Need Help!- Thread milling with x z c

[murrayclair]

We have a nexus 450m with a matrix cnc. Can someone please reply with how to treadmill with x z c only. I have 2" BSP threads to mill in a 300 PCD.

With the matrix I think I should be able to do this in a manual unit using polar coordinates.

[froggy]

no 3 axes interpolation in G12.1 mode.
Just G code macro programm with each point calculate..

[jimiscnc]

well, the good news is that the thread form is cylindrical, as opposed to a cone (spiral?)for tapered threads. This method does not need G12.1. You can stay in C degrees and be just fine.

i forget the program set up minutia for engaging C axis and turning driven tools on, but these have to follow the proper sequence and be properly nested to start and stop. i remember M210-212 mill mode and lathe mode. Also need C axis brake codes - index clamp, contour mill semi-clamp and no clamp. The "semi-clamp" really helps with the cutting dynamics when milling in C axis. The index clamp is just a higher pressure so as to behave like a toothed indexer coupling when the part needs to remain stationary.

11 TPI = ,0909 per 360 degree revolution

C0.0
G0 Z-.909
G1 U-.2 (engages the thread mill into the workpiece. The number is fudge for explanation only. dont know dia of cutter, so assume it was positioned right at the workpiece prior to this)
G1H-360 Z-1.0 F720.0 (H = incremental C using C always makes the F mean degree per minute. This would be 2 RPM. To get real feedrate means figuring out a lot of circumferences and proportions)
G0 U1.0 (move cutter away)

The Z-.0909 positions the cutter ten threads deep to start. Your one revolution ends up 1.0" deep and eleven total threads. This is for a multi tooth cutter. You could also use a single tooth and rotate the part 11 times while moving Z 1 inch deep.
I'm a little fuzzy, but I think the H - would result is a right hand thread.

H is being used because C axis can be set up two ways by parameter. The ungood way is if its thinking shortest path, in which case. if you're at C0.0 and program C360.0 then the command is instantly satisfied and no motion takes place. You could still get there by programming C in less than 180 degree increments, but then you'd have to calculate the proportional change in Z with each block.

I ignored the ramp on and off because that takes some calculations. the concept here is to maintain a helix when you tangentially ramp in. If the ramp sweeps 90 degrees to get full engagement, Z should change 25% of .0909 in the ramp on arc.

The ramp on off stay in helix is to minimize undercuts and dwell marks at the start and stop of the cut.

It is much easier to visualize if you think of an X-Y plane on a typical VMC. You put your cylindrical part in a stationary chuck and contour mill in X-Y as Z advances in a linear proportion. Which is helical. The tool to workpiece relative motion is pretty much the same, but it's much harder to visualize on a 3 axis mill turn lathe!

Nice machine you have there.

-90% Jimmy

PS - in general, it is not best to ever G0 with C being commanded. give it a high F number instead and stay in G1.

[Integrexman]

Originally Posted by murrayclair We have a nexus 450m with a matrix cnc. Can someone please reply with how to treadmill with x z c only. I have 2" BSP threads to mill in a 300 PCD. With the matrix I think I should be able to do this in a manual unit using polar coordinates.

What do you mean by 300 PCD?