Cutting signs in Rowmark plastic - 1/32” Upcut bit help

Hi there,

I’m hoping you can help. I’ve been reading an article from 1st November 2016 called “CNC engraved instrument panels”

I’m about to start a similar project using the same Rowmark material at 1/16” thickness and a similar 1/32” end mill tool for engraving fine text (I’m using a fish tail end 2 flute bit). The article has been very useful, but i have a few questions that have come from reading it.

I’m aware these tiny bits are extremely fragile and so I’m aware I need to get my cutting and feed speeds right as well as the depth of pass too. I’m fairly new to the world of CNC so I’m struggling to find out how work these out. I’m aware I have to bare in mind chip load but I am a bit lost in calculating any speeds.

Any help would be much appreciated.

Many thanks


These are the bits I am using

Keep RPM low, try to use single flute bits and go fast.

Since you wont be deep in material you dont need bits with long flutes.
The V-bits you show should be nice, they are strong.

I cut Rowmark etc with V-bits regularely at 1500mm/min @ 10k RPM
Depth 1mm/pass

If I were to use a 1mm 1F end mill I would calculate for chipload and go full depth per pass.

Chip thickness in mm * RPM * Number of flutes = Feed rate in mm/min
Example : 0.025mm * 16000 * 1 = 400mm/min

Note that chip thickness need to include runout/tool deflection and chatter.

Thanks for your response.

I’m only going to be cutting about 0.2/0.3mm deep in order to remove the top colour. I tried using a 60 degree tool initially which was too big for this small text (most noticeable in the edges/corners), but it also left a poor finish at the bottom of the cut. I used Easels recommended settings for that. I think with using the v bits I have to cut slightly deeper than required as struggles to remove the top layer with the fine point. That was my thought process for going to the Upcut bits (also based on the linked article in my original post). Very new to this so happy to have any information that will help with these cuts.

How can I find the the chip load? Is this something I can request from the manufacturer?

Chip load / thickness is for the most part only available from reputable mfgrs but one can often use similar values for generic brands / unspecified end mills.

I use this one:

V-bits as you have experienced dont provide a good “floor” finish. V-bits can also provide issues shwoing in your picture, a “dog-bone” corner of the letters. This is probably because the V-bit used have a minute flat spot causing the bit to go a minute step to deep.

A 1mm 1F end mill would be my go-to bit for plastic engraving provided the design isnt too small or intricate.
A 3-5mm flute length is all that is required.

I use 1/32" bits with settings as follows: FR:680 PR:304.8 DPP: 0.2 and have had fantastic results on Rowmark. Hope this helps.

I’ve done alot of these types of faceplates for amps. I typically use 1/32 or one of these v-bits if there are finer details.


Great, thanks for all the replies - they’re really helpful.

I’ve now run a few cuts and the 1/32” bits are engraving with some really nice detail. The flat point v-bits look great I will try them out. Are they what you used for the amp faceplate @MechanicalGoose - I have some switch panels to make which are very similar in design to that. What software are you using to design those?

One problem I am coming across now is the top red layer I’m cutting is getting caught on the cutting bit. It doesn’t seem to be affecting the cut, but I just wondered whether it could be an indication a speed may be too high or low or not enough depth of cut.

Also, the Rowmark I’m using has a 3M adhesive backing on it ready for sticking the signs I’m making up. The signs are 150mm x 75mm. Do you think I’m better off cutting these out to size first and then engraving them. The bonus of cutting to size first I can see is there’s quite a lot of flex in the large sheets so the Upcut bits are definitely trying to lift the material which is difficult to control in the large sizes.

I don’t particularly want to cut them out with the 1/32” bit as I want to save the life in those small bits. I was thinking of using a straight cut bit to cut the signs out and a v-bit the bevel the edge. If I engrave first I struggle to locate the tool in the same home position after changing the bit as they different sizes etc… I suppose this would be easier if a ran the project all from XYZ 0 as that way it’s a fixed position for all the tools.


I make a few of these cake toppers from 1,6mm single color Rowmark, usually by a 30deg V-bit. I use the same bit for cut out and also for design elements.

Large, thin sheet need good support/hold-down otherwise they will lift when using upcut bits. I use masking tape and cyanoacrylate (CA) glue to temporarely bond the sheet down. Cutting everyhting out from a large sheet is worth while time-wise as there will be no need to replace precut stock, change bits etc.

Another “trick” I use is to make the cut-out in two stages, first stage with incremental depth (two passes for full depth) then a final stage where I run the same path but at full depth only. This clean out most of any “fuzzies” left from the first stage.

Using a 30deg V-bit I run 1400-1600mm/min @ 10k RPM

1 Like

Yes I use either the downcut 1/32 or the vbit i linked. I design everything in Illustrator.

The sheets I carve don’t have pre-installed adhesive but I use adhesive tape to hold the plastic down while I cut to avoid using clamps.

Another thing that might help is upping the speed of the Dewalt. The smaller the bit, the slower the tip speed. So for things like this I run it at #2.