3D Milling (Roughing & Finishing)

[Brakeman Bob]

Hi Matt. I am glad you liked HSM. I find that on jobs with a lot of 3D (I'm talking 10 million lines of code upwards) HSM gives a real time time saving. You are right in that the lead in/out and the links are smoother and this is where the time is saved as the machine isn't straining the acc & dec so much and therefore getting closer to programmed feed.

Another plus with HSM is you will get better 3D finishes that display less facetting than the vanilla 3D routines. The combined strategies are very useful too, as are the options for constraining the tool working area. However, it ain't honey and roses all the way as I find the roughing strategies in vanilla 3D more useful, especially the plunge and trochoidal milling. Still, it is stuff like this that makes CAM such an interesting thing to do for a living isn't it?

Have fun.

Bob

[mattpatt]

CAM is most interesting indeed, but can also be very frustrating when it doesn't generate like you'd want it to.

It's a shame that it's only a part of my job, as I'd like to spend more time on it, but I just don't get the chance.

However, when I see the finished job it's great to know that I made it, start to finish. From idea to finished product. I used to do my own anodizing as well, but my neighbours complained about the smell of the acid, so finally had to farm that out!

[Eclipze]

I've done quite a fair bit of 3D milling, but the one area I struggle with is increasing the speed of movement. I would really prefer to be running at 1000mm/min or above, however for 3D surfaces it slows right down to ~250mm/min. I can reduce the step size with the facet tolerance (large gcode file) and increase the acceleration, however it get to a point where the CNC is shuddering under the rapid accel/deceleration from point to point movement. The shuddering causes additional tooling marks in the surface of the work piece. So I have to reduce the speed.

It appears that Solidcam only generates the profiles with small linear steps, and the resulting movement is stepwise/jerky. Does anyone know if there are any techniques to produce gcode that provides a smoother/faster movement? Does HSM improve on this limitation?

[Brakeman Bob]

Originally Posted by Eclipze I've done quite a fair bit of 3D milling, but the one area I struggle with is increasing the speed of movement. I would really prefer to be running at 1000mm/min or above, however for 3D surfaces it slows right down to ~250mm/min. I can reduce the step size with the facet tolerance (large gcode file) and increase the acceleration, however it get to a point where the CNC is shuddering under the rapid accel/deceleration from point to point movement. The shuddering causes additional tooling marks in the surface of the work piece. So I have to reduce the speed.

HSM would help here and without being more familiar with your machine it is hard to say how much. An awful lot will be down to the machine, the servos and the control. For example, how many blocks ahead is the control reading? Is your control "smart" such as FANUC HPCC? How are powerful are your servo's and are they tuned correctly? When you say you increase the acceleration, do mean you put the gains up and/or the acc & dec? This could be the cause of the trouble as without proper tuning with an oscilloscope, high feed rates can give rise to axis instability.

Have you got access to a ball-bar? If so, run ball bar tests at 500, 1,000, 2,000 and 5,000 mm/min. This will give you a very good idea to the capabilities of the machine. When I worked for a machine tool builder our standard ball bar test was 3,000 mm/min at 150mm radius.
The shuddering you describe at those low feed rates could indicate all is not well with your ballscrews and a ball bar test would show that up straight away.
To give you an indication of what I expect from the machines in our shop, we have a Mori Seiki SH400, 10 years old with Fanuc 16MA and for 3D milling Aluminium I program a Ø6 ballnose at 12,000 rpm and 3,000 mm/min. On very curvy geometry prior to HSM, the machine made it up to about 2,000 mm/min. Programming with HSM and the machine managed to get up to about 2,600 mm/min. And the machine wasn't shuddering, the lost feedrate was due to the movements being too short for the machine to get up to it's full velocity.

[Eclipze]

Thanks for your reply :-)

The CNC runs 305oz/in stepper with Gecko G203V drivers and Mach3. I use the DIN_ISO CNC controller in SolidCAM. The acceleration parameters are set it Mach3. I can easily traverse 3500mm/min without stepper dampers, however usually only cut around 1,000mm/min.

Not familiar with ball bar tests, however looking into it I believe the root cause is the way the gcode is generated. For example, if I do a 2D profile with curves, the end mill will slice through the material and not slow down around the corners. The gcode uses commands to perform arcs. Whereas in 3D milling, the entire gcode is point to point. Any profile curves are now made up of small straight lines between two coordinates.

The limitation of the CNC is the maximum acceleration before the machine flexes (only a small machine). So if I stop with a deceleration of 500, it stops perfectly, but the momentum energy dissipates as a little bit of machine flex from the sudden stop. When this happens running the 3D milling code, it produces a shuddering noise around tight corners, though will reach maximum feedrate where straight sections are machined. The shuddering causes slightly more machining marks on the surface of the material.

So a 2D circle utilising gcode commands for arcs is very smooth and very fast >1000mm/min. A 3D milling operation however falls below 350mm/min and shudders it's way around, where only point to point gcode is utilised.

At this stage, I am unsure as to whether a solution involves optimising settings, or whether it's a limitation of Solidcam or one of Mach3.

[Brakeman Bob]

Originally Posted by Eclipze The limitation of the CNC is the maximum acceleration before the machine flexes (only a small machine). So if I stop with a deceleration of 500, it stops perfectly, but the momentum energy dissipates as a little bit of machine flex from the sudden stop. When this happens running the 3D milling code, it produces a shuddering noise around tight corners, though will reach maximum feedrate where straight sections are machined. The shuddering causes slightly more machining marks on the surface of the material.

I think HSM will help a little, but not much as this is a machine dynamics problem and HSM's only contribution would be to smooth out the sharp corners. The only software that I know of and that would be of benefit is OptiPath from VeriCut. This looks at a tool path and then applies a feedrate for every block, effectively hard coding the acc & dec into the machining program. very expensive, especially as you have to buy a seat of VeriCut to enable OptiPath to run.

Is the acc & dec in Mach3 straight line or ramped? If ramping is available, try changing the ramping co-efficient. Or perhaps there is a parameter for changing acc & dec depending on the distsnce to be travelled in the block.

On the ballbar thing, I used to run tests with the ballbar path programmed as G01 interpolation to test acc& dec response.

[Eclipze]

Mach3 has linear trapezodial ramping profiles for each axis, and does not have any other related adjustment. I've played around with different accerations, however there is a point where it slows down the feedrate through corners. When too high, the jerky stepping becomes more pronounced.

Perhaps the problem is related to how the gcode is interpreted. I'm not sure if every CAM software generates the same point to point steps for 3D milling (where no advanced gcode commands are available to improve the trajectory), or whether it is a limitation of the Mach3 software in how it interprets the gcode. Whereby it accelerates to a point, decelerates approaching the same point, then accelerates away from the point. If is were to look ahead and plan the transistion from one point to another, could it be smoother? I guess this statement is suggesting any such "smoothed" transistion between two points implies requires some sort of non-linear curve, which may not be exactly expected. But with a fine enough resolution, it wouldn't necessarily be an issue.

Thanks Brakeman Bob... you've got me thinking in a few directions that might solve this one. Perhaps with the next small 3D milling job, you could help with generating a 3D milling operation so I compare the HSM with Solidcam to see if there is a difference.

[Eclipze]

Problem SOLVED!!!

First I'd like to specifically point out the issue was not with SolidCAM which I had previously questioned. The jerky motion was if fact to do with Mach3.

Mach3 has two motion control modes, Constant Velocity and Exact Stop. This is set under the Config --> General Config. I did have it on constant velocity, but it was acting like exact stop mode. In the Setting tab (Alt-6), there is an option for "CV Feedrate", which was enabled. I turned this off and the difference it quite apparent. I could turn it on and off while air cutting and it's a BIG difference. With it off... very smooth and the indicated feedrate remains at the 1000mm/min. Turn it on and during 3D corners it would erratically slow right down to below 300mm/min.

I would recommend other Mach3 owners consider trying this, as it should improve the cut finish and reduce fatigue/wear on the CNC.

[Brakeman Bob]

Well done mate. Tell me, is this setting something you can turn on and off through the G code like using a Fanuc G10 call? If it isn't, then you might have to separate your 3D stuff from all the rest of your machining to get accurate hole positioning.

[Eclipze]

I'm not sure. I don't have a tool changer anyway, so 3D milling operations are already separated ;-)