Rowmark Heavy Weights - HDPE panels

Checking-in to see if anyone has had experience routing this amazing sign material. The material is extremely strong and has impressive ratings for weather resistance. However, I am having a difficult time achieving crisp edges on my engravings due to “feathers” left behind by the cutter that are really difficult to remove. The spec sheets on the material suggest slowing the speeds & feeds way down to avoid melting which I have tried without success. I believe my DeWalt 611 on the “1 setting” is still about 16,000 RPM. My cutters are new… end mills work better than v-bits. Has anyone used this material… any suggestions?
Thanks… Don

How many flutes on the vbit? If it’s >1 see if you can find a single flute comparable bit as that will more or less ‘slow’ the cut down further

I recently cut some parts with the xxl.
The feeds and speeds are in the description, and was using a regular old straight flute, router bit. 1/4".
1/4", 2fl, router slotting bit. 19153 rpm 119/59 ipm, feed/plunge. .2" DOC.


Thanks Dan… both my v-bit and end mills are the 2 flute variety. I’d even be happy if I could figure out a way to effectively scrape off the feathers, but they are tenacious!!
I will try your suggestion.

Thanks Jerry… I will admit the outside edges cut using an end mill were better than inner engraving letters for example. And, the end mill did better than a v-bit.
PS… it appears you made some serious chips too!!

1 Like

Hi Don, I have had correct results in HDPE using those settings:

6.35mm square endmill (#201 from Carbide3D) => 12000 RPM + 1250 mm/min

This is for the Makita, for the Dewalt you should put it at min RPM (can’t remember the value) and adjust (increase) the feed rate accordindly

My experience is that “slowing the speeds & feeds” actually means INCREASING the feed rate, since there is a practical lower limit to RPM on our routers on the Shapeoko (even more so on the Dewalt than on the Makita). To avoid melting, and since RPM will be at its min value, the only way to avoid overheating/melting is therefore to move faster.


Hi Julien, I think part of my problem is the Rowmark “Heavy Weights” HDPE is a 3 ply construction with contrasting layers for making signs. Since I cannot slow the DeWalt 611 less than 16000 RPM (or can I?), would I be better of getting a Makita router? In the meantime, I will try your suggestion of increasing the feed rate. Perhaps too, I’ll need to reduce the “depth per pass”?
I appreciate your input.

Its important to increase the feed rate so as to cool and not melt. Its when you feed too slow that the bit stays in one place too long, and melts the plastic.

1 Like

I mill almost exclusively HDPE. Usually I’m around 1 or 2 on the DWP611 speed and I feed about 750mm/min with a two-flute carbide end mill. I find I can do about a 4mm maximum depth cut before I start having rigidity issues, but for roughing a full plunge slot at this speed I get significant chatter in the Y direction, where my SO3 is least rigid. I also opted for the standard size SO3 due to rigidity concerns.

To improve your cut, I would recommend the following:

  1. Play with feeds and speeds while cutting. Be very careful if you do this, but I actually feel the temperature of ejected chips to be sure they’re coming out fairly cool. As several have mentioned, often slowing down rpm or increasing feed can improved this as you’re cutting larger chips, minimizing heat put into the material.
  2. Utilize a 0.01in or 0.1mm finishing pass at full depth. This should cut your hairs off automatically.
  3. If you don’t have it already, I highly recommend buying a high precision collet set from Precise Bits. If you’re using it, the stock collet has high runout which could very well be causing uneven engagement of the cutter.

I believe part of my problem with this material from Rowmark is that it is a hybrid 3 layer HDPE sheet designed for outdoor signs and the cutter may be reacting differently between the surface and the core layers? I did not see your message until I had finished running some tests today with the DeWalt 611 set at 1 (16000 RPM) and the feed cranked all the way to 2500mm/min. It concerned me running it that fast, but there was significant improvement with the feathered edges and my XL did not seem to object… is it safe to drive it that fast? I think the feathers are now manageable with a little steel wool treatment.
I will likely get one of the high precision collets you referenced, but I am wondering if I should just invest in a Makita router that can be run at a much lower RPM?
Thank you.

1 Like

the Makita router goes down to 10.000 RPM, so it may make sense to get one if you’re going to cut a lot of plastic, and considering it is not very expensive.
To go even further down the RPMs, you could consider buying a superPID that will allow you to go down to ~5000RPM with the same router, though it involves a bit of tinkering.

1 Like

I bought a SuperPID expecting this to be an issue for me, but I am able to cut clean edges at high RPM and a much more conservative feed rate than you. I think I’ve seen this material before on playground equipment and I don’t believe there is any difference other than color between the layers, but I guess that could be an issue.

I’d recommend a sharp carbide endmill with a low helix angle… LMT Onsrud makes some excellent ones specifically for cutting plastic. I think far more likely is that there is excessive runout in your spindle, probably due to the collet. If you think for a second what that would do, even with maybe 0.001" runout, you end up with one of the flutes cutting a chunk of the material and the other one unable to follow in it’s same path to extend the cut and clear any chips or hairs created by the prior flute. They have a nice explanation on Precision Bits.


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.