Author Topic: CNC mill spindle up grade  (Read 4475 times)

Offline Vixen

  • Full Member
  • *****
  • Posts: 2546
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #45 on: October 14, 2021, 10:59:56 AM »
Hi Mike, good to know that your experiment was so successful.
.............

To clarify for the future is this speed issue for HSS cutters
Is this rule of thumb, 2/3 of a carbide cutter the way to go there ?
Hopefully I will have the chance to discuss a valid thumb rule here with one of Sorotec guys beginning of November at the exhibition.
They are always very helpfully and they do have a lot of experience from the own milling part production for there machine kits also.                                                    



It's a minefield out there, with lots of conflicting information about. The Sorotec guys should be able to give you the best answer.
In the mean time, I have found this comparison chart for surface speed Vc and feed Fz for different materials. You can see how much slower the recommended surface speed for HSS is compared to Carbide.



It will do untill we can find a better chart. Use it for guidance only.

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: 3057
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #46 on: October 14, 2021, 11:56:51 AM »
Hi Mike, thank you very much.
Good to have this industrial recommendation.
The Hoffmann home page does offer for each cutter a calculator for speed and feed rate.
But unfortunately, they do not offer there any Aluminium material to choose, only 5 to 7 steel variants are possible to select for my 3 flute HSS cutter
May be they do not offer Aluminium because, there is nothing to do really wrong.
Never the less, my usage of the 3,4,5 and 6 mm cutters of these 3 flute HSS series, also some sizes in the longer version, was without any accident so far.
Speed and feed rate orientation since 3 or more years with the Sorotec calculator only so far.
I can not remember, there was one cutter getting blunt so far.
I have broken some, but there has been always other reasons, mostly by a collision.


Just running the finishing with my second attempt of this female torso.
Roughing out yesterday was real a pleasure. 



Kind Regards
Achim

Offline Hugh Currin

  • Full Member
  • ****
  • Posts: 680
  • Box Elder, SD, USA
    • www.currin.us
Re: CNC mill spindle up grade
« Reply #47 on: October 14, 2021, 03:30:20 PM »
Mike:

Is the feed in the chart above for each tooth? If not is it specific to a particular number of teeth?

Thanks.
Hugh

Offline Vixen

  • Full Member
  • *****
  • Posts: 2546
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #48 on: October 14, 2021, 04:23:38 PM »
Hello Hugh,

The parameter Fz (AKA. chip load or tooth feed) is usually defined as Tooth Feed distance in mm per tooth per revolution. Be careful, there may be an inch equivilant.

The parameter Vc (AKA speed) is usually defined as surface speed of the cutter in metres per minute.

I cannot vouch for that particular chart, it came off the internet.  :killcomputer: :zap:

I still treat all of these feed/speed charts with caution. Use them for guidance (an indication) only. Our model making machines are no way as rigid as an industrial machine so we cannot drive them as hard or expect to achieve the numbers on the charts. Certainly HSS cutters need to run at much lower feeds and speeds to the carbide cutters, as indicated by the chart. The reverse is probably why I had so much trouble when I started using carbide tooling, I still used the same low feeds and speeds as for HSS, which was a mistake. Carbide thrives on higher speeds and feeds, It realy comes into it's own with very small Ae (AKA width of cut or step-over) values and very high feed rates and high spindle speeds

The rest is up to you to experiment.


Mike


« Last Edit: October 14, 2021, 04:26:57 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: 8491
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #49 on: October 14, 2021, 04:40:19 PM »
Hoffman may only give steel cutting speeds for that cutter as it is not an aluminium specific one, you could try looking to see if they have high helix ones for aluminium.

My rule of thumb is 30m/min for HSS and 100m/min for carbide when machining steel.

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3057
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #50 on: October 15, 2021, 07:09:37 AM »
Mike, Jason I am waking up this morning still surrounded by the light darkness of the jungle and the minefield direct in front.
But suddenly there is a small path through it direct in front of me.


It seems that I have no understood the information, given by company Hoffman which is there for each cutter at their web site.
Also here, with my 5mm HSS 3 flute cutte, is the specific chart like in picture #1 shown.
I have seen it before, but was not able to understand the numbers.


Now I have recognized, that by using the cursor and keep it at a specific place over the chart an explanation will appear, like picture #2
So the numbers should show the unity m/min, what could be in my understanding information about Vc=cutting speed (Schnittgeschwindigkeit)
That means the supplier recommendation Vc for Aluminium for this cutter is 83 m/min.


If I enter this Vc into the Fusion tool libary (second line from above), it calculates a spindle speed of 5284 U/min, first line.
Inserting Fz=0,02 mm chip load (Vorschub pro Zahn, second line second box) a calculated feed rate (Schnittvorschub) Vf=317,04 mm/min is calculated there.
This all seems to be logical for me now.


Given the same figures into the Sorotec calculator shows nearly the same.
We have to ignore the two red crossed information, because by our theories so far, it will give optimal information about carbid cutters only and not HSS.


The picture is getting clearer for me now about this professional figures and calculations.


Still a miracle, why does my HSS cutters going like hell with much high speed and feed rates without any problem so far ?
 
 
 
Kind Regards
Achim

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3057
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #51 on: October 15, 2021, 07:34:30 AM »
Spindle test  continued again.
Testing a chamfering with a 6 mm, 3 flutes, 90░ carbide tool was my next action.
The mostly used sector of the cutter is nearly 3 mm in diameter.
The Sorotec calculator was fed with the data of a 3 mm, 3 flute cutter.
Used cutting data for this operation:
N=20.000 U/min
Vc= 377 m/min
Vf= 1.500 mm/min
Fz= 0,025 mm
Ae and Ap a bit only for chamfering
The result nearly fine, some minor chatter was there, may be next time some reduced values may help and a thinner chamfer will surely help for better results. 
Kind Regards
Achim

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8491
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #52 on: October 15, 2021, 07:41:46 AM »
That's around what I said back in post #8 "If I had the top speed of your spindle I would be at 8-12 thousand rpm with Carbide and 5-6 for HSS"

Your cutter will work at the higher speeds but it may not do so for very long as there is a risk faster wear which then causes overheating of the HSS and also an incresed risk of aluminium welding itself to the tool.

To make the most of your new spindle it would be well worth moving away from HSS and changing to Carbide at least for the most commonly used cutters at first and then slowly replace the rest as and when they become worn. Before I got the CNC I only had 2 or 3 carbide cutters the rest all being HSS for use on the manual machines now if I open the draw under the CNC just about all are Carbide as they allow me to feed faster even with my slower spindle speed therefore keeping run time as short as possible while also lasting longer and there is not that much difference in costs at the smaller <6mm sizes

It does not look like Sorotec do 3-flute cutters so you may have to look elsewhere, I have tended to mostly by these as just likes Mikes calculation you can run them 50% faster than 2-flute and I would be at 5-600m/min feed with my 5000rpm spindle in aluminium, with the fogbuster you should be able to keep up with chip removal when you are at a similar feed per tooth but using 15000rpm of 1500-1800mm/min on the adaptive cuts of 0.1-0.15D. I also leave my infeed and outfeed at the same speed as the cut so you can gain a bit of time there too.

J
« Last Edit: October 15, 2021, 07:51:44 AM by Jasonb »

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3057
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #53 on: October 15, 2021, 08:37:47 AM »
Jason, it is exactly as you mentioned it.
At my very first beginning, I have bought some Chinese cutter in Luxembourg.
At the conventional mill it was a nightmare already, you did never know what you get.
So I have made a decision there only a reliable source will solve this problem. 
That was the reason to swap to Hoffman as a cutter supplier.
And as you said, there was no reason to buy carbide cutters for my 2.900 U/min revolution speed with the Optimum BF20L mill.
Starting with the CNC mill in 2013, there was the Proxxon motor with 2.500 U/min so no need think about other cutters also.
When the higher speed time started in November 2019, I have used for milling what was under the bench, so far without any real problem.
Now I have learned some more about the usage of CNC milling for model engines, I agree it would be a good idea, to keep the remaining HSS cutters for the conventional mill. Some Carbide/VHM ball cutters and chamfering tools are available already.
Also a nearly complete set of VHM short drills with 1/8" shaft for CNC usage only are available since a longer time now.
These are really very helpful at the cNC mill, but don┤t try to use these the conventional way.
I did one time for 2 second only, than it was broken.


Sorotec does offer a coated and uncoated 3 flute cutter, Hoffman does offer a very wide range of 3 flute VHM cutters, so it will be no problem to find the right series for replacement and CNC usage only.
Kind Regards
Achim

Offline Vixen

  • Full Member
  • *****
  • Posts: 2546
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #54 on: October 15, 2021, 10:27:02 AM »
Achim, Jason.

I have found this discussion most interesting and helpful. I feel I now have a much better understanding of how to get much more out of carbide tooling. I had always been too timid, keeping the spindle speed and feed rates low, as is appropriate for HSS tooling. These discussions have shown us all, how carbide tooling thrives on higher speeds and faster feeds and has encouraged us to experiment. For me, the biggest breakthrough was in understanding the enormous advantages of very low 0.1 D    Ae (step over) values  . The work required to peel off a thin wafer is so much less than for a conventional chip. Now, I am able to create deeper pockets, in one pass, than ever before.

I am now able to remove material at a much fast rate, that chip removal has become important. Before, blowing down a plastic tube was enough, now I need to consider something better. I have tried using my old compressor and blow gun. The compressor was far too noisy for continuos use, besides the pressure was too high and the chips were blown everywhere, so I went back to usng the blowpipe.

Jason, you said something a while ago, about buying a new low noise compressor. Was that just for your CNC work, does it have the capacity (pressure and flow) to run normal compressed air tools as well. I'm thinking mainly of the bead blast cabinet. So what pressure do you use to clear the chips on your CNC? I think you said you had some form of lube fogger. Perhaps you could remind us of that device at the same time.

Pleased to have accompanied you both on the journey of discovery,

MIke
It is the journey that matters, not the destination

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

Offline Admiral_dk

  • Full Member
  • *****
  • Posts: 2789
  • S°ften - Denmark
Re: CNC mill spindle up grade
« Reply #55 on: October 15, 2021, 11:26:19 AM »
Gentlemen - it has been very informative for me too, and very likely more people around here  :cheers:

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8491
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #56 on: October 15, 2021, 12:56:31 PM »
I'll post about the compressor etc over the weekend, probably put it in a new thread as this one has drifted away from the spindle upgrade. Hopefully Achim will add something about his fog buster and the superior pumped versions that Sebastian End has developed.

Will also add a bit more here later.


Offline fumopuc

  • Full Member
  • *****
  • Posts: 3057
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #57 on: October 15, 2021, 02:00:35 PM »
Mike, Jason, thanks for this, for me a very much useful discussion about cutting parameters.


Here is the link to my compressor up grade end of 2019.
https://www.modelenginemaker.com/index.php/topic,9436.msg210907.html#msg210907
Really silent and for the constant usage with my fog buster system very well suitable.
Seems to be Chinese and available at every corner under different brand names.
Still available for EUR 379,00.


And yes, it is still really silent, today also.
« Last Edit: October 15, 2021, 02:29:12 PM by fumopuc »
Kind Regards
Achim

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8491
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #58 on: October 15, 2021, 06:59:12 PM »
The other advantage of Carbide over HSS is that it is a stiffer material so that for the same diameter of cutter you can take a heavier cut be that in Ae or Ap without as much tool deflection and/or risk of chatter. So even if you don't have the fastest spindle speed to run it at it's optimum speed you can still take more off in a single pass than you could with the same size HSs cutter provided the rest of the machine is capable.

I don't know if you have seen this guy's video's who is from your part of the world but he uses quite a lot of Hoffman tooling and gives all the cutting data which may be of interest. We can only dream of having a machine like his but at least the purchase of a cutter or two is possible for us hobby users. He also has an interesting way of almost removing the part from the clamped block of metal.

https://www.youtube.com/c/BavariaCNC/videos

Offline fumopuc

  • Full Member
  • *****
  • Posts: 3057
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #59 on: October 16, 2021, 07:40:03 AM »
Jason thanks for the link. I didn`t know this canal before.
It is pure industrial milling so not something what really attracted my attention so far.
But with today's knowledge sure good to have a peek.

I have skip my slot experiment with  the spindle testing yesterday, which was done before chamfering.
Purpose was to mill a simple slot, not a pocket to see how it will behave and if it will affect the surface.
The milling strategy slot was selected, what means the cutter will follow a slot line, it doesn┤t matter which size the width is.
So if the slot is 5 mm in width, than also 6 mm cutter can be selected and he will follow the slot contour.
Here the CAD model say 5 mm width and I have used the same 5 mm cutter as the hole time before.
cutting parameters:
N= 18.000 U/min
Vc= 283 m/min
Vf= 2.000 mm/min
Fz= 0,037 mm
depth of the slut 2 mm.
The selected tool plunging into the material is shown in the first picture.
It works fine, visible as usual a little mark, may be that is effected by some flexing.

The final 2D test was an engraving.
The tool a 1/8" Carbide/VHM graver 36░ and 0,5 mm tip.
Cutting parameters:
N= 20.000 U/min
Vc= 199,5 m/min
Vf= 1.000 mm/min
Fz= 0,05 mm
ap= 0,15 mm
This has to be told Fusion by adjusting a negative "stock to leave".
It is a bit tricky here, because for making a single line engraving  the Fusion engraving strategy is not the right tool.
Engraving in Fusion means to remove material between to lines.
If a single line engraving should be done than trace is the right strategy.
Trace will follow a line and the depth has to be adjusted with the negative stock to leave input.
If I see the result, than selected speed and feed seems to be fine for Aluminium.
This tool is my one and only and used ( perhaps misused) already some time, so may be not in best conditions anymore.

For some 3D machining testing I have made the decision to mill the female torso again.
With all the just learned I will rework the hole machining process.
The higher Ap and lower Ae strategy will be used, also a complete revised order of the single operations.
A good opportunity to recheck and rework my tool library concerning the new spindle shape and speed and feed rates.
« Last Edit: October 16, 2021, 12:32:08 PM by fumopuc »
Kind Regards
Achim