear being confined to the same area of the insert. If I shouldn't be doing it this way totally fine, I would just love to understand the why. 

[JParis]

7 minutes ago, Terminus-Est said:

If I shouldn't be doing it this way totally fine, I would just love to understand the why. 

Heat is the enemy of all tooling...dragging a tool across a surface with no chip being taken, heats the tool unnecessarily leading to premature wear. That's just one reason

[TFarrell9]

Along with what JParis said, it's a waste of time. Sometimes that may matter and sometimes it may not. 

Also, there shouldn't be blend issues using the same tool to cut separate chains unless something is done incorrectly on the programming side. With that being said, I generally rough with one tool and finish with  another. When finishing with a finishing tool, it's generally a continuous path to cut faces and diameters. Even with down-cutting though, you won't see transitions or blend issues unless your parameters are less than ideal.

[Terminus-Est]

That makes sense, I know its extra tool wear and the heat element makes sense. I can only assume we didn't see more issues due to the high pressure coolant(2000 psi) or moving fast and getting off the face quickly. I'll change my approach. Thank you all for the information and sharing your knowledge. 

[AMCNitro]

In order to do it the way you want to you have to get away from using "facing" and just draw your contour all together.  So when you pick your chain it includes the face of the part, just like if you were programing a ball end.  It will work just fine with roughing, but depending how you pick your chain for finish, you might be starting on the face of the part.  For a few years now, I start my finish on the left side of the part, it works better IMO.

That said, I don't think it's a good idea.  If you r aim is to save the time from the retract moves, you can set them to be really short, the turret doesn't need to tract all the way home.