Haas NextGen dynamic toolpaths question

[Charlie Pierson]

We have a new Haas VF2SS with the high speed machining option.

Are there any special codes (such as Mazak's G61) to turn this function on/off ??

Thanks in advance.

[kccadcam]

Are you talking G187?

https://www.haascnc.com/service/codes-settings.type=gcode.machine=lathe.value=G187.html

 

[kccadcam]

Our UMC-750 post is setup like this:

 

[Colin Gilchrist]

53 minutes ago, Charlie Pierson said:

We have a new Haas VF2SS with the high speed machining option.

Are there any special codes (such as Mazak's G61) to turn this function on/off ??

Thanks in advance.

As Kevin has mentioned, the code for Haas is G187, with "P1 - P3", used to specify the "machine mode". (P1 = Rough, P2 = Mid, P3 = Finish). There is also an optional "E" parameter, which is the "Max. Corner Rounding" value.

The "P level" will change the Accel/Decel profiles, for how hard the machine can be pushed. This is really better to apply for the "old-school" pocketing method of cutting. Although, if you are doing Surface Machining, you will see a difference.

The biggest issue you will face during testing is this: When you are using the Mastercam Dynamic Paths, the motion of the toolpath itself has already been "smoothed out", with Arcs, if you are using the Mastercam Toolpath Filter Settings. (Create Arcs/Reduce Lines.)

The code to "turn off" the HSM Mode is "G187", with no P Code, or E Code on the same line. (All this does is set the machine back to the "default" HSM Mode. (Typically G187 P2, with E0.02)

Typically I will use G187 P2 for Roughing and Semi-Finishing, with an E value between .004-.040.

For Finishing Ops, I will use G187 P3, with E0.0002. (Basically, you want "very little" corner rounding, and you want the machine to "track closely with the programmed path".)

 

 

[Charlie Pierson]

Thanks to all for the info I needed and the quick responses