Erratic Feedrate When Cutting Spline Lines

[david.quayle]

Ivé had this issue both times I have cut something when the original Fusion Sketch was drawn with Spline Lines. The issue being, the Feedrate changes a lot during the cut. When the cutter is cutting the peaks of the knobs shown in the attached image it runs at the correct feedrate, when the cutter gets half way into the valleys, the feedrate slows to about 1/5 of the set feedrate and jerks forward until it is half way out of the valley and then it speeds up again, repeating this over and over as it goes around. Very annoying

Does anyone know what might cause this erratic behaviour, if anything I thought it might slow down on the tighter peaks?

At this stage I dont know much about code and rely on Fusion Cam to do it for me. I have just had a look at the code and there are sections throughout that look odd to me, see below, maybe you can tell me whats going on.

[amcfarlen]

From the brief description it sounds like the CNC controller (Mach3 perhaps) is struggling with the look ahead trajectory and stops and starts trying to cut the curves.

The G-Code that is generated by Fusion will be very accuratet, but can make some programs quite long. Depending on your machine and controller it may struggle.

One thing to try is to turn "Smoothing" on in the Passes tab. Depending on the complexity of the part and choice of machining path, it can significantly shorten the code. This helped me with some programs that were almost impossible to run.

However I had one last week that no matter what Mach3 would not cut what should have been some nice smooth sweeps at speed. I've managed to installed and configure Mach4 that has a much better trajectory management and the part cuts perfectly at speed.

[david.quayle]

Thanks for the reply.

I am using Mach4. I don’t think it is the processing speed, could be wrong though 🙂

I tried the Smoothing as suggested and also made the tolerance bigger, the code went from 10000 lines to 2000 lines. If I draw a similar shape just using arcs the code is only about 200 lines.

I tweaked the Constant Velocity angle speeds and the combo of that ans Smoothing made it better but far from perfect. Fusion Cam seems to be able to deal with some parts of the Spline using arc code but other part are lots of straight lines and that’s where the movement is at it’s roughest.

Are you using Constant Velocity? If you are what Feedrates are you using in each angle?

Are you inches or Metric J

[LibertyMachine]

Smoothing is going to be your answer. 

What do you have your tolerance and smoothing set to? This is found on the "Passes" tab

[amcfarlen]

Yes. I use constant velocity and work in metric. The file that I couldn't cut in Mach3 has no problems in Mach4 was to build a mould for a concert ukulele. There are no straight lines in that file. All curves made up of one single spline per side with 6 control points. Feed rate is at 3000mm/min. 

[david.quayle]

I changed the tolerance from 0.01 to 0.1.

The section of the cut where Fusion CAM creates lots of short lines looks just like an Arc, so why it creates all the short line is beyond me.

I thought I'd outsmart the program but using the Spline on the peaks (which cuts fine because it uses Arc's in the code) and then an actual arc in the valley's but of course Fusion then refused to generate a toolpath !!!

[david.quayle]

I know it depends on the machines capability but I would be interested to know what speeds you have entered in to the CV angles.

[amcfarlen]

Not sure where I'd look for that. My speed is set at 3000mm/min and smoothing is at 0.01 and it cuts just fine in Mach4 at that speed, but in Mach3 it just stutters and stops in all the deep curves. Works as expected in the longer more relaxed curves.

[david.quayle]

I'm no expert but here goes;

The CV Angle Feedrates are accessed by opening the Wizard TAB at the top of the Main screen, then you will get to choose the Wizard you want from the Menu as per the attached. When you open the CV_Feedrate selection it will give you the CV Angle Feedrate Table like shown in the attached. The theory I have been given is that if 0 is entered into all of the Angles it works just like Exact Stop and stops before changing direction, although I'm not sure that's how it behaved in my case, I need to go back and test (one day maybe)

If you want to speed things up, you make sure CV is on, and then enter speeds into the angles. What happens is, as the cutter get close to an angle change, it slows the feedrate but doesn't stop in the corner, as soon as you move away from Exact Stop, you start to get deviation in the corners which can range from minuscule to substantial depending on the speed/acceleration and your machines physics.

If you have a look in yuor CV_Feedrate table please let me know if "179"is entered into Angle 0, mine had 179 in 0 and the rest were 0

There are other tolerances that affect speed etc but I'm still trying to get my head around those.

[amcfarlen]

That's the first time I've seen that box in the Wizards Section. Never look there 'cause I don't use them. 

When I checked it says  CV turned off, and everything is set to 0. Just as I suppose it would be from the initial install.

In my main Mach4 Config Screen I have Use CV ticked. 

[david.quayle]

Im as sure as I can be that if you turn CV on in the wizard, and then enter speeds into the wizard angles you can probably improve your cutting time by quite a bit. theoreticaly your cutters should last longer as well. 0 degrees is a straight line and 179 degrees is the cutter turning back on itself (less 1 degree of course). If you enter faster speeds into the lower angles, as fast as your comfortable with, and slower speeds into the higher angles (I will use 0 for a lot of the higher angles) then the whole show should run better.

[david.quayle]

I have tested Mach4 with Constant Velocity turned on and appropriate feedrates entered into the Wizard, now the curve cutting I was having issues with is as smooth as silk, well almost. It’s a vast improvement for sure.

There is a new Wizards available which helps with entering the Feedrates. If your interested they are at, https://www.machsupport.com/forum/index.php/topic,35649.msg244192.html#msg244192 the downloads are in Reply (post) 31