CNC rpm & feed

[Rewound]

Ihave the opportunity to use a CNC router and I am trying to use fusion to create the NC file

so (soft wood) for a 7mm HSS 4 flute mill fusion has chosen 4000rpm at 500 mm / min
I tried GBT and asked for optimal cutting (for tool life) and it says 10,000 rpm and 4500mm / min (anything slower would cause to much heat build up (which seems counter intuitive))

what speeds should I be using and does slower really produce more heat?

 

[Sideways]

What's GBT ?


If you are going to cut wood, why would you use a 4 flute HSS mill ?
Think routers for a minute. No one uses HSS. We use TCT cutters because they handle abrasion and stay sharp longer. They are readily available.

When cutting it's essential that your combination of rpm and feed means that each edge cuts a real shaving, and doesn't just scrub over the same surface again and again creating friction and wood dust.
Soft wood is prone to burning so you need an adequate feed rate to cut and move on from edge to cutting edge.
Chip clearance is an issue so fewer flutes are better and remember multiple passes taking relatively shallow cuts.
Just relating to use of a handheld router, I'd be looking at a 2 flute TCT cutter. Probably a spindle speed of 10,000 rpm+ multiple shallow passes incrementing by 2-3mm depth each pass.

The speed I'd push a 6 or 7mm 2 flute through softwood I think would turn out to be noticeably quicker than 500mm/min, so if I was using a 4 flute that "noticeably faster" would also be doubled, but as we don't think in those terms cutting handheld, I can't be specific.

A four flute cutter would need half the rpm of a 2 flute and just 1/4 of that of a single flute cutter for a given feed rate.

 

[Rewound]

firstly its not my machine and this is the cutters I have been told I can use!

yep, they are the type of milling cutters I would use on the metal milling machine. I was surprised not to see normal router bits but then I have never used a cnc router before. and interestingly when I look at Fusion (cad software) it just shows these type of milling heads

we have boxes of normal woodworking router bits but i'm told they are not for this machine!
is this what is normally used in woodworking cnc machines?

So I am a bit limited at the moment and my first task is to get the thing up and running (i don't think anyone really knows how to use it (or at least set it up to do 3d cutting.))

I have done a test NC file for tomorrow and have set the speed to 10,000 rmp 4500mm/min and limited cutting to 4mm depth - see what happens

 

[Chief Sawdust Maker]

I run a CNC Router pretty much daily in a commercial shop cutting Oak, Ash, Maple, Plywood & Redwood
For the majority of my work which is profile cutting shapes out of material from 5mm to 30mm thick I use either 1/8 or 1/4 Carbide 2 flute spiral cutters, I use upcut and down cut depending on the item and the work holding method.
Spindle speed is usually between 18,000 to 19,500 rpm
Feed speed is usually around 100 inches per minute
Depth of cut when profile cutting usually 1 x the dia of the cutter
A link to probably the most comprehensive cutter range along with speeds and feeds https://www.amanatool.com/
The key to successful feeds and speeds is chip loading which i would suggest you goggle and read up on
If you want to post more details of the wood, the machine and the cut or cuts, I can give you an idea of the cutter with sppeds and feeds i would use in my shop
Hope this helps
D

 

[Rewound]

I run a CNC Router pretty much daily in a commercial shop cutting Oak, Ash, Maple, Plywood & Redwood
For the majority of my work which is profile cutting shapes out of material from 5mm to 30mm thick I use either 1/8 or 1/4 Carbide 2 flute spiral cutters, I use upcut and down cut depending on the item and the work holding method.
Spindle speed is usually between 18,000 to 19,500 rpm
Feed speed is usually around 100 inches per minute
Depth of cut when profile cutting usually 1 x the dia of the cutter
A link to probably the most comprehensive cutter range along with speeds and feeds https://www.amanatool.com/
The key to successful feeds and speeds is chip loading which i would suggest you goggle and read up on
If you want to post more details of the wood, the machine and the cut or cuts, I can give you an idea of the cutter with sppeds and feeds i would use in my shop
Hope this helps
D

thankyou - I will get back to you tonight, off to have a play with it now, try and learn how to position the head and upload the NC - it is going to be a huge learning curve.

what software do you use to design stuff on - hope it is fusion as I am OK with that (3d printer and laser cutter) but never used the manufacture side before and its full of setting that I don't understand (although I have managed to create a basic NC) just hope it wrks


I do work with wood quite a lot (see my latest project below), but the CNC router is going to be a new challenge, and I don't think anyone here really knows much about it

still to be finished!

 

[Steve Mehrlich]

i have a relativley small desktop cnc router, workable area of 750 x 750 ish, and im always surprised at how slow the sweet spot for my spindle is when running at an average of 2500 - 3000mm/min.
i agree with mr sideways, 2 flute carbide cutters 4mm or 6mm with a spindle speed of 12000 rpm is good for me in oak.
depending on what youre doing will make a difference to your cut depth.
you mention 3d cutting which is a completely different ball game to profile cuts.

 

[Chief Sawdust Maker]

Wow nice table very impressive
I use Carveco Maker, I come from an autocad background and managed to get a subscription deal on maker. It does have its niggles, I have tried demo versions of most of what's out there and I will most likely change in the future, but its finding a gap in the workshop schedual to have time to learn new software and convert existing projects.
Look forward to hearing how you got on and happy to try to help

 

[Steve Mehrlich]

im amazed that anyone could make that table without a cnc, very good.....

 

[Rewound]

i have a relativley small desktop cnc router, workable area of 750 x 750 ish, and im always surprised at how slow the sweet spot for my spindle is when running at an average of 2500 - 3000mm/min.
i agree with mr sideways, 2 flute carbide cutters 4mm or 6mm with a spindle speed of 12000 rpm is good for me in oak.
depending on what youre doing will make a difference to your cut depth.
you mention 3d cutting which is a completely different ball game to profile cuts.

at the moment the machine is only used very occasionally and has only been used to cut stuff out and engrave. I think they start off with a pdf convert to dxf then the macine makes th NC, then they adjust the Z manually.

when I say 3d I want to have the Z in the NC - so what I was going to try and do today was this - a cut at 3 different heights

 

[Rewound]

im amazed that anyone could make that table without a cnc, very good.....

they have a laser ccutter which is just fantastic - the only real skill in that table is the leg

 

[meccarroll]

I'd go pretty much with what Chief Sawdust Maker has said above.

A lot will depend upon the machine rigidity and power of the spindle you are using. A solid metal frame with 3Kw spindle will handle faster feed rates than a bolted aluminium frame with a 1 Kw spindle.

I would not use a four flute bit for solid wood or even plywood, two flute would be better.

The cutters in a CNC are spiral because they help remove waste chips as they cut straight cutters don't and so heat builds up and the bit generally can not move as fast.

I have a ridgid steel frame CNC with a 2.2Kw spindle and cut melamine faced chipboard at around 14000-18000 RPM with a feed rate of 3000mm min and that seems to work for me. The bit I use in melamine is a special 8mm staight bit with chip breakers so specially designed for melamine faced chipboard on a CNC but in sheet wood like plywood I'd probably use a spiral bit. I'd def use a spiral bit in MDF (Compression Bit).

Take a look on Utube to see the difference between Up cut, Down cut and compression bits. I think you will be dissapointed with the finished resut using a four winged cutter that's if it does not overheat and break before the job is done.

Mark

 

[Ollie78]

Single flute compression bit is very good for most sheet stuff and general woodworking.
It is all about chip clearance. If you look at the spec sheet for many of the cutters it is impossible to reach the feed rate required for the correct chip removal with smaller cnc routers.
I have been running a single flute compression at 18000 rpm . I was using mostly 2 flute cutters but the singles suit my machine better.
The difference when you get the speed right is you don`t get dust but nice little chips instead.

here is a chart of speeds.
https://cdn.shopify.com/s/files/1/0...ds_Chart_Rennie_Tool_Company.pdf?v=1680523145

By comparison I have a 3 flute carving bit that wants to go at 1600rpm and as fast as my machine will push it.

Another issue is that many spindles lose torque at speeds below half thier maximum so you wouldn`t want to run a 24000 rpm spindle at 8000 rpm in order to get the right chip load, so you need to increase feed rate.

This explains about chip load
https://www.rennietool.co.uk/blogs/news/solid-carbide-router-bits-speeds-and-feeds

 

[Steve Mehrlich]

at the moment the machine is only used very occasionally and has only been used to cut stuff out and engrave. I think they start off with a pdf convert to dxf then the macine makes th NC, then they adjust the Z manually.

when I say 3d I want to have the Z in the NC - so what I was going to try and do today was this - a cut at 3 different heights
View attachment 188849

and have you managed to model , simulate that in fusion?

 

[Rewound]

and have you managed to model , simulate that in fusion?

yep - and it worked

the diameters were all 1mm too small, however I think that was because of this setting?

I think I now understand what the 'stock to leave' option is - although radial & axial?

As for the 'max roughing stepdown' since I was using a 7mm mill could I have set this to 7mm (esp for softwood?)
any thoughts on any of the other settings?

 

[Steve Mehrlich]

yep stock to leave will be it, axial leaves 0.5mm in the z and radial leaves 0.5mm in the y and x. adaptive toolpath is good for 7mm deep no problem and thats a healthy optimal load. easy..

 

[Rewound]

yep stock to leave will be it, axial leaves 0.5mm in the z and radial leaves 0.5mm in the y and x. adaptive toolpath is good for 7mm deep no problem and thats a healthy optimal load. easy..

I see that 'optimal load' thing now - it will take 2.8mm (horizontally) of material on each pass? on a 7mm mill that would be 40% of max ? I take it that setting will probably just adjust itself for dif mill sizes? and would seem a reasonable amount to take off for wood.

 

[Rewound]

and should I have used climb or conventional (I know what they are but never entirely sure what to use)

 

[Steve Mehrlich]

i always run with climb

 

[Steve Mehrlich]

I see that 'optimal load' thing now - it will take 2.8mm (horizontally) of material on each pass? on a 7mm mill that would be 40% of max ? I take it that setting will probably just adjust itself for dif mill sizes? and would seem a reasonable amount to take off for wood.

yes so 7mm in the z and 2.8mm in its horizontal moves. 2.8mm is hefty , okay in a softwood, you might need to dial that down in anything harder.

looks pretty good apart from the tear out on top, either get yourself a compression bit or run a second op with a downcut bit. with a compression bit you might be able to get rid of the stock to leave and machine it to size in one go, that will depend on the depth of those steps?. if you go with a second op with a downcut bit get rid of the stock to leave in the axial but leave 0.5 in the radial so the downcut bit has something to clear up.

 

[Ollie78]

Amost always use climb cut. The exception is when using a last "cleanup" pass. Sometimes refered to as a "spring pass" in metal machining.
This is sometimes helpful to remove fuzzy surface finish.
V carve pro will automatically do this when doing lettering depending on the direction of the curves etc.
Leave 0.5 mm under and then do last pass with reversed direction. Can`t remember how fusion 360 does this but I think there is an option.