Author Topic: CNC mill spindle up grade  (Read 4234 times)

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3048
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #15 on: October 11, 2021, 12:51:06 PM »
Hi Mike,
you will find the download not at the webshop site.
It is at the company site, Services, Downloads, Fräsparameter
Schnittdatenrechner

But if I remember well, you have made already an attempt and that has struggled due to the 64bit and Windows.



Kind Regards
Achim

Offline Vixen

  • Full Member
  • *****
  • Posts: 2514
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #16 on: October 11, 2021, 01:05:43 PM »
Hello Achim,

Your memory is much better than mine. Yes, you did send the link before but as you say it is a 64 bit program, which I cannot run on my old Win machine

Thanks again

Mike
It is the journey that matters, not the destination

Oh! sod the journey, lets hit the bar and pool instead.

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3048
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #17 on: October 11, 2021, 01:13:16 PM »
Mike,
5.000 rpm would give this result for EN AW 7075 and a 5 mm cutter with 3 flute.
Would it match with your experience ?
Kind Regards
Achim

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8458
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #18 on: October 11, 2021, 01:15:22 PM »
Just looking in quickly but I could not see where the cutter material is entered in the calculator and would expect HSS to be somewhat lower than Carbide, also Sorotec seem to only sell carbide which may be the reason why? Also Hoffman don't give a speed only a chip load.

Offline Vixen

  • Full Member
  • *****
  • Posts: 2514
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #19 on: October 11, 2021, 03:53:58 PM »
Hello Achim,

I have not yet found a feed calculator that I like to use. I am still trying to understand the Sorotec calculations.  I would need to have a working calculator and play with all the numbers to appreciate how well it works. I think Sorotec use their own figures for fz (tooth feed)(chip load??) but cannot find the parameters used to derive the fz.

Last week I used these parameters to machine the gearbox covers on the W165. all set by guess and feel.

Tool                            2 flute carbide 7.0 mm dia
Cutting speed   Vc      500 m/min
Spindle              n       5300 RPM
Z depth of cut   Ap      5.0mm
in feed              Ae      1.0 mm (15%)
Feed rate          Vf       200 mm/min (could be increased)
Material             Fz       0.030       6082 (HE30 T6)

The cutter sounded to be working hard, it was easier when I increased the spindle speed to maX, I believe I could also have increased the feed rate much higher. But it was working well so I continued, without changing the program. Maybe I will be braver next time and try a higher feed rate.  :zap:

Does anyone else use a different feed calculator that they trust?

Mike
« Last Edit: October 11, 2021, 05:42:36 PM by Vixen »
It is the journey that matters, not the destination

Oh! sod the journey, lets hit the bar and pool instead.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8458
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #20 on: October 11, 2021, 04:25:04 PM »
As I often use a router for woodworking I can understand why you would want to move away from that as I would not want to be using it for an extended period of time even when wearing ear protection, the KX3 is not bad and you can easily have a conversation next to it when at 5000rpm. The was a member over on ME forum who won a Shapeoko gantry type machine and he found it very noisy with a Dewalt router and as there was not much speed control had to use small diameter cutters to avoid overspeeding at the cutting edge which just made the noise worse.

Like Mike I am limited to a 5000rpm maximum speed which with my usual 6mm dia cutters is OK with steel and cast iron as I can run at the right sort of speeds of 4-5K rpm but I am not fast enough to get the optimum speeds for aluminium of smaller diameter tools.

I do try to run at the makers or suplliers suggested spindle speeds where I can but our less powerful and less rigid machines mean the feed rates and to some extent the depths of cut have to be adjusted to the individual machine. I tend to mostly use 0.02mm per tooth (Fz)in steel and cast iron and 0.03-0.04mm/tooth (Fz) in aluminium depending on whether there are any tight internal corners where I will run slower as the cutter engagement is higher and a risk of chatter,

So for a carbide 6mm dia 3-flute cutter with a 0.03-0.04 Fz at 5000rpm I would be feeding at 450-600mm/min which is actually not that different to your figures as at 18,000 that would be 1800-2160mm/min. However if it were an HSS cutter I doubt I would want to run it so fast and my 5000rpm would be about the max I would take it to even if I had a faster spindle. Just looking at my YG-1 catalogue for s 3-flute uncoated HSS-bo at 5mm dia they suggest 6300rpm for both slotting and side cutting and the other supplier I use a lot suggests 7000prm which is what made me ask about your chosen speed. Your Fogbuster will help with the speed and is something I still have to sort out though I do now have a better compressor.

I can't remember what your mill started life as but that will have the biggest effect on how much you can take off, I would tend to take heavier than you have shown here typically with the usual 3-flute 6mm cutter for the first surfacing I would be 1mm deep and say 5mm wide. Then for adaptive the numbers would be 6mm Ap height x 1mm Ae stepover. I may alter this to suit the job but would tend not to go much over that "area" of metal removal so may also use 12mm Ap and 0.5Ae for example. I tend to leave 0.3mm radial on these cuts and then do a finish contour with one roughing pass of 0.2mm Ae and finish pass of 0.1mm Ae.

The bit of your cut that I gave ringed does look a bit "ugly" could it be that the fogbuster is nor reaching the back of the tool?

I really need to sit down wit ha big block of 6082 and just try a few more variables out to really see what my machine can do. What I detailed above it is quite happy with and does not sound under any strain plus I can keep up with clearing the swarf and brushing on some lubrication, no doubt it could be pushed harder but as I only use it a few times a month am happy to stick with what I have found works, it would be different if I had a batch to do or was using it several times a week. No doubt you will go though a similar process with the new spindle to find out what works best on your setup. It's all good fun.


Offline Jasonb

  • Full Member
  • *****
  • Posts: 8458
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #21 on: October 11, 2021, 04:34:44 PM »
Mike I posted as you did

Fusion will calculate the feed for you if you enter the spindle rpm and chip load, or you can enter cutting speed and dia and it will then work out the rpm. Alter any one of the numbers in the chart I just posted (2nd image) and it will adjust the others so really comes down to which perameters you want to enter and it will work out the rest.

There is also quite an extensive tool library with all the data there but it's based on having a high enough max speed, coolant and a rigid machine so some of the feed rates can get quite scary and you have to watch out that you don't leave them at those settings! I tend to use it to just get the basic cutter dimensions and speed, then reduce speed if needed down to 5000 and enter a chipload I feel my machine will be happy with.

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3048
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #22 on: October 11, 2021, 04:35:13 PM »
But it was working well so I continued, without changing the program.


Hi Mike, this is was for sure  a very good decision.
As I mentioned before already, it is jungle.


But if you see the parameters from above mentioned gear box covers and add your feeling concerning the perhaps possible higher feed than it will bring closer to the lower shown picture.


The fz values (tooth feed in mm/ tooth/ revolution) are coming from this chart.
https://webseite.sorotec.de/download/fraesparameter/schnittwerte_en.pdf
The cutting speed Vc ( in m/min) for each material also.


It should be easy to prepare an excel  spread sheet for easy calculation with the shown formulae.
I have done it once temporary, only to see, if it will give similar results as the calculator.


But as always, you have shown already, that experience and feeling are not so bad to get a proper result.
At the end it will be a mix of everything.
[size=78%]     [/size]


« Last Edit: October 11, 2021, 05:12:26 PM by fumopuc »
Kind Regards
Achim

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3048
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #23 on: October 11, 2021, 04:58:06 PM »
As I often use a router for woodworking I can understand why you would want to move away from that as I would not want to be using it for an extended period of time even when wearing ear protection, the KX3 is not bad and you can easily have a conversation next to it when at 5000rpm. The was a member over on ME forum who won a Shapeoko gantry type machine and he found it very noisy with a Dewalt router and as there was not much speed control had to use small diameter cutters to avoid overspeeding at the cutting edge which just made the noise worse.

Like Mike I am limited to a 5000rpm maximum speed which with my usual 6mm dia cutters is OK with steel and cast iron as I can run at the right sort of speeds of 4-5K rpm but I am not fast enough to get the optimum speeds for aluminium of smaller diameter tools.

I do try to run at the makers or suplliers suggested spindle speeds where I can but our less powerful and less rigid machines mean the feed rates and to some extent the depths of cut have to be adjusted to the individual machine. I tend to mostly use 0.02mm per tooth (Fz)in steel and cast iron and 0.03-0.04mm/tooth (Fz) in aluminium depending on whether there are any tight internal corners where I will run slower as the cutter engagement is higher and a risk of chatter,

So for a carbide 6mm dia 3-flute cutter with a 0.03-0.04 Fz at 5000rpm I would be feeding at 450-600mm/min which is actually not that different to your figures as at 18,000 that would be 1800-2160mm/min. However if it were an HSS cutter I doubt I would want to run it so fast and my 5000rpm would be about the max I would take it to even if I had a faster spindle. Just looking at my YG-1 catalogue for s 3-flute uncoated HSS-bo at 5mm dia they suggest 6300rpm for both slotting and side cutting and the other supplier I use a lot suggests 7000prm which is what made me ask about your chosen speed. Your Fogbuster will help with the speed and is something I still have to sort out though I do now have a better compressor.

I can't remember what your mill started life as but that will have the biggest effect on how much you can take off, I would tend to take heavier than you have shown here typically with the usual 3-flute 6mm cutter for the first surfacing I would be 1mm deep and say 5mm wide. Then for adaptive the numbers would be 6mm Ap height x 1mm Ae stepover. I may alter this to suit the job but would tend not to go much over that "area" of metal removal so may also use 12mm Ap and 0.5Ae for example. I tend to leave 0.3mm radial on these cuts and then do a finish contour with one roughing pass of 0.2mm Ae and finish pass of 0.1mm Ae.

The bit of your cut that I gave ringed does look a bit "ugly" could it be that the fogbuster is nor reaching the back of the tool?

I really need to sit down wit ha big block of 6082 and just try a few more variables out to really see what my machine can do. What I detailed above it is quite happy with and does not sound under any strain plus I can keep up with clearing the swarf and brushing on some lubrication, no doubt it could be pushed harder but as I only use it a few times a month am happy to stick with what I have found works, it would be different if I had a batch to do or was using it several times a week. No doubt you will go though a similar process with the new spindle to find out what works best on your setup. It's all good fun.


Jason, I agree 100%, it is always a kind of try and error to get the best and what will work as the best for each of us.
You have mentioned it already, the stiffness of our hobby milling machines can not be implemented in all these nice charts and calculators.
For me here it was necessary to do a test with my not so rigid Proxxon hobby mill, up graded by a nearly industrial spindle.
I will continue tomorrow with a report of the finish machining of the open pocket and what I have made there to get a nicer surface.


Concerning the mist cooling, I would not do the fog buster system again.
The state of the art today, there I am sure, is the peristaltic pump system, as made by Sebastian End, called ColdEnd.   

Kind Regards
Achim

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3048
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #24 on: October 11, 2021, 05:08:24 PM »
Hi Mike,
just another attempt.
If I use  Jasons general recommendation of fz 0,03 mm for aluminium in the calculator, than we are much more closer to your feelings.
That means used feed rate so far, 200 mm/min plus your feeling to try a bit more means 300 mm/min.
So have a look at the picture below, please.
Kind Regards
Achim

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8458
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #25 on: October 11, 2021, 05:11:44 PM »
Yes I've watched quite a few of Sebastian's videos and that's a nice home made machine that he has as well as the Sorotec ones. The Int taper spindle he has also makes tool changing quick, the smaller ATC spindles with their INT20 taper are nice too but quite a bit more expensive :(

I still have a feeling that the Sorotec chart is based on carbide tools not HSS so spindle speed would need to be reduced for HSS.

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3048
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #26 on: October 11, 2021, 05:21:57 PM »

I still have a feeling that the Sorotec chart is based on carbide tools not HSS so spindle speed would need to be reduced for HSS.


That really could be, next time I have a chat with one of them, I will ask and try to find out.
May be I will visit them in Friedrichshafen, "Faszination Modellbau" exhibition, beginning of November.
Kind Regards
Achim

Offline Vixen

  • Full Member
  • *****
  • Posts: 2514
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #27 on: October 11, 2021, 07:46:55 PM »

The fz values (tooth feed in mm/ tooth/ revolution) are coming from this chart.
https://webseite.sorotec.de/download/fraesparameter/schnittwerte_en.pdf
The cutting speed Vc ( in m/min) for each material also.

It should be easy to prepare an excel  spread sheet for easy calculation with the shown formulae.
I have done it once temporary, only to see, if it will give similar results as the calculator.


Hello Achim.

I have already found that chart, thank you. The calculations are simple enough to do without a spreadsheet. Finding the correct value for the various parameters, not so easy.

One problem is the inconsistant use names to describe the different parameters and translation problems between languages.. Some offer less ambiguous descriptions than others. This is how I understand the parameters (correct me if they are wrong)

Fz is often described as the chip load or sometimes feed per tooth and depends on the cutting tool material, tool diameter the type of material to be cut

Vc is often described as the tool surface speed and depends on the hardness/ machineability of the material to be cut.

n is the spindle speed and depends on Vc (tool surface speed) and d (tool diameter).

Vf is the feed rate and depends on  n (spindle speed), z (number of cutter teeth) and Fz (tooth load parameter)


What I cannot find is anything that ties in Ap (depth of cut) and Ae (step over or width of cut) to any of the above. I would have expected the Ap and Ae combination to exert some requirement of Vf (feed rate)

My machine seems happy to do adaptive clearance with Ap = 5.0 mm and Ae = 1.0 mm, Obviously a deeper/wider and faster feed rate cut would need more spindle power and would flex the mill structure ( and cutting tool ?? ) more.  Do you just find a level where the machine is happy and not straining? Is that all there is to it? I doubt that.

Yes, it's a jungle .... no arguement.

Mike


« Last Edit: October 11, 2021, 09:30:04 PM by Vixen »
It is the journey that matters, not the destination

Oh! sod the journey, lets hit the bar and pool instead.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8458
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #28 on: October 11, 2021, 08:06:15 PM »
The makers sometimes give you guidance, for example the YG-1 catalogue gives two sets of data for most cutters, one for when it is being used for slotting and another for side cutting which would be a contour or adaptive cut.  generally the slotting is 1D deep and obviously 1D wide which is quite a heavy cut and a lot more than the old manual rule of thumb of d/4 for depth. The other side cutting is usually 1.5D high by 0.1D stepover (also what F360 defaults to) and this seems to be more within our machines abilities. Slotting tends to be a bit lighter than side cutting as far as chipload and spindle speeds which would seem right given the larger engagement and volume being removed..

Ball nose cutters give you a suggested stepover and all have  a proviso to be reduced for the very smallest cutters in the size ranges. But as you say its a bit suck it and see for what works for you and when you find the sweet spot make a note of it so it can be used again.

If you don't mind the colourful language this is quite enlightening as to how fast you can feed if the spindle speed is upto it and the machine solid, his is homemade by JBwelding blocks of granite together. You can also see his machine gives spindle loading as would other industrial machines so the amount of metal removal would be adjusted to get it working within the best power band.

« Last Edit: October 11, 2021, 08:13:28 PM by Jasonb »

Offline Vixen

  • Full Member
  • *****
  • Posts: 2514
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #29 on: October 11, 2021, 09:49:48 PM »
Still thinking about the Ap, Ae relationship.

Ap times Ae defines the amount of material removed, the bigger the number the more work the spindle motor must do at a given RPM and feed rate.

So. Would an ampmeter, measuring spindle motor current, be an effective 'Spindle load meter' ?

Could you set the depth/ width of cut and then adjust the feed rate to be less than so many amps?

Mike  :thinking: :thinking:

All this is getting a long way from model engineering, more like production engineering where every minute counts.
It is the journey that matters, not the destination

Oh! sod the journey, lets hit the bar and pool instead.