Milling Type 1 Grey PVC

[jsummers]

Hi,

We're milling rough surfaces--i.e. things that looks like an ocean bottom or a moutain range--in blocks of Type 1 Grey PVC with precision down to 1mm (0.04 in). We've finally got CAM algorthims that will generate reasonable rough and finish tool paths and have figured out speeds and feeds for our flat and ball end mills (sizes down to 0.01 in, to handle the deep valleys). But we have a few problems that I'm hoping some of you folks with more milling experience might have some insight about.

1) Our final surface tends to have some flat areas where extra material has been removed during the cutting. I've tracked this down to large chips fracturing off during the roughing passes (due, I assume, to the shear strength of the material being exceeded). The cut quality is good otherwise and the speed and feed didn't cause this at all when test cutting. Could the plunge roughing be the source of the problem?

2) The finished surfaces seem to have greater detail on the peaks than in the valleys. It seems to me that if the CAM was working it would cut everything with unifrom detail. Could the mill be removing too much material in some of the semifinish passes so that the finish pass just air cuts in some areas? Most of the CAM software is designed for metal, which is suspect is generally much more ductile than the PVC we are using.

3) What are people using as a coolant for plastics milling? We use a Arizona Vortex CoolTool now. It certainly cools the air, but the claimed 100 deg. drop seems a bit of stretch judging from our system (running at 90 psi just before a particulate filter). Is this going to be enough cooling for 4 ft. by 4 ft. surfaces and 12+ hours of continuous cutting?

Thanks,

Jason

[billp]

Jason,
Many CAM programs let YOU decide how much material to take off on your roughing passes. You might want to try and give yourself a larger allowance ( OR leave more material on ..) before you begin a finishing pass. Plunge roughing shouldn't chop off pieces unless your plunge rates are excessive. If it's happening in the actual cutting process you might even have too large a bit for the purpose at hand.
Can you give more info on your bit sizes, feed speeds, and software used to generate the toolpaths?

[jsummers]

Bill,

Thanks for the information. I haven't used plunge roughing previously, so maybe these feed rates in z (that I listed below) are too high. The amount of material removed with each pass is usually pretty conservative. I'm having these problems on a surface with a maximum relief depth of about 1 in. that I cut with

1) a constant-z plunge roughing path that creates about 5 terraced layers using a 1/2 in. flat end mill

2) a second roughing routine that uses a 1/4 in. flat end mill to clean up and add some additional layers in tight spots

3) 3 rastered finish passes with ball end mills 3/8, 1/8, and 0.055

We're trying out CAM programs now with these initial trial cuts. This first was generated by Delcam PowerMill, though not with me as the user since we just received some cut files to test how well the software works for these kinds of rough surfaces. I also plan to test MasterCAM and VisualMill. VisualMill is the only software that I will actually be the operator for.

Right now we are using Onsrud carbide plastic-cutting mills for all of the flat end mills and the larger size ball end mills and 2 flute Robb Jack carbide cutters for the smaller size ball end mills (<1/8 in).

For larger mills I am using 10000 rpm on our Porter Cable Router and for the smaller cutters (<1/8 in) I use 25000 rpm.

The ball-end mills are

CED (in) x-y feed (ipm) z feed (ipm) CEL (in)
1/2 111 28 9/8
3/8 111 28 9/8
1/4 111 28 7/8
3/16 111 28 3/4
1/8 111 28 1/2
0.055 52 13 0.0825
0.04 38 9.5 0.06

The flat-end mills are

CED (in) x-y feed (ipm) z feed (ipm) CEL (in)
1/2 111 28 9/8
3/8 111 28 1
1/4 111 28 3/4


Does that seem reasonable?

Thanks,

Jason

[kerrazy]

your feed and speeds are to quick. Which is in turn causing the tool to overcut the part.

try 60 ipm feed rate and 39ipm plunge rate.
Also set your your rpm to 13000, and leave it there for all cutters in this material.
what is your stepdown, or depth of cut on each pass for the 1/2 inch end mills, you could go as deep as .25 for each pass.

Good luck, Dale

[kerrazy]

I would use only ball mills on this as well. Unless you really need tight 90 degree shoulders, this may reduce some cutting time.

I would probably hog out the material with a few roughing passes with the 1/2 inch ball mill, and then use the 1/8 inch ballm ill to clean it all up leaving enough material for a final finishing pass.

[jsummers]

Dale,

Thanks. I'll try the slower feed rate in x-y.

I just tried a rough cut that rastered across the surface at fixed z height: no problems with chipping. I'll have to wait for the final finish pass to evaluate the overall quality.

I'm a little confused about using a ball end mill for roughing though--aren't flat end mills the standard?

js

[kerrazy]

I prefer a ball mill, when doing relief work. If it is flat work I use a flat tool.

It is more forgiving in corners and such.
Dale