Newbie- how to improve surface quality?

[davidsutton]

I am cutting 3d spheres (100mm dia) from stl files in machineable wax.
The toolpath is being generated in a program called maquette volume.
For the finish toolpath I am using a 3mm ballnose at 0.4mm increments cutting in a paralell fashion along the x axis.
My machine is a 3 axis isel with servos.

The surface quality is too stepped or ridged -any ideas about how to get the best finish?

1. If I use a different CAM software (say mastercam) to generate the toolpath - would this improve the surface quality?

2. If I use a 1mm cutting tool at say 0.5mm increments would this improve the surface quality - or would it be better to go for a larger dia cutting tool?

3. Is the paralell toolpath the problem - would I be better off trying a contour cut for example?

4. Any ideas about 'coating' the cut piece of wax in anything - i.e fix the surface quality in post processing?

Any help would be appreciated!!!!
The models will always be from stl files rather than true cad surfaces.

[Harri J]

Hi David,

Some quick answers to your questions:

CAM systems break up arcs into tiny moves - the more moves, the better the tolerance in respect to a true sphere. So the stepover and tolerance settings (don't know yuor software, may or may not have them) will have a tremendous effect on the finish.

Choose the largest possible ball nosed tool your machine can run, this will give your smaller scallops with the same toolpath settings. If you need a really fine finish you might like to check tool runout too. Think of it this way, you are cutting a series of trenches, the larger the tool the flatter the trench.
(The 1mm tool would give an awful finish so you can forget that.)

Sometimes the original file can be the problem, you might need to check the settings on the stl side too.

If you know any gcode it is the perfect solution .. just a few lines of code and you have a parametric program that will give you perfect spherical surfaces and control over finish quality. Assuming your machine supports parametric programming...

Cheers,
Harri

[ironDigit]

did you already try adjusting feeds and rpm's?

good luck

[ger21]

A larger tool will give a smoother finish, if you keep the stepover the same.

[Andre' B]

Haas has some tips on 3D surfacing here. http://www.haascnc.com/solutions_3D.asp

The thing about a sphere is you want to use water line type of programming around the equator but near the poles that will get you some nasty steps. If you use a step over pattern you get just the opposite.
But since a sphere is very easy to describe with an equation a macro type program is easy to write.

Here is something I have been playing with for cutting spherical surfaces, but have not used it on a job yet. It steps around the sphere with an angular step which avoids the above problems.
Sorry but it is in inches.

If you control does not do macro B you may consider getting a seat of NCPlot, it has a macro translation feature which will take a program like this and output it as a much longer simple gcode program.

By changing the values assigned to the variables it is possible to do many different types of cuts. As shown (first pic and the code) it does an external surface starting at the top pole and cutting around to 10 degrees below the equator. To do this cut you would need a ball type cutter that can do a 10° undercut. The step angle is 2° mostly so the picture is not just a blob of circles you would make it smaller for a real finish cut.

The second pic was done by changing #2 to -0.1875 and #4 to 80.0 and #5 to 180.0, note that the work offset is at the center of the sphere and the tool length offset is to the center of the ball end mill and not the end. This is not normal practice but it makes the programming easier.

#1=3.0(RADIUS TO CUT)
#2=0.1875(RADIUS OF BALL EM)
         (+ IF DOING AN EXTERNAL SURFACE)
         (- IF DOING AN INTERNAL SURFACE)
#3=2.0(STEP ANGLE)
#4=0.0(START ANGLE)
#5=100.0(END ANGLE)
#6=30.0(FEED RATE)
#7=10.0(PLUNGE FEED)
#8=0.0(X OFFSET FOR DISK CUTTER)
#9=0.2(BACKOFF)
(**************************)
(* YOU SHOULD NOT NEED TO *)
(* EDIT BELOW THIS POINT  *)
(**************************)
#8=ABS[#8]/#2*ABS[#2]
#9=ABS[#9]/#2*ABS[#2]
#18=[#1+#2]
#19=#4
#24=[#18*SIN[#19]]
#26=[#18*COS[#19]]
#14=[#9*SIN[#19]]
#16=[#9*COS[#19]]
G0G54X[#24+#14+#8]Y0.0Z[#26+#16+1.0]
WHILE[#19LT#5]DO1
#24=[#18*SIN[#19]]
#26=[#18*COS[#19]]
#14=[#9*SIN[#19]]
#16=[#9*COS[#19]]
G1X[#24+#14+#8]Z[#26+#16]F#6
G1X[#24+#8]Z[#26]F#7
#24=RND[#24*1000]/1000
IF[#24LE0.0]GOTO9
(MAKE CIRCLE)
G3I[-[#24+#8]]F#6
N9
#19=#19+#3
G1X[#24+#14+#8]Z[#26+#16]F#6
END1
(MAKE LAST PASS)
#19=#5
#24=[#18*SIN[#19]]
#26=[#18*COS[#19]]
#14=[#9*SIN[#19]]
#16=[#9*COS[#19]]
G1X[#24+#14+#8]Z[#26+#16]F#6
G1X[#24+#8]Z[#26]F#7
#24=RND[#24*1000]/1000
IF[#24LE0.0]GOTO19
(MAKE CIRCLE)
G3I[-[#24+#8]]F#6
N19
G1X[#24+#14+#8]Z[#26+#16]F#6

IF[#2LT0.0]GOTO20
G0X[#18+#8+#9]
GOTO21
N20
G1X0.0F#6
N21
G0Z[#18+#9]