V-Grooving in High-Density Polyethylene (HDPE)

Advice on tool choice and toolpaths to cut clean grooves in HDPE material with minimal melting and re-welding problems. August 31, 2009

Question
I want to use my v-cutter to route a shallow (2mm/3mm deep) pattern into the surface of 3/4 starboard. Test pieces in MDF are coming out excellent but results in Starboard (plastic) are bad (re-melting). Any recommendations on rotations and feed speeds?

Forum Responses
(CNC Forum)
From contributor T:
Can you try this in two passes? The second being .010 depth of cut?


From contributor B:
Starboard material is very similar to other dense plastics like UHMW. Wood bits do not work well in plastic. You want a the speed of your cutter to be between 600 to 1800 feet per minute (these are recommended speeds). If you have a 1/2" cutter, you are going to want to run it around 3 to 9 thousand rpm. Your feed rate is .01 inches per revolution.

I have machined a lot of plastic. If you are cutting a pocket or a groove like you are describing, you will get a lot of melting in dense plastic. I would suggest that you use some sort of misting. In the application that you are describing I will typically use a mill instead of a router. However, if you mist the part it will help prevent melting. Misters can be bought for routers.

Lastly you want to use a plastic bit and if you don’t have the profile you can also use bits for aluminum and soft metals. Do not use a wood bit. Sometimes you can get away with a wood cutter when you are profiling but when you are cutting a pocket or something that does not go all the way through it will not cut well.


From contributor G:

Starboard is pretty easy to cut. But, don't use either a bit specific to wood or a bit that has seen wood. A v groove cutter, solid carbide or carbide tipped should work fine. I’m not sure about the feeds and speeds mentioned. I think theoretically they are fine, but I've never run starboard anywhere near those numbers (always faster rpm, slower feedrates).

Now, the one area that you may need to work on is the tip of the bit. Starboard won't turn to dust like MDF and because the speed of the blade at a sharp point approaches zero, the wider the flat on the bottom (or have the bit ground with a bit of a ball end), the better. I wouldn't say I see a lot of melt, but a little melt can keep some chips in the groove, otherwise just try a new or different bit. Starboard is HDPE and a fair bit easier to cut than UHMW.


From contributor M:
The problem is the tool you are trying to use. There is not enough rim speed at the tip of the tool to effectively cut and eject the chips. We recently did a job very similar here. We had to make hundreds of 1/8" deep v-grooves in MDF, HDF and Starboard. The solution to the problem was having a v-groove blade made for us. We then mounted it to our horizontal aggregate and got absolutely flawless grooves on all parts.

From contributor M:
I should also add that it was a 5" dia. 6 wing cutter that we had made for that.

From contributor J:
When cutting any material using a v bit that is not an insert style you will typically get melting in plastics and you cannot avoid this to a point. The reason is the v bit you use based on solid carbide design will have a zero RPM at the center of the bit and will melt or drag due to no cutting edge.

From the original questioner:
The solution to use the aggregate is great for straight groves. As soon as you have non-straight lines to follow it only works with a C-axes (I don't have) and a lot of programming to compensate the offset of the tool. Creating text would be very cumbersome.

For straight lines it would also be possible to have a tool made utilizing the onboard grooving saw instead of an aggregate (even more limited in direction). The tool I am using is an insert type tool and I might try to get one with a flattened or rounded point if that would help. I am not creating a v-groove for folding, but just some patterns to make some parts slip resistant. I wonder what many of the sign makers are doing. They seem to do a lot of lettering by routing into all kind of plastic materials. The best result so far (using the insert tool V with 92deg.) is at 5000mm/min (~200"/min) and 18,000 RPM.


From contributor M:
I have done text lettering in Acrylic with a miterfolding bit. The first try made a mess of it with re-welding of chips, etc, but by using a fresh sharp cutter and making a cleanup pass of a few thousandths the lettering came out nice. I wish I had saved or could remember what the feeds and speeds were, but I can't seem to find them. A little experimentation should get you there pretty quick though.

I appreciate the zero velocity at the tip being a problem, but good results are possible. Onsrud makes some engraving tools with a flat on the point as you describe. I think they are made to do lettering and engraving with a land at the bottom of each letter rather than to specifically address the zero velocity at tip issue, but they may be worth a try as well. Take a look at the 37-00 to 37-20 series.

Related Articles