Surfacing and the HSM option

I am making some parts with some 3D surfacing for the first time, and noticing a noticeable stutter or slowing down when the machine gets to corners, steep sections, etc. I'm running a 1/4" ball EM at max machine rpm (7500) and ~120 ipm feed. The program is as output from Mastercam X5. Maybe more surprisingly I've also seen this issue when using HSM type clearing tool paths at 70-100 IPM, where the tool is only moving in X and Y but seems to stutter in corners where there are lots of small line segments.

As an experiment I turned on the 200 hr trial of the HSM parameter, and it made a noticeable difference. I guess I'm surprised that I ran into this issue at what I thought were fairly reasonable feeds, compared to what the machine specs say it can travel at. I think a contributing factor is also that mastercam is spitting out lots of small moves rather than arcs. The programs are also too large for my 1MB of memory (again, WTH Haas?) so I'm running it off of a USB stick. I tried a smaller portion of the same program from internal memory and didn't see a difference.

Yes, I know a machine with higher rpm would be better for aluminum, and yes I know should have bought the HSM option, but this machine was all I can afford at the time so I'm using it as is for now.

Am I just running into the limitation of the control's 'look ahead' capacity without using the HSM option?

Two things: In Mastercam, you need to work with filtering your toolpaths. Let it assign G18 and G19 codes as needed. Keep changing filter settings and watch the size of the toolpath after it regenerates. You'll learn quickly what does what.

Before you do that, try this: Insert G187 P1 E0.010 before your roughing ops (or any op that you want to feed quickly). The P1 sets servo accel parameters to "rough", which accelerates / deccelerates harder. P2 is "Medium" and P3 is "fine". Don't fuck with P3 at all. Ex.xxx represents an accuracy parameter of some sort. Don't be scared to use larger numbers... the factory setting here is .025 in 2007. Mess around with this stuff and you'll be making big gains.

120 IPM is reserved for fine 3D finishing only in my shop.

Sorry I should have been more specific, this is for a final finishing pass only.

My lack of knowledge is going to show here, but I tried reading about the filtering settings in mastercam and still didn't get a clear idea of what exactly it does. Guess I've got some experimenting to do.

The Haas high speed machining option is really a "doing anything other than going in a straight line for a long distance" option.

I, like you, assumed that since I didn't think I did HSM, I wouldn't need the HSM option. Turning it on made a significant difference in just about every real world operation.

You're going to need the HSM option if you're doing ANY surface machining period. You need the extra look ahead for all that code, and 3 lines ahead won't help at all.

I use 2:1 ratio with .001-.0005 tolerance
View attachment 52870