New milling motor Proxxon FBS 240/E upgrade to Kress 1050 FME-1

So I have a cnc, that is about 90x45cm in size. Until now I was using the Proxxon FBS 240/E, but it is not up to the job, so I need to replace it. Right now I am thinking about getting a Kress 1050 FME-1, or one of the chinese 2.2kW liquid cooled motors (the chinese one is also twice the price). Which would be a better option for me, or should I get something completely different. I am mostly working with wood and occasionally plastics, but I would like to be able to also work on aluminum, when we upgrade the machine.

The Chinese water spindle is way better than the Kress, which is not really made for that job. Its like comparing Ferrari to a tractor

Quote:

---

Originally Posted by Boyan Silyavski

The Chinese water spindle is way better than the Kress, which is not really made for that job. Its like comparing Ferrari to a tractor

---

I was leaning towards the Chinese spindle, since i saw a comparison, and it is a lot quieter.
As far as I know Ferrari also made tractors, and the Proxxon I had was not made for the job, but it worked for the last few years. But as I said, I will most likely go with a Chinese spindle.

Poslano z mojega ONE A2003 z uporabo Tapatalk

Quote:

---

Originally Posted by Zynch175

As far as I know Ferrari also made tractors, and the Proxxon I had was not made for the job, but it worked for the last few years.

---

Think you'll find that was Lamborghini.!!. . . But Boyan is correct Kress are toys in comparison.

So I found some local guys doing a group buy, and I got in, so I ordered a 1,5kW spindle, since the 2,2kW are quite a bit over my budget.

I had a Kress. Noisy as hell. Go for a smaller Chinese Watercooled spindle if you can.

And I wouldn't worry about going for the smaller spindle. I doubt that many home-built machines can fully load the bigger spindle and the main reason for choosing the larger size is they usually take ER20 collets which allow up to 1/2" cutter shanks.

Indeed. The Kress is only rated at 1050 Watts. I think it will smoke before it delivers that type of output.

Quote:

---

Originally Posted by Neale

And I wouldn't worry about going for the smaller spindle. I doubt that many home-built machines can fully load the bigger spindle and the main reason for choosing the larger size is they usually take ER20 collets which allow up to 1/2" cutter shanks.

---

I went for the 1.5kW one, since the group buy has the 1.5kW or 2.2kW. And I decided that the new spindle is going on the new machine, that is in the process of designing (about 1000x1500 in size). It is going to be a modified frame of an embroidery machine, and the stepper motors and their drivers will also come from the machine. Once I get some drawings together I will post it to get an opinion on the design.

Poslano z mojega ONE A2003 z uporabo Tapatalk

Quote:

---

Originally Posted by Neale

And I wouldn't worry about going for the smaller spindle. I doubt that many home-built machines can fully load the bigger spindle and the main reason for choosing the larger size is they usually take ER20 collets which allow up to 1/2" cutter shanks.

---

I've got a 2.2kw WC spindle coming for a new build, what size cutter could these handle in aluminium??

I have read that torque drops badly at lower speeds but what is the usable range???

Quote:

---

Originally Posted by Davek0974

I've got a 2.2kw WC spindle coming for a new build, what size cutter could these handle in aluminium??

I have read that torque drops badly at lower speeds but what is the usable range???

---

Typically 12 - 24K. Size of cutter all depends on width and depth of cut.

http://zero-divide.net/?page=fswizard get used to using this, it also tells you how much power you need.

Quote:

---

Originally Posted by Chaz

Typically 12 - 24K. Size of cutter all depends on width and depth of cut.

http://zero-divide.net/?page=fswizard get used to using this, it also tells you how much power you need.

---

Thanks, looks like small cutters and solid carbide are the way forwards. HP does not really factor until you get up in the 10mm dia range and a 10mm carbide tool is quite spendy. But at that size machine rigidity would be a serious factor so conservatively I would guess that carbide cutters <5mm dia are the order of the day for aluminium.

Good calculator in that link BTW

Quote:

---

Originally Posted by Davek0974

Thanks, looks like small cutters and solid carbide are the way forwards. HP does not really factor until you get up in the 10mm dia range and a 10mm carbide tool is quite spendy. But at that size machine rigidity would be a serious factor so conservatively I would guess that carbide cutters <5mm dia are the order of the day for aluminium.

Good calculator in that link BTW

---

Ye, very good as a starting point.

Stick to 2 flute for alu, my 'favorite' sizes are 8mm roughing, 6 and 10mm for finishing, 4mm for smaller if needed.

Quote:

---

Originally Posted by Davek0974

I've got a 2.2kw WC spindle coming for a new build, what size cutter could these handle in aluminium??

I have read that torque drops badly at lower speeds but what is the usable range???

---

The usable range is between 5000 and 24000 rpm if the VFD is setup properly. But yes torque does drop at lower speeds so does have limitations.
You can use the full cutter size range upto 13mm in aluminium but it will affect DOC and Feedrate. I cut lots of aluminium and find 8mm with 3 flutes is nice size that allows good DOC and feed rates. If used with trochiodal toolpaths the removal rate is brilliant and shifts large amount of chips.

My 2 most often used cutters are 8mm 3 flute rougher and 6mm 2 flute spiral flute for finishing. When ever possible I use Trochiodal toolpaths.

Quote:

---

Originally Posted by Chaz

Stick to 2 flute for alu

---

Not always the best for Alu. It depends on the job and type of cut. If your profiling for instance and not slot cutting then more flutes are better. They allow faster feed rates with higher MRR and give better finish.
I find 3 flutes are best at roughing.? They are Stiffer and more ridged so can cut deeper. Feed rate and MRR is higher. They give a better finish if not roughers because More flutes.
The only thing is they need more attention to chip clearing and chip clearence. So not ideal for Slotting or small pockets and tight corners where tool cuts on two edges. When used with trochoidal tool paths they rock compared to 2 flute and can be run much faster with more DOC.

Quote:

---

Originally Posted by JAZZCNC

Not always the best for Alu. It depends on the job and type of cut. If your profiling for instance and not slot cutting then more flutes are better. They allow faster feed rates with higher MRR and give better finish.
I find 3 flutes are best at roughing.? They are Stiffer and more ridged so can cut deeper. Feed rate and MRR is higher. They give a better finish if not roughers because More flutes.
The only thing is they need more attention to chip clearing and chip clearence. So not ideal for Slotting or small pockets and tight corners where tool cuts on two edges. When used with trochoidal tool paths they rock compared to 2 flute and can be run much faster with more DOC.

---

Agreed but generally this is good advice. I use 3 flute 8mm corn cob to rough. The rest are 2 flute.

Certainly anything higher than 3 in alu generally is a problem for most.

Great, thanks.

Things are simpler on my manual Bridgeport - just throw in a tool, set the speed to the chart and turn the hand wheels at a rate that keeps her happy :) Got a lot to learn - my reason for building a CNC partly.

So i have a g-code file from SheetCam and it was programmed for say a 6mm roughing cut leaving an allowance for finish, do i need to make a second file for the finish cut or do you use the same cutter but just program a final cut for the finish pass??

One job i have in mind has some 3mm holes in it, i would be looking at ramping in with a 2 or 2.5mm tool for them and then do the outside profile with a larger tool maybe - I am lacking knowledge of how you change tool and get back to exactly the right place OR do you use the tool dia offsets in Mach3

As i said, lots to learn;)

Quote:

---

Originally Posted by Davek0974

Great, thanks.

Things are simpler on my manual Bridgeport - just throw in a tool, set the speed to the chart and turn the hand wheels at a rate that keeps her happy :) Got a lot to learn - my reason for building a CNC partly.

So i have a g-code file from SheetCam and it was programmed for say a 6mm roughing cut leaving an allowance for finish, do i need to make a second file for the finish cut or do you use the same cutter but just program a final cut for the finish pass??

One job i have in mind has some 3mm holes in it, i would be looking at ramping in with a 2 or 2.5mm tool for them and then do the outside profile with a larger tool maybe - I am lacking knowledge of how you change tool and get back to exactly the right place OR do you use the tool dia offsets in Mach3

As i said, lots to learn;)

---

Get Fusion 360, watch lots of good utoob vids on how to CAD and then CAM in it. Sorted.

Quote:

---

Originally Posted by Chaz

Agreed but generally this is good advice. I use 3 flute 8mm corn cob to rough. The rest are 2 flute.

Certainly anything higher than 3 in alu generally is a problem for most.

---

No it's not generally good advise because depends on the type of cut and machine, along with several other factors like cooling etc.
Slot cutting is worst case for most because chip clearence is less so people use less flutes to give more clearence. But if the machine is strong enough and cutting parameters are correct then 3 flute will work just fine and give higher MRR. It's generaly only good advise to those that don't know there machines capabiltys.!
Like wise for finishing or cutting with plenty of chip clearence like profiling then multi flute cutters work great provided the machine can handle the higher feed rates. People go wrong by using multiflute cutters is wrong situations or more often much too low feedrate. If run correctly in right places multiflute cutters give a much better finish.

Quote:

---

Originally Posted by Chaz

Get Fusion 360, watch lots of good utoob vids on how to CAD and then CAM in it. Sorted.

---

I have that installed, trial period. I found it very complex TBH.

For what i need to do, SheetCam should be ok, I am very familiar with that as I use it a lot for my CNC plasma table, but that has no tool sizes - just the torch and that never changes size :)

Will be watching some videos though

I sometimes use 6mm 2 flute carbide tools with a 45 degree helix, but they are a little more expensive.

The more standard 30 degree helix also works but the 45 degree angle is supposed to be more tailored to aluminium cutting.

Quote:

---

Originally Posted by Davek0974

So i have a g-code file from SheetCam and it was programmed for say a 6mm roughing cut leaving an allowance for finish, do i need to make a second file for the finish cut or do you use the same cutter but just program a final cut for the finish pass??

---

Just one file for both operations.
If corner radius are larger than the roughing cutter and the flutes edges are good enough for finish then use same tool. If not then just use smaller tool for the finish so it can clear the corners, always use a tool just little smaller than the corner radius. But in both cases it can all be done in one file.

Quote:

---

Originally Posted by Davek0974

One job i have in mind has some 3mm holes in it, i would be looking at ramping in with a 2 or 2.5mm tool for them and then do the outside profile with a larger tool maybe - I am lacking knowledge of how you change tool and get back to exactly the right place OR do you use the tool dia offsets in Mach3

---

With circler pockets or holes Spiral rather than ramp if possible.
When you change tools the G-code file just stops tells you to change the tool and waits for you. You then can jog the machine to easy position to change the tool. After changing the tool you reset the new Z height by touching off the material again and setting zero. Then just press cycle start and the cutting continues.
The Cam software will have taken care of tool offsets when created the g-code.

Great so I can pretty much ignore the tool offsets in Mach as it's all done in cam - program roughing cut on tool 1, program tool change, program finish cut on tool 2. Mach3 runs the roughing cut, stops and requests a tool change, I change tool and re-zero Z, press go and drink coffee ?

Now it makes sense, gets confusing when you have tool charts etc in Mach, I presume they are meant for g-code where the tool offset is not pre-programmed in cam?

Yes i meant spiral cut not ramp.

Thanks BTW

Quote:

---

Originally Posted by Davek0974

I presume they are meant for g-code where the tool offset is not pre-programmed in cam?

---

No tool offsets are for machines that have spindles with tool holders that can be changed. In this case you measure the tool length offset which is the distance from the tool tip to the surface on the holder that contacts the spindle nose. You also have the option to enter diameter for when doing tool compensation. Say for wear or under size tools.

On manual tool change spindle without repeatable holders, like ER collet system on most routers then it's not used and just leave empty. It's actually important that you don't have any values in these because if the Cam calls for G43H which is tool length compensation and theres value in that tools offset it will be applied to the tool length and change the Z height.

To see this happen do a test. Set tool #1 in tool offsets to height of 10mm and save. Then zero out the Z for tool #0 which will be the default tool when first starting mach and all offsets are referenced from.

Now using MDI type g43 H1 T1 (space between them) and you'll see the Z dro change to -10. G43 applied the tool length offset and now mach thinks the tool is at different height.! . . . Very dangerous when not being used correctly.

Don't forget to go back and set tool #1 to zero.!!

Great, thanks for that, its all starting to make sense now, surprising differences between plasma cutting and milling.

Dave