Feeds and speeds for lexan

What are the feeds and speeds for lexan that your teams use? And where is a reliable place to search for more information on feeds and speeds for different materials? We are trying to cut an intake on our schools new Cnc as practice.

What is the RPM cap of your CNC? Is it a router, a mill, etc? What kind of bits do you currently have? There are a lot more things to consider before a decent answer can be given.

For instance, on our CNC router, we cut at 18,000 RPM, use an 1/4" O’ flute bit that’s designed to cut hard plastics, and using the manufacturer specs, cut at 108 inches per minute, and typically between .060" and .100" depth of cut.

1 Like

I am not sure what the RPM cap is right now but here is the link to where we got it which has more information: http://www.cncrouterparts.com/pro4896-4-x-8-cnc-router-kit-p-253.html
It is a CNC router. As for Bits we just got the machine so we dont have too many we have a 1/2in flat endmill 3 flute and a 1/4in drill bit but we are open to recommendations for more bits as we are willing to purchase whatever bits we need.

Thanks that was very helpful

There are a lot of inexpensive bits on the market at this point, like the ones from Ozzy Boards

We use Vortex Tool and they have a really good life and are designed around plastic.


They also have aluminum versions (they have an A after the part number, so like a 5730H would become a 5730A). We find they last quite a while in a production environment, and can be substituted in a pinch if needed.

Also, the router kit you linked to does not have a spindle, and having that knowledge is pretty critical, and lists 2 different kits for how fast of a movement it can make. Both of which are faster than you likely will run, unless you are running plywood and a multiflute bit.

This is extremely helpful to us… thanks for all your help

I’ll try to get back to you on the spindle but our Eng Tech teacher isn’t here today so I am not sure what spindle we are using currently


Depending on the CAM platform you are using, you can set parameters, to give you what you need as well.

Many people find G Wizard to be a useful guide for feeds and speeds in various materials.

Some bit manufacturers offer good recommendations on feeds and speeds for their bits. Here is an example from Onsrud for hard plastics.

As many have responded, it will be important to understand the RPM range your spindle is capable of and an idea of the rigidity of the machine. In general, it’s a good idea to start with the less aggressive end of the settings from something like G Wizard or manufacturer recommendations and increase as you verify that your machine can handle it. You can also start with a shallow depth of cut and increase it as you find what your machine and bit can handle.

For routers which usually want to run above 10000 rpm and are happier at 15000 or more, you will almost always want to use single flute bits so you can get reasonable chip loads with reasonable feed rate. Three flute bits are more appropriate for mills with much lower rpm.

When cutting plastics, it tends to be better to use conventional cutting rotation rather than climb cutting rotation. Climb is definitely better for aluminum. The curled chips produced by conventional are better for plastic cutting than the chunky chips from climb. You can try both ways, but be sure to at least try conventional.

While you could possibly practice cutting with your 1/2" three flute endmill, it would probably be a much better idea to take the time to get a much smaller single flute upcut bit and start with that. I’d recommend something in the range of 4 mm to 1/4". Starting with a known high quality bit like an Onsrud 63-769 and getting a feel for the capability of your machine and then possibly moving to lower-cost decent generic single flute bits like those sold by WCP, those sold by Ozzy Boards, or imported Huhao bits might be a good strategy.

Chances are that you will be able to successfully cut polycarb with a single flute bit in the 4 mm to 1/4" range with feeds in the 60-120 ipm range, 15-20K rpm range (assuming that’s possible with your spindle), and depth of cut from 1/16" through one bit diameter. I wouldn’t start with 120 ipm, 20K, 1D DOC, but you might be able to get there.