Colorcore hdpe finish quality issue

Materials Plastic
1

I recently completed my first project using Colorcore hdpe. After conducting numerous test cuts to evaluate cut finish quality (primarily the flat horizontal black surfaces), I selected a 60 degree V bit and a Y direction raster tool path for the job. This produced the best surface finish, which was defined as minimal tool marks and a shiny black finish.

When I ran the full project cut, the final result was pretty decent however there were some noticeable tool marks and a gouge in one region (labeled with a red arrow in plot below). My tool path information is shown in the plots below.

I have some questions. Any idea on what could have caused the gouge? The cut was supposed to be constant depth. Does anyone have any suggestions to reduce or eliminate the tool marks (different bit(s), speeds/feeds, etc)?

Here is some additional information regarding the job:

  • Workpiece was attached to spoilboard using blue tape/CA glue. A checkerboard tape/glue pattern was used.
  • RPM: used value recommended by King Plastic
  • Feed: used value recommended by King Plastic
  • Depth of cut: less than max value recommended by King Plastic

image
image633Ă—723 84.4 KB

image
image261Ă—677 14.3 KB

image
image588Ă—528 15.3 KB

1 Like
2

Foghorn,
Personally, I would consider a really thin pour of epoxy colored appropriately into the carved area and not be concerned on finessing the cut. It would be much faster and easier too.

1 Like
3

Thanks for the suggestion.

4

Not sure exactly, could be one or more of a few things including loose bit, lost steps with the Z-axis, or the material shifted on the bed.

Only use a V-bit for the edges of pockets, not for the inside (field) removal. I noticed your stepover for the V-bit was 2% which I imagine not only took forever to cut, but the sharp point of the V-bit is not designed for smooth, flat, surface finishing. It’s more of a form or shaping tool. I suggest switching to a V-Carve toolpath and use either a 1/4" or 1/8" flat end mill for a clearance tool. Then let the V-Bit do the edges where it works the best.

When using end mills, if I want as smooth surface as possible (i.e. less sanding), I will set the stepover for the bit to between 8 and 10 percent. Going over 10 may not be enough (sometimes it is), and I have seen diminishing returns using less than 8 or 9 percent versus the amount of time required for the carving itself.

Regarding speeds and feeds, its not easy to recommend anything specific. However, IMHO, 150 in/m and 22k RPM is somewhat high for a V-bit. With plastic (acrylic) you can’t go too fast or you will heat up and melt the material and possibly clog the flutes with this melted material. And, without getting into unnecessarily complicated chipload math, IN GENERAL the more flutes you add to the equation, the slower your bit needs to rotate and feed (relative and compared to the same size bit with less flutes) so as not to clog the flutes with material that doesn’t have time to be evacuated. Again, this is a very general statement and can change depending on material and the machine your using. Just to note, they make single-flute O-bit end mills just for plastics and foam.

So, in summary, I’ll throw out these numbers as a STARTING point if it was me doing the cutting and using a V-Carve toolpath. Also, make sure to double-check the bit is secure in the router and won’t slip.

1/4" 3 flute end mill for a clearance tool. 3 flutes is what I think is most common in use
80 in/m feed
40 in/m plunge
18k RPM
10% stepover

60 degree V-bit
40 in/m feed
20 in/m plunge
16k RPM
25% stepover (since only used for edges of pocket)

If the edges of the pocket are angled too much or the corners are not sharp enough, then switch to a 30 degree V-bit keeping same speeds.

2 Likes
5

Thanks for the detailed response. I used the vbit speed and feed recommended by the plastic supplier. Melting or flute clogging were not observed.

I initially started with a 1/8 single O flute up cut end mill. This produced a dull finish on the black surfaces. The plastic supplier said that this is less likely to occur with a vbit which is why I switched.

I might test the end mill/vbit combo approach.

I was also wondering if running a finishing pass on the horizontal sufaces with a smaller end mill, say 1/16, might produce a more glossy finish like the vbit did.

Thanks again for the feedback.

1 Like
6

Nice explanation. Are the feeds/speeds 80/18K/10% for plastic or wood?

7

Well first, it’s a little hard to tell from your overhead photo, but it doesn’t look like the V-bit produced very much of a glossy finish? All I see is what looks like a material with a yellow colored plastic surface and some type of wood (MDF, MDO etc) beneath that surface which has been exposed. And, this sub-surface appears marred with not just the noted gouge but circular and linear marks.

With that said, only a Profile toolpath allows for a “last pass” option. And, if not mistaken, is used to prevent things like horizontal banding from wood carvings, or overall surface finish on the edges of aluminum, brass, and other metals. Noting, the last pass operation simply performs a full cut depth pass in one single pass, just at a tiny amount for the DOC. Also, I don’t think you’re going to get consistent results if you try to perform a last pass manually by specifying two separate toolpaths. You might give it a try, but I’ve never heard of trying that or done so myself. At that point, you may want to revert to sanding or re-surfacing this sub-surface material with something like epoxy as mentioned earlier by Jim.

1 Like
8

Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.

If I was going for the best finish here I’d look for a corner radius / bull-nose (not ball-nose). That will get rid of the sharp corner in the “V” and fish-tail/flat tooling. Typically you can also use a larger stepover than with a ball-nose and get a smooth cut. Up-cut would be preferable as a down-cut will effect the floor finish.

A few other things from this thread. RPM and feed-wise functionally comes down to surface speed, shear, and chipload.

    RPM
      Higher RPM is fine as long as give it enough feed to have at least the minimum chipload to cut and not rub/grind the material. There is a limit to the amount of surface speed (RPM) before it effects the cut. It depends on the tool geometry and diameter though. Conservatively if you stuck to around 1200 SFM your max RPM would be 30K for 1/8", 15K for 1/4" and 7.6K for 1/2". This is the cutting diameter so you'd have to calculate it for a "V" cutter.

      You will also pickup more shear force the higher the RPM which can help with soft materials. The flip side is that you also pickup slightly more heat. Although, that amount is very minor compared to too small of a chipload.

    Chipload

      For something like HDPE I'd want to hit no less than a 0.002" chipload, I'd probably start at double that if the cutter is over 1/8". You can go a LOT higher than that depending on the tool and the rest of your cut settings though. The idea here is that you need a minimum size chip to support itself during the cut and the greater that sized chip the more material you are sinking the heat into as the majority of the heat comes from forming the chip (assuming that you are not rubbing).

      So for feed chipload * flutes * RPM. e.g. 0.002" chipload on a 2 flute cutter running 20KRPM would be 80IPM (0.002 * 2 * 20,000).

Can’t tell from your picture but is the gouge just a line or does the entire cut get deeper after that? If it’s the entire cut after then most likely you bit slipped in the collet. If it’s just a line that’s deeper than you have another issue.

One final thing. You have that cutter programed wrong. At least according to what I can find for that cutter it has a 1/32" flat. That means that it should be entered as an engraving tool with the flat. Using it as a “V” will effect the size of the top cut width from both a “missing” part of the cutter tip and a change in the growth of the tool.

Hope that’s useful. Let me know if there’s something I can help with.

1 Like
9

Thank you very much for the information John.

10

I can’t speak to the anomaly that caused the gouge, but I would recommend using a normal square end bit (as large as the part geometry will allow), and do a finish chamfer cut. That’s my normal mode of workflow when cutting colorcore. This sign was done with a 1/8" bit and chamfered with a 45 deg. chamfer bit. I usually cut this material .080" deep (one pass).

PXL_20220404_150340488 (1)
PXL_20220404_150340488 (1)1920Ă—2560 319 KB

1 Like
11

Thanks for the feedback Bill.

12

Bill, Can I ask what feeds/speeds are you using for a starting point?. I plan on using Spec o-flute bits and as you know the stuff isn’t cheap so looking for a starting point.

13

Honestly Dean, this stuff is so easy to work with I never gave specific feeds & speeds a thought. Being an old-school manual machinist, everything was run by the seat-of-my-pants, so to speak. And this carried over into my CNC. My default feedrate for a 4-flute 1/8" endmill is 30 ipm at about 8-10k RPM (I usually run everything conservatively). When I cut to depth to expose the core color, I cut .080" (single pass DOC). When I cut address signs, I have actually cut thru 1/4" material in one pass.

I think your 0-flute cutter should work quite well for you, as it will clear out chips more effectively than my 4-flute. You can adjust RPM & feed-rate on-the-fly. And as long as you’re not overloading the cutter with too fast of a feed rate, this stuff will cut fine for you.

I apologize that I can’t give you a more technically astute response, but in reality, cutting this stuff is so user-friendly that you almost can’t go wrong with reasonable speed/feed rates.

2 Likes
14

There are some CNC related documents on this web page: https://www.kingplastic.com/products/king-colorcore/

1 Like
15

Thanks Bill, I probably should see if Spec has a tool DB as well, it may already be covered in that…

1 Like