Novanite - Has anyone worked with this material?

[BruceH]

I just got in a sample of a material from Mexican manufacturer Plastiglas, called Novanite. The stuff feels very hard like ceramic to the touch, seems brittle (chipped edges from shipping), and is very dense (as heavy as aluminum), yet I can easily shave off thin filings from the edge with a razor knife. Does this sound like any material any of you have worked with before? As a neophite Shopbot operator, I have no idea where to start with bit choice, feeds or speeds. Any input would be appreciated.

[Brady Watson]

It's a generic version of Corian.

Start cutting @ 13,000 RPM; MS,1.5,0.7 and see what the machine tells you. Increase speed or RPM as necessary. RAMP-Plunge into the cut - not straight down. Keep pass depths conservative at first until you are comfortable going deeper.

2-flute upcut/end mill will work or visit Onsrud for solid surface specific tooling.

-B

[Kyle Stapleton]

We cut quite a bit of Corian, what bot do you have?
We use a o-flute and a two flute up-cut (1/4") 13,000-15,000 rpms @MS 3 ips, .125-.23 per pass.

[BruceH]

I have a PRS Alpha 120 x 60 with single spindle and a vacuum table. Do you recommend a plastic cutting bit for this material? I ask because it seems much denser than acrylic.

[Brady Watson]

Do not cut @ 3 IPS until you verify that the design and settings are capable of doing the cuts.

This is why I gave you baseline numbers to start...THEN feather in more speed as YOUR machine allows you to.

As I previously stated - 2-flute carbide end mill or bit specifically made for cutting solid surface from Onsrud.

-B

[bleeth]

There are a multitude of formulas for "solid surface" material. Even Corian uses several different ones depending on the exact pattern and look they want. Many contain a specific percentage of polyester and this added to acrylic will make it harder, but also more brittle. As a result there is never a "one size fits all" machining technique. I often will use a straight flute 0-flute as I have found it gives me a better finish edge as well as allowing me to cut much smaller parts without failure from movement of the parts. I generally will use 2 passes, always ramping in, in conventional direction and leaving a thin skin and then do a final pass cutting out the parts. Due to the high cost of the material I rarely cut very fast. 1.5 ips or so and spin (using the ears to adjust accordingly) anywhere from 8-12.5 thou.

[BruceH]

Thanks, Dave. Can you explain what you mean by "using the ears to adjust accordingly"?

[Kyle Stapleton]

We cut cutting boards (about 10"x12") at that speed with a skin for vac table.
Also your shop will smell for as long as you leave that stuff in your DC.

[bleeth]

When cutting any material you will learn what it should "sound like" when cutting at the correct feed/speed combo. With plastic you don't get quite the same easy to tell chips like from wood. So you pick your starting spin speed based on asking questions, checking Onsruds chip load charts, etc and then when cutting you can adjust the turning speed up or down to get that "right sounding" cutting action. The more experience you have the better you get at it. Even the same bit in the same material can need speed adjustment as it gets dulled from use, particularly when you are talking solid surface which dulls the heck out of bits fast.

[BruceH]

Thanks to everyone for the input. I've tried RPM's ranging from 8K to 12.5K, at 1.5ips. Each test cut looked fantastic, and I can't honestly tell much of a difference between them. It seems like the sweet spot for this material is pretty generous. The bit was not hot after any of the cuts. At this point, should I start ramping up the feed rate, or just stop fiddling and back the RPM back down to 8K to extend the bit life?

[Kyle Stapleton]

What are you cutting?

[David Iannone]

Do not cut @ 3 IPS until you verify that the design and settings are capable of doing the cuts.

This is why I gave you baseline numbers to start...THEN feather in more speed as YOUR machine allows you to.


-B

That is a good rule to live by. I always toolpath slow, then creep them up OR down, ya never know. Its a lot easier to speed up the machine than it is to slow it down.

Dave

[Brady Watson]

Today, 11:30 AM

Novanite - Has anyone worked with this material?

Today, 12:07 PM

We cut quite a bit of Corian...

Today, 12:39 PM

We cut cutting boards (about 10"x12") (sic - out of Corian) + pics

Today, 05:17 PM

Thanks to everyone for the input. I've tried RPM's ranging from 8K to 12.5K, at 1.5ips. Each test cut looked fantastic, and I can't honestly tell much of a difference between them. It seems like the sweet spot for this material is pretty generous. The bit was not hot after any of the cuts. At this point, should I start ramping up the feed rate, or just stop fiddling and back the RPM back down to 8K to extend the bit life?

Today, 05:21 PM

What are you cutting?

OK...I give up. 4:20 ?

-B

[Kyle Stapleton]

Thought it was clear what material he is cutting...
I was asking what he was cutting... Ex: a large countertop 25x80 with two sinks, or maybe small little parts like 2" tall letters for some project.

If he is making the countertop I think changing the speed from 1.5ips would be a grat idea. If it is the letters 1.5ips seems fine.

[BruceH]

I see. So, look to go a bit faster for large simple geometry, and slower for the articulate stuff? Is that a general rule of thumb regarding other materials as well?

I'm not working on a specific project just yet. This piece is just R&D. The plan is to use this material (or another like it) for signs, including some 3D carving. I carved a few different types of paths with various bits at the suggested feeds & speeds, and they all came out very clean. It's a great material to work with. I found that Vcarving with my .25 60º engraving bit gave a beautiful, crisp flute, but I had to run the paths twice to clean out the hard packed chips. That was a lot faster than trying to clean it out with air or a knife.

You've all been great help figuring out where to begin. Thanks so much!

[scottp55]

Bruce, No experience with this material, but if it was a new wood or bit for me...
I would go back to 12.5K that you said the cut was good at, then gradually increase Move Speed by .1IPS steps using the Shift> while watching and listening to cut quality. When cut quality degrades, Back it off to last speed it was cutting Great. Then edit the bit in the toolpath to that speed. Then if you want to maximize it, go again and increase RPM at the same time you increase Feed.
Then if you want to play with Depth Of Cut you can.
On chip clean-up. I quite often run a clean-up/speed pass to get rid of fuzzies and or any deflection from my 1/8" bits. I Copy the toolpath/rename it by prefacing with Speed/ then edit the bit to go either a full depth pass (if bit has the CEL for a VBit), then double Z(or more)Move Speed, and increase X,Y Move Speed by at least 50% and (sometimes 300% depending on material) as it's really not "cutting" and only cleaning chips and possibly a VERY light skin layer.
Saves a lot of very persnickety sanding finishing on fine details.

On curvy and small items, quite often the machine never gets up to the speed you have it set at because of the Virtual Ramping(nothing to do with the ramping you may/should be putting in the Toolpath). You have to play with it a bit and find out what's best for your machine/material/and specific file.
Hope this helped.
scott

[Brady Watson]

Bruce,
Any time you attempt to cut a material you haven't worked with before, it is best to err on the side of caution and go slow at first - then add more cutting speed as the tool allows. Make observations (sight...sound...smell) and adjust MS and RPM as you see fit to get it running in the 'sweet spot'.

As a general rule, I tell new users to start cutting at 2,1 and 12-15k for their baseline; a little slower for denser materials. Once the tool is cutting successfully, then keep adding more speed to see what you can get away with - without the tool sounding too labored or screaming (as Dave points out), with good cut edge quality. You can go nuts with chipload calculations, but they are really for high output production & it is rare that most machines with actually cut at that rate.

The basic idea here is to keep your new tool intact - actually cutting parts without snapping off right away. It gives you some time to observe and listen how to tune it. Nothing is worse than chucking up a new bit and then promptly breaking it off...like 3x in a row because you are starting into the material too aggressively. :eek:

In case you haven't figured it out, you can pause machine movement with the spacebar or S key and press 'I' to Insert a command. Then insert MS and change your Move Speed to something else with the fill-in sheet & then Resume your file. It will pick up where it paused and cut at the new move speed.

-B

[scottp55]

"In case you haven't figured it out, you can pause machine movement with the spacebar or S key and press 'I' to Insert a command. Then insert MS and change your Move Speed to something else with the fill-in sheet & then Resume your file. It will pick up where it paused and cut at the new move speed."

Thanks Brady, Usually doing small stuff, so will Shift> say .4IPS at a time before changing going back to change original Toolpath, as overriding speed in a 1" design too much, can make for "Jerky" moves that affect cut quality. VR settings don't change to accommodate the increased speed I thought?
Does inserting command do the same thing (too abrupt a stop at change of direction)?
Thanks,
scott

[Brady Watson]

Changing the speed via shift + < or > should be used with discretion. Try not to increase speed by too much, because that will result in jerky movements. The command buffer stack is only refreshed (and recalculated with applicable accel/decel VR settings) when there is a break in the file. That includes pausing the file.

-B