Feeds, speeds for finishing pass

Hey there everyone!

So I've just finished building a DIY CNC machine (Root 3 CNC with a 2.2kw spindle)

I think I'm getting the hang of things now and familiarising myself with feeds & speeds for various end mills and stock.

I understand the reason the tool removing the optimum sized chips and tuning the feeds and speed to achieve a target chip load etc.

E.g after lots of reading and multiple tests, I've settled on this for a 2 flute 6mm compression bit, cutting 6mm ply.

HOZLY 6 * 22 * 50L Compression bit (Tungsten Cobalt + DLC)
2 passes @ 3.5mm DOC per pass
13000 RPM 1040 mm/m

That works fine and all, and it doesn't tear the top or bottom due to the compression bit, but it doesn't really give a nice precision edge.

However, if leave 0.5mm on the roughing passes, and then come back and take off that last 0.5mm with a finishing pass with say 20,000 RPM at 500mm/m it makes the cuts look so much nicer. Damn nice actually, considering it's a machine made from mostly 3D printed parts and skateboard bearings.

So my question is, with the stepover only being 0.5mm on a 6mm diameter bit for this finishing pass, can I disregard these commonly stated chipload equations and go slow with a high RPM and make a bit of fine dust just for the finishing pass?

Thanks!

Hi TQ - If your making dust vs chips your tool is rubbing so is wearing. Just because you are cutting at 0.5mm radial does not mean you can fudge the cut. Well you can but then you will use more tools than needed as they wear faster. So if you look at the tool makers catalogue it will have chip loads for slotting and finishing. Use the finishing Cl and your tool will be happy and your wallet will be happy. Do some test cuts and look at the sawdust. If they are chips then that's good if its dust then make the CL bigger.

2F 13000rpm and 1040mm/min is feed/rpm/N 1040/13000/2= 0.040mm which is a small chip. I usually cut in the 0.1 to 0.2mm range for ply. 0.05mm is good for finishing... Peter

by the way to get a precision edge you will always need to do a rough pass and a finish pass. Roughing and finishing have different purposes and even different tools. eg for finishing a parallel router bit maybe better than a spiral bit so the edge is cleaner cut. keep at it...

Chip Load Chart - CNC Tooling - Cutter Shop (cutter-shop.com)

this chart says 0.3mm for plywood and soft wood. I think it would have to be a commercial machine to chomp that much and clear the tool in the cut... I have been using DLC coated 1F bits lately and they have been excellent. I expect they could cut at 0.3mm as the coating is very slippery and flicks chips out really nicely...

Premium 3.175mm single flute end mill DLC Coating carbide spiral milling cutter cnc engraving woodworking acrylic – Aliexpress

DLC diamond like coating - it has the lowest friction coefficient of any of the coatings plus the coating results in a sharper tool...I like them. They are even quieter than others.

your finishing spec is 0.0125mm chip thickness so I expect your making dust and burnishing the timber vs cutting it. Its getting down to your tool runout spec... So one tooth maybe cutting one is rubbing.

In almost every case I climb cut my roughing pass with Walnut, Maple, Cherry, Baltic Birch ply, etc. and leave about 0.005" for the finishing pass cutting conventional. I use the same bit, usually 1/4" compression, 18k rpm, 175 ipm to 250 ipm for both the roughing and finishing passes. My edges come out very clean. The finishing pass is full depth and I usually overlap the starting point at least 1/2", sometimes more.

Quote:

---

Originally Posted by peteeng

Hi TQ - If your making dust vs chips your tool is rubbing so is wearing. Just because you are cutting at 0.5mm radial does not mean you can fudge the cut. Well you can but then you will use more tools than needed as they wear faster. So if you look at the tool makers catalogue it will have chip loads for slotting and finishing. Use the finishing Cl and your tool will be happy and your wallet will be happy. Do some test cuts and look at the sawdust. If they are chips then that's good if its dust then make the CL bigger.

2F 13000rpm and 1040mm/min is feed/rpm/N 1040/13000/2= 0.040mm which is a small chip. I usually cut in the 0.1 to 0.2mm range for ply. 0.05mm is good for finishing... Peter

by the way to get a precision edge you will always need to do a rough pass and a finish pass. Roughing and finishing have different purposes and even different tools. eg for finishing a parallel router bit maybe better than a spiral bit so the edge is cleaner cut. keep at it...

Chip Load Chart - CNC Tooling - Cutter Shop (cutter-shop.com)

this chart says 0.3mm for plywood and soft wood. I think it would have to be a commercial machine to chomp that much and clear the tool in the cut... I have been using DLC coated 1F bits lately and they have been excellent. I expect they could cut at 0.3mm as the coating is very slippery and flicks chips out really nicely...

Premium 3.175mm single flute end mill DLC Coating carbide spiral milling cutter cnc engraving woodworking acrylic – Aliexpress

DLC diamond like coating - it has the lowest friction coefficient of any of the coatings plus the coating results in a sharper tool...I like them. They are even quieter than others.

your finishing spec is 0.0125mm chip thickness so I expect your making dust and burnishing the timber vs cutting it. Its getting down to your tool runout spec... So one tooth maybe cutting one is rubbing.

---

Ok thanks.
Well I got a target chip load of 0.046mm from the 'starting out' table here https://www.mekanika.io/blog/learn-1...s-explained-12
Would you say this is bad advice?

The problem I have is if I try push too hard on this machine and move the feed rate up to say 3000 to get to your suggested chip load of 0.1mm, the cut starts to become inaccurate and I get chatter etc.

I guess then if really do need to always have a higher chip load, but not move too fast, I need reduce the depth per pass?
The problem then is, I believe it needs to bury up-cut portion of the compression bit in the first pass so the top doesnt rip up, which on the 6mm diameter bit looks like about 3mm.

As mentioned, I'm already using DLC coated tools. They look very much like the ones you linked, only 2F instead of one. And they're compression bits.

I can see now that reducing the number of flutes to one will double the chip size at the same speeds so perhaps that's where I've gone wrong.

I'll switch to single flutes first and see how that goes.

Hi TQ - The stiffness of your machine will always be the limiting factor. If its a hobby, time and material removal rate (MRR) does not matter. But it is good to understand the physics of the process to get the best value from your bits. Its all a juggle to find your machines best DOC, chip thickness etc to achieve a good cut. Once you know these parameters you can stick to it. Then you can work on your machine stiffness if needed. I like 1F tools and your going down the right path. Keep learning... Peter

Regarding 0.046mm CL. I don't think it's bad advice, its just a number. The thicker the chip the better the MRR plus if the machine can do it the less chance of rubbing so you get the best tool life. Then there's tool sharpness to consider. A new tool will be able to have a larger cut. All of these factors:
tool run out, machine stiffness, tool stick out, tool sharpness, how many penguins you have, spindle power, machine accuracy, how the controller discretises the path etc end up affecting the cut.... the more you learn the better machinist you become.