Removing cusps along machined XY axis angled contours and radii?

[Anonymous]

Hello all, I recently bought a new Syil X5 CNC machine that runs Mach 3. I have created some calibration components to machine and see what the initial accuracy and ornamental surface finish is like.

The Problem:

Features machined directly along the X or Y axes have an impeccably brilliant surface finish, though, features that are machined simultaneously along the X and Y axes do not. There are large noticeable cusps in these areas. These areas include radii and angled walls (which have various X and Y cardinal influences).

Attempted Solutions, Hypotheses and Results:

Backlash issue along X or Y axes? Not the case. Both axes measured with a Mitutoyo tenths indicator by appropriate metrological protocol. Resulting backlash values of equal to or less than two tenths of a thou (0.0002 inches). Additionally, the respective axes were jogged in incriments of 0.0001 inches from 0 to 0.001 and back to 0 with less than 0.0002 loss. Moreover, the axes were physically pulled/pushed to test for backlash. (Yes, I know this level of performance is rather high for a machine like this). 

Tolerance Issue in Fusion 360 Toolpath? Not likely. At first tolerance was set to a reasonable 0.002 (smoothing disabled during all tests). Things did not change when tolerance was eventually decreased to 0.0001.

Cusps Setting in Fusion 360? No. I tried all combinations including machine cusps (with values set at 0) to no avail. 

Fusion 360 Mach 3 Post Processor Linearization Issue? Does not seem like it. I changed the linearization setting to 0.0001 instead of the default 0.002 and did not notice any changes in the machined work-piece. 

(Pictures Below. Red Indicates Problem Areas, Blue Indicates Good Areas).

Final Finishing Pass. Zero Stock to Leave.3D Roughing. 0.007 Radial Stock to Leave.Red Problem Area. Blue Good Area.Red Problem Area. Blue Good Area.

[HughesTooling]

You didn't leave the toolpath in the file you uploaded but doubt that's the problem. A part made from lines and arc will automatically produce lines and arcs in the g code, for 2d profile tolerance will only apply to splines. Can you upload the file again with your toolpath and also upload the G code. You'll need to rename the g code file with a txt extension. Really you need to look at the machine and settings for this, although the backlash looks OK with no load what about under load, also what about the gibs are they too tight\ too loose?

Mark

[s.noke71]

Turn the settings to 0.001 and turn the smoothing on at the same setting.

If no good it has to be an issue with both axis moving together feedback error and re positioning or something.

Could you try a large dia circle at see what that is like?

[HughesTooling]

@s.noke71  For a part with just lines and arc you do not need smoothing Fusion will automatically produce lines\arcs in the g code.

Here you can see just lines and arcs are generated with smoothing disabled.

Mark

[s.noke71]

It helps on a part i machine

[Anonymous]

Thank you for your sharing your prophetically knowledgeable wisdom. I contacted the manufacturer and they suggested to try changing the acceleration rate of the servos; I did, and to no avail unfortunately. 

Attached one will find the toolpath, a screenshot of the post-processor settings used, and the post-processor files as well.

When I reviewed the g-code it seemed as though there were large "gaps" between specified coordinates. Instead of, say, going from X0.0001 Y0.0001 to X0.0002 Y0.0002 it specifies coordinates like X0.0500 Y0.0500 to X0.1000 Y0.1000. Could this inferred "resolution" of specified coordinates in the g-code be the issue?  Perhaps changing the extension to .nc instead of .tap for better machine understanding? Also, I only changed the tolerances in the post processor to finer values, though, the standard minimum chord length seems to be relatively large at 0.25, maybe this is the culprit?

Regarding gib adjustment: I dont know if this is possible since the machine has linear guide ways and its construction is not of the box-way variety. XY "lock-up" is  a perfectly valid presumption, and it could be the case though considering the machine has relatively large and proper ball-screws and 1HP servo motors as well for its small footprint (they were optional extras) this doesn't seem likely. 

[HughesTooling]

The  " Machining Test G code.txt" file has an adaptive toolpath as the first op. This is all linier moves and is not intended for finishing. How much allowance are you leaving for the finishing 2d contour?

The 2d contour op in the file looks good, just lines and arcs and on it's own will give a good finish. Think you might be roughing too close to the finish size.

S10000 M3
G0 X-0.271 Y0.3525
Z0.6
Z0.2
G1 Z0.0394 F15.
Z-0.2125
G18 G2 X-0.2335 Z-0.25 I0.0375 K0.
G1 X-0.196
G17 G2 X-0.1585 Y0.315 I0. J-0.0375
G1 Y0.069
G3 X0.069 Y-0.1585 I0.2275 J0.
G1 X0.315
G3 X0.4971 Y-0.0831 I0. J0.2575
G1 X0.6051 Y0.0249
X0.7131 Y0.1329
G3 Y0.4971 I-0.1821 J0.1821
G1 X0.4971 Y0.7131
G3 X0.1329 I-0.1821 J-0.1821
G1 X-0.0831 Y0.4971
G3 X-0.1585 Y0.315 I0.1821 J-0.1821
G1 Y0.069
G3 X0.069 Y-0.1585 I0.2275 J0.
G1 X0.315
G3 X0.4971 Y-0.0831 I0. J0.2575
G1 X0.6051 Y0.0249
X0.7131 Y0.1329
G3 Y0.4971 I-0.1821 J0.1821
G1 X0.4971 Y0.7131
G3 X0.1329 I-0.1821 J-0.1821
G1 X-0.0831 Y0.4971
G3 X-0.1585 Y0.315 I0.1821 J-0.1821
G1 Y0.285
G2 X-0.196 Y0.2475 I-0.0375 J0.
G1 X-0.2335
G18 G3 X-0.271 Z-0.2125 I0. K0.0375
G0 Z0.6
G17

Mark 

[Anonymous]

I thought so too, I left .007 radial stock from the roughing adaptive toolpath and later finsihed it with a 2D contour like we see. What I did to save time and get down to the bottom of this was to leave the part in the fixture and come back with updated .tap files with only the 2d contour. Each different 2d contour has less and less stock to leave. I have so far taken off about 0.02 radially with only 2d contours. I think that if there were any cusps or such left from the adaptive roughing op they would have been gone by now. 

I am going to try reducing the feedrate drastically from 15 inches per minute to 3 inches per minute and see how it goes. 

[HughesTooling]

Here's a backplot of your code and all looks good so you need to be looking at your settings in mach or the machine. You can download the backplotter, NC Corrector here. It looks like you have material left by the adaptive so the 2d contour that's all lines and arcs will give a good finish. This code would work fine on my machine. By the way all setting on the post dialog are in mm, the 0.25 min cord means any arc less than 0.25mm is linearized. Some controls will do a full circle if the start and end point are too close, not good if the arc is 100mm diameter but is only 0.2mm long.

Mark

[HughesTooling]

---

@Anonymous wrote:

. Each different 2d contour has greater and greater stock to leave.

---

Have you gone the correct way with stock to leave? You should have a negative amount.

Mark

[Anonymous]

I agree that it must be mach 3 or control related. I will be updating this post and giving credit where it is rightfully due when I hear back from tech support. Thank you Mark for weeding out unlikely problems and being instrumental in the search of a solution. Double thumbs up!

[Anonymous]

My bad I made a typo. I shall correct my response. I am certain it is removing stock. 

[HughesTooling · Accepted solution]

Looks like you are conventional milling, personally I'd always climb mill.

Mark

[Anonymous]

I almost always climb mill. I changed that variable a while back early on in the troubleshooting process to see if it made a difference. 

[Anonymous · Accepted solution]

Problem Solved!

Special thanks to HughesTooling for distilling the many factors involved and nudging things in a great direction. 

Experiment Notes:

The smaller part pictured was also used for test cuts like its bigger counterpart, though, it is smaller since it has had more stock removed than the larger one. The test pieces were never removed from the talon-grips in the vise until completely finished to increase the experiment's fidelity. The only notable parameters modified were the acceleration rate of the servos in Mach 3, tolerance of the 2D contour, stock to leave, end-mill, coolant (or lack thereof) and climb/conventional milling direction. The smaller better-looking finish was obtained WITHOUT coolant. Using coolant would significantly improve surface finish. 

Results & Influential Solutions:

Climb Milling enabled much better looking surface finishes. I always use climb milling but when I initially started experimenting I changed it from the default "climb" to "conventional" in the 2d toolpath and forgot about that until I was reminded by someone far wiser than myself. 

Tooling played a pivotal role in cutting performance, as one would expect. I switched from the larger moderately-worn 3/8 4 flute endmill with a 35 degree helix and 0.001 runout at tool shank to a smaller less-worn 1/8 4 flute endmill with a 45 degree helix with less runout. 

Tolerance 

Servo Acceleration Rate seemed to have helped. Increasing it by two orders of magnitude resulted in less cusps.

Bottom Line: I found that, in my situation, decreasing the tolerances in Fusion 360 and changing settings at the machine control coupled with high quality tool holders and end mills yielded great results. From now on I will get a high quality short gauge-length dedicated shrink-fit toolholder to accommodate a premium dedicated finishing tool with a high number of flutes and an appropriate helix angle for the materials I cut while being sure to use plenty of coolant!