Thread: Milling Flats/Hex with C axis/ X axis moves - SQT-18 MS - Mazatrol T plus

Hi Guys,

Sorry to put up a duplicate thread as there is a similar thread in the machining forum for a different machine.

Now to clarify I am not talking about Polygonal Milling with the special live tool (Z axis). It is my understanding that you can move the C axis with a X axis feed with a live tool and create flats and shapes. I'm new to this so I need some schooling. How does this happen on a Mazak?

This procedure is similar--but just the opposite--how a CNC mill can interpolate a circle just using X and Y axes without a rotary table.

Tool is parallel to spindle. End mill is fed down in X as C is rotated. At center of flat, X axis now feeds up in X as C is still feeding same direction. The C-axis has to interpolate any flat that is not in line with the center.

Any flat that IS lined up with spindle centerline (screwdriver slot for example), C axis is locked at 0° while endmill feeds down to X0. After X gets to center, C axis rotates to 180°, locks, then X axis feeds up to finish slot.

Thanks Philabuster,

I understand how you would do a feature on the end of the part (Like a hex for example) with a Z axis tool.... but what about a Hex that's in the middle of the OD of the part that you cant' reach with a Z axis live tool?

You need a Y axis to get it all true and proper.

If milling the polygon shape on the perhifery of the bar without Y you'll end up with a polygon that is 'wrapped' around the part at best.
Maybe that's what you want... If thats the case then the question is programming it in Mazatrol, and I can't help.

Originally Posted by Tom3197

Thanks Philabuster,

I understand how you would do a feature on the end of the part (Like a hex for example) with a Z axis tool.... but what about a Hex that's in the middle of the OD of the part that you cant' reach with a Z axis live tool?

I have milled a hex on various bolt shaped parts with the X axis live tools without Y axis motion. This works just fine as long as the flat length is smaller than the end mill diameter. Plunge in on Z, index C axis 60°, plunge in, etc, then part off. I often do these operations by <cough> lying to the machine and telling it to do a face drilling cycle. Works good and easy to program. My old T-3 machine doesn't know--or really care--that it has an OD end mill called up to do face drilling, but new machines might throw up an alarm.

Ok, I've just got some new toys sitting around so I'm trying to wrap my head around what I can and can't make them do. I had a part print on my desk that was basically a 8" long shaft that had a two hex features towards the middle of the part and was trying to figure out how to do them... I can do one of them the way you have described Phila, but I can't do the second that way because of a turned diameter that is larger than the Hex corners and is only located .100 away. I would need to invest in one of those polygonal turning tools to do this feature because I don't have the Y axis. But at the same time I've heard those are *really* only good for softer materials... they probably wouldn't like the Stainless.

Originally Posted by Tom3197

Ok, I've just got some new toys sitting around so I'm trying to wrap my head around what I can and can't make them do. I had a part print on my desk that was basically a 8" long shaft that had a two hex features towards the middle of the part and was trying to figure out how to do them... I can do one of them the way you have described Phila, but I can't do the second that way because of a turned diameter that is larger than the Hex corners and is only located .100 away. I would need to invest in one of those polygonal turning tools to do this feature because I don't have the Y axis. But at the same time I've heard those are *really* only good for softer materials... they probably wouldn't like the Stainless.

I haven't done it yet, because I haven't needed too, but my plan to accomplish what you need should the time arise is to use a woodruff cutter and cut X and C only.

Phil helped me program this part about a year ago:


I used the same endmill to cut the hex and and round pocket in the center instead of using a facegroove tool.

I like that idea David, I would need the tool to reach another 4" back from the front of the part to get the feature.... it could work! Also, you have a PM. Thanks for all your help guys, I'm sure I'll have more questions!

Originally Posted by Tom3197

I like that idea David, I would need the tool to reach another 4" back from the front of the part to get the feature.... it could work! Also, you have a PM. Thanks for all your help guys, I'm sure I'll have more questions!

Just a thought, if the woodruff cutter diameter was large enough maybe you wouldn't need to have it hanging 4" out...?

Very good point... Didn't think of it that way...

Originally Posted by Tom3197

Very good point... Didn't think of it that way...

As long as the diameter exceeds the tool holder by more then the depth (measured from the largest OD in your way) of the flat you need to cut you should be golden... At least that is what I would do

Absolutely, a great way to do it! Its the "little" things like this that make this forum great.