Model Engine Maker

Supporting => Tooling & Machines => Topic started by: fumopuc on September 25, 2021, 06:34:51 AM

Title: CNC mill spindle up grade
Post by: fumopuc on September 25, 2021, 06:34:51 AM
Hi everybody,
end of 2019 I have done the first step and replaced my original Proxxon FF500 spindle motor by a high revving mill motor, how is its common in wood working from Mafell.
Here (https://www.modelenginemaker.com/index.php/topic,9435.0.html) the link to this older posting. I have been very happy with the possible high revs up to 24.000, specially for milling aluminium and brass.
I have been not so happy with the noise and the power and torque.

After checking the market, I have found the Teknomotor 1,1 KW HF spindle, which could be the step in the right direction. So, a quick sketch was made in the CAD to see the overall integration also in relationship to the movement of the table. A bracket had to be designed to adapt the new spindle to the mill also.
From the electrical and electronical side, an electrical cabinet was necessary to run it with 3 phases 220 Volts. Also here was the CAD check very helpful to select the right cabinet size. Space for a line filter, a switching power supply 24 Volt and a relay, the frequency converter and a brake resistor have to be found. I was a bit of a long-time project, but now the Hardware is installed and the cabinet has found its final place close to the mill now. Space is rare in my little shop under the roof.
Here the first test run with a minor adaption of the EdingCNC software to control the spindle correctly by a 0-10 Volt signal, originally given by the G-Code now in future. What means at the other side, the right speed has to be defined now always proper in the CAM, so the programmer has to work there carefully now.
Next to do, the assembly of the bracket with spindle at the mill and to find the best way for the moving orange cable.   
YuXEvcWJVRA

PS : I am heavily struggling with the text editor today. Nearly impossible to post anything.
Title: Re: CNC mill spindle up grade
Post by: Vixen on September 25, 2021, 11:21:43 AM
Hello Achim,

Fitting the Teknomotor to the mill looks like the easy bit, compared to making the electronics installation. I am impressed with the way you have made such a neat installation in the cabinet.

We have a saying "It looks like a bought one" and your installation looks very professional.

Please can you explain how you did the G-code to 0 to 10 volt signal conversion. Did you use an interface card, or was it achieved within the EdingCNC software?

Keep us posted with progress. Waiting for the first chips to be made.

Regards

Mike

Title: Re: CNC mill spindle up grade
Post by: fumopuc on September 25, 2021, 06:54:08 PM
Hi Mike,
the EdingCNC software can recognize the speed information in the G-Code.
This will be translated inside the EdingCNC into the 0-10 Volt signal, what is activated now.
Concerning the electrical cabinet, I have had some professional help.
A the very beginning, I have recognized that all this small bits and pieces for a proper assembly and the wiring are not available in my shop.
Everything is available online in the net and easy to order, but i.e. for the need of 0,3 meter cap tail, you have to order minimum 1 meter plus the freight charges.
All these added was together much more, than let the assembly job done in a shop, where everything is available of the shelf.
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 08, 2021, 06:53:19 AM
Hi everybody, successes with my spindle up grade.
Everything seems to fit mechanically nicely.
I have swapped the Mafell against the Teknomotor with bracket.
I won a bit of z height, nearly 15 to 20 mm, by this design.
Followed by a tramming procedure.
The software (EdingCNC) had to be fed with the information about the new position of the lower end of the ER20 collet.
Also position of tool length sensor and collet had to new adjusted in the software.
The 3D printer was very helpful to fit the wire and to store new equipment for the mill now.
The test piece for first milling operation is in the CAD now and the CAM will start its work now.
   
 

 
Title: Re: CNC mill spindle up grade
Post by: Kim on October 08, 2021, 05:36:24 PM
A very tidy upgrade there, Achim!
You're 3D printer did you proud!  I'm going to have to get me one of those someday :)

Can't wait to see what parts you make with your new CNC spindle  :ThumbsUp:
Kim
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 09, 2021, 07:27:48 AM
A very tidy upgrade there, Achim!
You're 3D printer did you proud!  I'm going to have to get me one of those someday :)

Can't wait to see what parts you make with your new CNC spindle  :ThumbsUp:
Kim


Hi Kim, thanks for watching.
After I have learned to do my things in a CAD Program, there was no reason anymore  for not using a 3D printer.
Before I was a bit discouraged, because the printing of some Chinese dragons from a set up CD was not what I have had in my mind.
In the meantime I am very happy with it, an a lot of, for me useful, items are made.
Not for the shop only, also in the  garden or anywhere else in the house.
 
 
Title: Re: CNC mill spindle up grade
Post by: Kim on October 09, 2021, 04:40:16 PM
Wow! Such a tidy shop, with 3D printed holders for everything. A place for everything and everything has its place.
I'll have to say, my shop isn't quite as tidy.  I'm more of "A pile for everything and everything has its pile" type of shop! :Jester:
Thanks for the inspiration!
Kim
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 10, 2021, 01:34:22 PM
Hi everybody, now it was time to get some swarf all over it.
I have made a test part in Fusion360, which should give the possibility to check as much as possible of the known 2D CAM strategies.
Than I had to define a basic spindle speed for new coming feed rates.
The below graph from Teknomotor shows, that at 18.000 revs the torque starts to drop down a bit.
So my decision, when ever possible, 18.000 revs is the speed to start with and adjust the feed rate in accordance to this.
The material of the test piece is a 7075 aluminium, the tool for nearly all is 5 mm, 3 flute, HSS Co8 cutter from an industrial German source.
First test was a face milling.
18.000 revs and a feed rate of 2.000 mm/min. Mist cooling as always. For me the fastest ever used feed rate.
ae 2,5mm and ap 0,5 mm.
Chips are flying around my ears and after some seconds it was over already.
The result in my eyes perfect.
Next one, a kind of trimming around the whole part.
So one time around the part, ae 0,5 mm and ap 2,5 mm, same speed/feed as above.
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 10, 2021, 02:18:47 PM
That sounds quite fast for and HSS tool of that diameter, I will be interesting to see if tool life suffers. You say it is a commercial grade cutter so do the makers give any suggested cutting data? If I had the top speed of your spindle I would be at 8-12 thousand rpm with Carbide and 5-6 for HSS

looks a nice spindle and should be better and quieter than the more router based one you had before.
Title: Re: CNC mill spindle up grade
Post by: steamer on October 10, 2021, 02:42:05 PM
Nice neat and orderly storage is soooooooo  nice to have.   I'm glad you put the effort in to build that, I know how convenient it is to have everything at arms reach!    :ThumbsUp:  :ThumbsUp:
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 11, 2021, 06:23:49 AM
Nice neat and orderly storage is soooooooo  nice to have.   I'm glad you put the effort in to build that, I know how convenient it is to have everything at arms reach!    :ThumbsUp: :ThumbsUp:


Hi Dave, thanks.
My shop is really very small, more a kind of a box under the roof. So if I start to search anything, I have lost already.
I like it to have a fixed place for (nearly) everything.
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 11, 2021, 07:16:15 AM
That sounds quite fast for and HSS tool of that diameter, I will be interesting to see if tool life suffers. You say it is a commercial grade cutter so do the makers give any suggested cutting data? If I had the top speed of your spindle I would be at 8-12 thousand rpm with Carbide and 5-6 for HSS

looks a nice spindle and should be better and quieter than the more router based one you had before.


The spindle is fantastic, very, very quiet and with enough power for my model engineering jobs.
I am really happy that I have done it, it was a kind of long term decision.
The speed of the Mafell before was O.K., also it was good to start the high speed milling learning curve with it, but the noise and vibrations was always an issue I didn´t like very much.


How long the cutter will last here ?
No idea, it is a used one, already more than 6 month in use, o.k. not every day.
Here the product information (https://www.hoffmann-group.com/GB/en/houk/Mono-machining/HSS-milling-cutters/Slot-drills-HSS-Co8-uncoated/p/191200-5?wayIntoCart=PDP&tId=#anchor_applicationTable) from the supplier.
He recommends

Feed fz for slot milling in steel < 750 N/mm2                                                                 0.008 mm


 For me this is not very helpfull, because it is a kind of upper limit, worst case, for this cutter.
I don´t do any slot milling here in steel.


I prefer a little tool, calculator since some years to see how the cutting data could be.
I can choose here first  the material.
Next step the cutter diameter and the number of flutes all in the first line.
The second line in the box below, shows the optimal calculation result for the input of material, cutter diameter and flutes.
In this case n=31.832 rpm, far away of what my spindle is able to do.
So now the first line in the box can be adjusted.
In my case I adjust the max rpm to 18.000, an a new calculation has to be made.
Result shown by the next picture.
This calculator is sure not made for big industrial machines, because as you can see in the last line, it recommends a max depth, ap, of 1 mm if used in slot milling.
And of course the given selection of material is not complete, but for me it gives me a first idea about were I am. 
There is another information (https://webseite.sorotec.de/download/fraesparameter/schnittwerte_en.pdf) available which was very useful for me to nearly understand the relationship in cutting data calculation.
That´s the way how I try to find my way through these jungle.
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 11, 2021, 07:43:35 AM
I'm off out now but will get back to you later,
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 11, 2021, 08:41:01 AM
Hi everybody,
next test to do with the new spindle, an open pocket.
2D adaptive cleaning.
Same speed and feed, ap, I have been more courageous as usual, 2,5 mm and ae 2 mm.
The result looks a bit ugly and starts to get "greasy" ( no idea if it is the term for this light floating material) , but for roughing out may be still o.k.
There is still 0,2 mm over stock for a cleaning operation.
Title: Re: CNC mill spindle up grade
Post by: Vixen on October 11, 2021, 12:27:48 PM
Hello Achem,

I am following your adventures into high speed milling with great interest. I am also exploring adaptive machining etc. I am currently limited to a 5,000 RPM spindle.

I agree with you, the adaptive clearing marks are a bit ugly to look at but they are more visually noticeable than measurable. I find a additional 0.002" (0.05 mm) deep finishing pass with 45% stepover improves the appearance

The Sorotec cutting data calculator (schnittdatenrechner) appears to be a very usefull addition. I have searched the Sorotec online shop but cannot find any reference their cutting data calculator. Please can you help me find it.

Cheers

Mike
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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  (https://webseite.sorotec.de/service/downloads/)

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



Title: Re: CNC mill spindle up grade
Post by: Vixen 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
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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 ?
Title: Re: CNC mill spindle up grade
Post by: Jasonb 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.
Title: Re: CNC mill spindle up grade
Post by: Vixen 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
Title: Re: CNC mill spindle up grade
Post by: Jasonb 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 (https://www.shop-apt.co.uk/2-flute-slot-drills-hss-8-cobalt-aluminium-series-un-coated/5mm-diameter-slot-drill-2-flute-for-aluminium-high-speed-steel-8-cobalt-un-coated.html) 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.

Title: Re: CNC mill spindle up grade
Post by: Jasonb 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.
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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 (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]


Title: Re: CNC mill spindle up grade
Post by: fumopuc 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 (https://www.shop-apt.co.uk/2-flute-slot-drills-hss-8-cobalt-aluminium-series-un-coated/5mm-diameter-slot-drill-2-flute-for-aluminium-high-speed-steel-8-cobalt-un-coated.html) 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.   

Title: Re: CNC mill spindle up grade
Post by: fumopuc 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.
Title: Re: CNC mill spindle up grade
Post by: Jasonb 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.
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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.
Title: Re: CNC mill spindle up grade
Post by: Vixen 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 (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


Title: Re: CNC mill spindle up grade
Post by: Jasonb 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.

h9q6j7POgOI
Title: Re: CNC mill spindle up grade
Post by: Vixen 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.
Title: Re: CNC mill spindle up grade
Post by: Vixen on October 11, 2021, 11:01:03 PM
Hello Achim, Jason.

Quote
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)

I think there is an answer to the Ae Ap question.

I found this on the Guhring site. It gives quidance as to how to modify Fz (chip load parameter) for different percentages of Ae and Ap.


Please Note: I have replaced the previous Guhring information with this, from the latest Guhring Catalog. The new information reflects the manufacturers latest lower Ae, higher Fz thinking.


(https://lister-engine.com/coppermine/albums/userpics/10013/Guhring_Fz_adjustment.jpg)

So, taking Jason's two examples:
For an adaptive clearance side cut where Ae of less than 0.25 D with a Ap of 1 D, use 100% Fz
For full width slot cut where the Ae is 1 D and the Ap is also of 1 D, use 25% Fz
Double Fz reductions apply to other Ae, Ap combinations

 The deep slot removes four times as much material than the adaptive side cut, so reducing Fz (chip load parameter) and hence the Vf ( the feed rate) by 25%, seems to make sense to me.

Mike
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 12, 2021, 07:17:36 AM
Hi Mike,
a very good path to follow, never seen before, because I have avoided to get deeper in there, in this industrial information.
Some years ago, I have downloaded a "Zerspanungshandbuch" from company Hoffmann, the company which sells my 5 mm 3-flute HSSCo8 cutter.
I was very new (2012) in this hobby CNC business and suddenly I was confronted with 1096 pages of industrial knowledge.
After a short time I have given up to understand anything, I was totally overloaded.
Now I have open the PDF again and found something similar as you have seen at the Gührung catalog.
Only one thing there is conspicuous.
In the actual milling catalog, can be downloaded at their homepage in English language also, there are different numbers/percentage for the ae values, than in your picture.
May be there was a revision ?
What ever, these ae / ap story is in my understanding one to one in very strong relationship to the stiffness and rigidity of the machine.
All these industrial recommendations  are far away of what I can use with my machine.
As I told before, if I use ap of 2,5 mm (0,5xD) and ae 2 mm (0,4xD) with my 5 mm cutter with a 2D adaptive cleaning operation than I have the feeling to be very encouraged.
I assume there will be no big difference, even if I will reduce the revolution.
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 12, 2021, 07:22:50 AM
The other thing to remember as the sideways Ae cut becomes deeper is the effect of "chip thinning" with a 0.1D the chip will actually be quite thin as you are almost tangental to the edge and it will be less than the chipload (feed) in thickness but with say a 0.5D Ae the chip will be at it's thickest and actually equal to the feed rate at the ctr line of the tool. So their suggestion to reduce feed as the Ae becomes greater makes sense.

Also as Ae increases so does percentage engagement, I'm sure we have all experienced that high pitch chatter at the end of a cut even on our manual machines as more of the tools circumference if in contact with the work.

F360 can even take into account tool life and I think it will reduce feed as the tool becomes worn but not something I have looked into.

Just a few more variables to be thrown into the pot that as you say a hobby user does not tend to need to look too far into but worth bearing in mind such a when doing pockets to try and make sure any internal radii are larger than the tool radius so you don't get chatter in the corners or worse weld a bit of aluminium to your tool.
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 12, 2021, 07:39:38 AM

Just a few more variables to be thrown into the pot that as you say a hobby user does not tend to need to look too far into but worth bearing in mind such a when doing pockets to try and make sure any internal radii are larger than the tool radius so you don't get chatter in the corners or worse weld a bit of aluminium to your tool.


Also 100% agreed. This is one of the very early things you recognize if you start with your CNC milling learning curve.
That was one reasons for me to declare the 5 mm cutters as a standard and upper limit  for me so far.
So a 3 mm radius can be used in most of the designs and seems not to be to big for the appearance in the models.
Title: Re: CNC mill spindle up grade
Post by: Vixen on October 12, 2021, 11:53:23 AM
Good morning guys,

It's interesting to compare the versions of the Guhring catalog information. Although the numbers differ, they both show the same trend: reduce Fz for deeper and wider cuts. That remains a usefull guideline for our hobby sized machines. I believe the latest Guhring catalog information takes into account the effects of chip thinning with very small Ae values 0.1D to 0.15D.
The chip thinning effect allows you to increase Fz significantly. Some say it is actually important to increase Fz to prevent tool rubbing at these low Ae values.

Modern high speed milling stratagies take advantage of the chip thinning effect. Adaptive milling (I still prefer the more descriptive term Peel milling) with small Ae values at the  increased Fz feed rates actulally removes material at much faster rate than normal. It does this without increasing the stress on the machine. The adaptive (or Peel) stratagy uses a constant Ae depth so does not overload in the corners... there are no corners. That means you can run the higher feed rates with little or no risk. The texture of the chips is also quite different. Normal milling produces chips, whereas low Ae adaptive (or Peel) milling produces fine needles.

Experimenting with lower Ae values and higher Fz feed rates should be interesting, it's the way they are going in industry. True, we woild be ill-advised to try and reach industrial speeds on our Hobby machines, but we can follow the general trend towards lower Ae and higher Fz.

I will lead the way. I need to machine some pockets 9.7 mm deep for the W165 gear box covers, in 6082 t6. I will use the same 7.0 mm dia carbide cutter as before. Therefore the Ap will be 1.4 D. I propose to use an Ae of 0.15 D (as before) I am going to wind the spindle speed up to max 5300 RPM and raise the feed rate to 320 mm/min for starters. LinuxCNC provides a slider to adjust feed rate while you machine. I can start with a very conservative feed rate and increase it towards 360 mm/min untill it hurts. If I have a problem, I will revert to two passes, each 4.8 mm deep; I have made that adaptive cut before without problems. I will try this in a couple of days time.

Mike
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 12, 2021, 12:01:35 PM
Spindle test continued.
As Jason already mentioned, there are some ugly faces at my test part after the roughing out with 2D adaptive cleaning of this open pocket.
The contour is showing waves and the flat bottom is not flat, there is a small step left hand side, shown in first two pictures below.

I have made an experiment with the stock to leave here also. Radial was 0,2 mm adjusted, but axial was 0 mm.
My idea was to check, is it is really necessary to do a final finishing for the flat bottom after a 2D ac operation.
In the second picture is clearly a kind of step visible.
It looks like, that the cutter is climbing up a little ramp and at the end of the pass he dropped down again before getting retracted for the next pass.
I would assume, this is problem of the machine, the Z axis is not rigid enough to avoid this.
The waves in the contour shows, that something is flexing, the cutter or the machine or may be both.

So a 2D pocket operation was prepared to do the final finishing.
Speed and feed untouched, same as for the earlier made operations.
The stock to remove alone the contour is 0,2 mm.
ae general was 2 mm and ap was adjusted by 0,1 mm.
I have adjusted a negative axial stock to leave here with -01, mm, so the cutter was milling a bit deeper as the original flat bottom data.
Not using the Fusion possibility to activate a second final pass without any adjustment of the cutter.
It does not look so bad, and the waves and steps are gone.
But lesson learned is, finishing is necessary, also for a flat bottom.

Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 12, 2021, 12:10:37 PM

It's interesting to compare the Hoffmann and Guhrung information.


Hi Mike, there is little misunderstanding coming up, my fault.
The mentioned/shown picture is from the actual Gühring Katalog, as available today at their homepage. 
Sorry for the confusion.
Title: Re: CNC mill spindle up grade
Post by: Vixen on October 12, 2021, 12:28:20 PM
Hello Achim,

OK, That's even better. The latest Guhring catalog reflects the modern lower Ae, higher Fz thinking. I will go back and ammend my previous posts to keep this data pool updated.

I also get the same machine marks and slight steps as you, even with 0.15D Ae values. Remember the adaptive clearing is a roughing pass which always needs a finishing pass to produce the flattest surface. Yes, something is flexing, perhaps the cutter and the machine. Thats inevertable with a hobby machine..... no room (or money) for a big Hass.

Have you tried lower Ae values yet?

Mike
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 12, 2021, 12:37:20 PM

Have you tried lower Ae values yet?

Mike


Hi Mike, that is my conclusion of our discussion here, lower ae may be 1 mm will be not bad.
I will take this into account next time.
My current test part is finished already, will report about it tomorrow.
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 12, 2021, 12:55:34 PM
One way you may be able to do an adaptive without the need to finish the bottom of the the cut is to play about with stay down distances and percentages which will reduce the amount of times the cutter lifts and goes back to take the next cut. More staydown can increase overall time on a larger part but not so much on our small items as it is not a lot further to take the long route back to the start rather than the direct over the top one. If you are using the free F360 then you can increase the non engaged feed so the tool moves faster on it's way back to the start much like it would if rapids were allowed.

Mach3 also lets you increase or decrease feed rate on the go as well as spindle speed which I have used a number of times if I feel the tool could cut faster or if I've got a bit too cocky.

You can work yourself into a corner with adaptive if the internal radius of the part is equal to that of the cutter and minimum cutting radius set to zero but both are best avoided to keep cutter engagement more constant. I certainly think about this now when drawing up a part where I would have had an internal radius that could be formed by machining right upto it with the manual mill I'll now make it larger or use a smaller dia cutter so it can run around the curve if possible.

The other big advantage of a large Ap is that you get to use all of the cutting  edges so tool should last longer than if you were just using the end 1 or 2mm. I think 16mm is the largest I have tried
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 13, 2021, 07:26:21 AM
Next step in spindle testing.
My test part has 3  pockets , shape of a slot with different depth 2,3,4 mm, my way to increase ap here.
The pockets are 6 mm wide, so for the  5 mm cutter it is not a slut but rather a pocket.
Fusion does offer different strategies for plunging.
Below a picture, which shows the strategies, which could be chosen.
The spiral type was my favorite her, the cutter is going down in a spiral ramp to a an before defined depth, here axial stock to leave 0,2 mm with a lower speed and feed rate.
Arrived a the bottom, a switch the the so far untouched speed and feed rate will made and the cutter will follow the contour one time around.
Picture 01 shows the result before any final machining.
Similar as at the open pocket with 2D adaptive cleaning, some flexing of the cutter could be seen in the right corner.
I have made a finishing operation to final dimensions, same speed and feed rate, but I did not get ride of these entire marking from the flexing.
Next pocket, the one in the middle, it is a bit deeper, 3 instead of 2 mm. Stock to leave again  0,2 mm.
I have reduced the feed by half now, from 2000 mm/min to 1000 mm/min,
And additional the finishing was done with an ae of 0,1 mm, so more turns has been necessary to get ride of the 0,2 mm stock to leave.
The result was much nicer/smoother.
The last lower pocket was down nearly the same way but feed rate again 2000 mm/min and depth is 4 mm here, so the ap was increased again.
Looking good, similar to the middle one.
Conclusion, the finishing with a reduced feed rate definitive gives better results, also with the ap of 4 mm, close to 1D here.
Title: Re: CNC mill spindle up grade
Post by: Vixen on October 13, 2021, 04:03:08 PM
Experimenting with lower Ae values and higher Fz feed rates should be interesting, it's the way they are going in industry. True, we would be ill-advised to try and reach industrial speeds on our Hobby machines, but we can follow the general trend towards lower Ae and higher Fz.

I will lead the way. I need to machine some pockets 9.7 mm deep for the W165 gear box covers, in 6082 t6. I will use the same 7.0 mm dia carbide cutter as before. Therefore the Ap will be 1.4 D. I propose to use an Ae of 0.15 D (as before) I am going to wind the spindle speed up to max 5300 RPM and raise the feed rate to 320 mm/min for starters. LinuxCNC provides a slider to adjust feed rate while you machine. I can start with a very conservative feed rate and increase it towards 360 mm/min untill it hurts.
Mike

Today I did that lower Ae, higher Fz experiment. It was very sucessful.

I needed to machine a 9.7 mm deep pocket in 6082 T6 aluminium for the W165 engine. I used a good quality 7.0 mm 2 flute carbide cutter. This represented a Ap of 1.38 D
I chose to use a Ae of 0.1 D. set my machines spindle speed to maximum, N = 5,300 RPM. I intially set the feed rate to 300 mm/min but quickly raised the feed rate Vf to 360 mm min.

Working backwards from    Vf = N x Z x Fz     I calculate the chip load Fz to have been 0.034; that's about 80% of the Sorotec chart.

Here is the toolpath created by EstlCAM. It's a complicated pocket having an island and two slots. The program starts by clearing the circular area to the left and then expands to clear the remainder. It finishes with a finishing pass around the outside of the pocket to remove the tiny scollops.

(https://lister-engine.com/coppermine/albums/userpics/10013/IMG_0481small.JPG)


You can see the pocketing progress in the following sequence.

(https://lister-engine.com/coppermine/albums/userpics/10013/IMG_0471small.JPG)

(https://lister-engine.com/coppermine/albums/userpics/10013/IMG_0472small.JPG)

(https://lister-engine.com/coppermine/albums/userpics/10013/IMG_0475small.JPG)

(https://lister-engine.com/coppermine/albums/userpics/10013/IMG_0476small.JPG)

(https://lister-engine.com/coppermine/albums/userpics/10013/IMG_0479small.JPG)


I was impressed. I have never produced so many chips in such a short space of time. The problem became one of clearing the chips as they were created. I used lung power and a length of 6mm plastic tube to blow the chips clear. The machining was done without any coolant or lubrication other than the occasional droplet of spit.

The machine cut the deep pocket quickly and easily. It felt like the machine was operating well within it's capacity and perhaps could  have used a faster feed rate, but discression ruled the day. As you can see the chips were long fine needles because of the shallow almost tangential cut.

Some other statistics. The overall run time was 28 minutes and the total feed distance was 9.7 metres.

The surface finish marks are more visual than measurable, but I will run an additional parallel line finishing pass with an Ae of 0.45 to clean it up visually.

Something magical happens with low 0.1 D Ae (width of cut) values. The cuts are very shallow and require comparitively little spindle energy to peel off the chip. The cutter seems to find a sweet spot which allows much higher feed rates Vf to be used, without stressing the machine. This must be the quickest way to remove material.

All in all,  very sucessful day

Mike
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 13, 2021, 05:23:36 PM
Turned out well and always satisfying when you have a big pile of chips at the end of the day.

It would be interesting to see if going to a 3-flute cutter would allow for an even faster feed yet keeping the chip load the same, the machine may have to work harder but possibly not if the low Ae means only one flute is cutting at any one time? I've tended to go for 3-flute when buying carbide cutters for teh CNC as I also like the FC-3 HSS ones for the manual mill so don't have much in the way of 2-flute tooling except for a couple of HSS aluminium specific ones that came via ARC and most of those are long series which do seem to chatter a bit. I've also gone for 4-flute ball nose cutters so I can feed them faster for 3D finishing.

Just make sure you don't go too blue in the face and pass out trying to keep pace with chip production
Title: Re: CNC mill spindle up grade
Post by: Vixen on October 13, 2021, 05:48:25 PM
Turned out well and always satisfying when you have a big pile of chips at the end of the day.

It would be interesting to see if going to a 3-flute cutter would allow for an even faster feed yet keeping the chip load the same, the machine may have to work harder but possibly not if the low Ae means only one flute is cutting at any one time? I've tended to go for 3-flute when buying carbide cutters for teh CNC as I also like the FC-3 HSS ones for the manual mill so don't have much in the way of 2-flute tooling except for a couple of HSS aluminium specific ones that came via ARC and most of those are long series which do seem to chatter a bit. I've also gone for 4-flute ball nose cutters so I can feed them faster for 3D finishing.

Just make sure you don't go too blue in the face and pass out trying to keep pace with chip production

Ha ha, I started with a cabinet full of chips from last week. Now it's even fuller  :Lol:

Working backwards from    Vf = N x Z x Fz  If you used a 3-flute cutter you should be able to raise the feed rate Vf by 150% for the same spindle speed. Wow that's flying!! Makes sense in a commercial world, but maybe not so important for model engineers.  A 3-flute cutter always sounds smoother than a 2-flute. HSS cutters need to be run at about 1/3 the spindle speed and lower feed to carbide cutters; if you go faster, you risk chip welding on the HSS.

The important lesson to take away from all this, is low Ae values, in the order of 0.1 D  are so much easier (lower stresses) on the machine, than taking the bigger cuts we are all so used to doing. Faster metal removal is a bonus.

Mike
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 14, 2021, 07:35:38 AM
Hi Mike, good to know that your experiment was so successful.
That is the why I like this forum, there is always something new, for me, to discover.
I have seen a lot a videos from, i.e. Sebastian End or others, were these Ae,Ap and Fz relationship was visible, but I have been not encouraged enough to try it.
As mentioned before, the high speed of the Mafell was already a step into the right direction, but the noise and vibrations has been more disincentive to me.
Now with the new, very gentle noise of the Teknomotor spindle, situation is complete different.


Yesterday I have started a 3D test with it already and made a revised CAM program for the female torso, which was milled in spring already with the 4th axis and the Mafell spindle. A report will follow soon.


Here first the next 2D test with the Teknomotor 1,1 KW HF spindle.


So far I have made only the very small pockets, , similar to a slut to see the general behavior.
There is not much possibility for the mill to accomplish the adjusted feed rate.
To do this better a 2D pocket in the shape of a circle was the next object to cut.


Roughing out with 2D pocket strategy and 0,2 mm stock to leave axial and radial.
5 mm 3 flute HSS Co8 cutter
Ap= 4 mm (0,8xD)
Ae= 1 mm  (0,2xD)
N= 18.000 U/min (spindle speed)
Vf= 2.000 mm/min (feed rate)
Fz= 0,037 mm (chip load)
Tool path first picture.


This was followed by a 2D pocket finishing process.
Three parameters has been changes.
5 mm 3 flute HSS Co8 cutter
Ap= 4 mm (0,8xD)
Ae= 0,1 mm  for the finishing passes only
N= 18.000 U/min (spindle speed)
Vf= 1.000 mm/min (feed rate)
Fz= 0,0185 mm (chip load)
And the additional last pass around without and changes has bee activated too.
So 2 passes to get ride of the 0,2 mm overstock and 1 final pass without any further adjustment for cleaning only.
Tool path second first picture.

And finally the result in the last picture.
I am happy with the result.

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.                                                    



Title: Re: CNC mill spindle up grade
Post by: Vixen 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.

(https://lister-engine.com/coppermine/albums/userpics/10013/2193_Cutting_Speed2C_Feed_and_Depth_of_Cut_1.png)

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

Mike
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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. 



Title: Re: CNC mill spindle up grade
Post by: Hugh Currin 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.
Title: Re: CNC mill spindle up grade
Post by: Vixen 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


Title: Re: CNC mill spindle up grade
Post by: Jasonb 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.
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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 ?
 
 
 
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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. 
Title: Re: CNC mill spindle up grade
Post by: Jasonb 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
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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.
Title: Re: CNC mill spindle up grade
Post by: Vixen 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
Title: Re: CNC mill spindle up grade
Post by: Admiral_dk 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:
Title: Re: CNC mill spindle up grade
Post by: Jasonb 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.

Title: Re: CNC mill spindle up grade
Post by: fumopuc 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 (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.
Title: Re: CNC mill spindle up grade
Post by: Jasonb 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
Title: Re: CNC mill spindle up grade
Post by: fumopuc 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 (https://www.modelenginemaker.com/index.php/topic,10210.0.html) 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.
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 16, 2021, 01:30:09 PM
I did not have too much of a problem getting the engrave to work. You need to extrude the writing so it has a flat bottom and then when doing the CAM select the edge of the letter not the bottom surface and then F360 will run the cutter up into the corners giving a nice engraved look and will automatically adjust the depth depending on the width of the letter.

FxdaV9fjsdo
tvnde64xjcU
I've been having a play and "peeling" at 1000m/min, video later :o




Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 16, 2021, 06:45:22 PM
Well with all this talk of High Speed machining I thought I would sacrifice a bit of 6082 to see how quickly I could convert it into a pile of chips.

As I have mentioned I tend to use 3-flute cutters most of the time so this was no exception and I chose an Aluminium specific one from APT with a 55degree Helix that had had some but not too much use. https://www.shop-apt.co.uk/end-mills-for-aluminium-standard-length-3-flute-55-helix-uncoated-carbide/end-mill-for-aluminium-6mm-diameter-3-flute-un-coated-micro-grain-carbide.html

They give some suggested parameters for side cutting of 13,000rpm and 1,500mm/min feed so working that back to my maximum spindle speed of 5000rpm gives a feed of 577mm/min. They don't give how large the side cut can be but most other makers seem to suggest an Ae (sideways feed) of 0.1 D so I went with this making each pass 0.6mm. Ap (vertical Depth) of side cutting seem to either be given at 1D or 1.5D so I went half way with 1.25D which equates to 7.5mm. I drew up a simple block 2" (51mm) wide with a 0.6 x 7.5mm rebate in it and produced the code to cut that at various Fz (chip load) values and simply altered my Y axis zero by 0.6mm each time to compensate for the previous cut. Once I got to 500mm/min I just used the override to increase in steps of 20% eg 100mm/min.

For the first few cuts I just dabbed on a bit of paraffin but for the 800m/min and above also turned on the air as I was having problems getting the fluid to flow with the air. and being an external cut the chips were doing a reasonable job of staying away from the cutter anyway.

At no time did the machine seem to be under any strain, there was a bit of vibration on the 450mm/min pass but that was from the chip guard rather than the cutter. I stopped at 1000mm/min as I did not want to push too much and risk metal welding to the cutter or worse. Even at the highest feed the finish was quite good for what is a roughing cut with a fine series of vertical lines that could be seen when held to the light but not felt with a finger nail.

I'm not sure how often I will run at 1000mm/min as it will depend on the job as to any increases in cutter engagement or getting the chips out if a small pocket is being cut but it is nice to know what the machine can handle.

I put video and an image of the cut surface together with the feed rate son a video, couple are not the best for focus and I also mucked up the 600 & 700 videos but there was nothing exciting to see there anyway.

HLAQzYkUdy8
Title: Re: CNC mill spindle up grade
Post by: Vixen on October 16, 2021, 08:33:03 PM
Some very impressive feed rates there Jason. Boy do those chips fly    :ThumbsUp: :ThumbsUp: :ThumbsUp:

There seems to be no limit to how high you can raise the feed rate with a straight cut.

As I said earlier, after I did my 0.1D Ae (sideways feed) by 1.4D Ap (vertical depth) internal pocket, something magical happens with very low Ae values with carbide tooling. The cutter finds a sweet spot, when it peels off a fine wafer of material due to the chip thinning effect, rather than cutting a chip. It feels as though you can keep increasing the feed rate higher and higher. However, I was not to brave as you, and never reached the high a feed rates you have achieved. Perhaps next time. :thinking:

Chip removal is so much better with an external cut than when the chips are constrained in a deep pocket. Even with an air blast, it is difficult to clear a narrow, deep pocket adequately, so reducing the feed rate gives more time to clear the chips from the cutting area. When the pocket opens up, chip clearance improves and the feed rate can be increased back to the higher rate.

I am working to improve chip clearance on my machine using a link-lock air jet, fed from a airbrush compressor. I am also working on adding some coolant/lube mist, fed from a small variable speed, peristaltic pump. I will let you know how that dosing pump works out. Not sure what fluid to use. The Jokish Solis Varo fluid that Sebastian End recommends is a bit difficult to obtain in the UK, likwise KoolMist from the States, are there any other good alternatves?

Mike
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 17, 2021, 07:48:44 AM
I did not have too much of a problem getting the engrave to work. You need to extrude the writing so it has a flat bottom and then when doing the CAM select the edge of the letter not the bottom surface and then F360 will run the cutter up into the corners giving a nice engraved look and will automatically adjust the depth depending on the width of the letter.

FxdaV9fjsdo
tvnde64xjcU
I've been having a play and "peeling" at 1000m/min, video later :o


Hi Jason, as I mentioned before, this is the perfect tool for the guys which are deeply involved in wood carving.
All these nice wooden name plates at your local pubs.
The font/letter is always like a box and the material will be removed inside it, between the lines.
For a simple "marking" or "labelling" of a part I do prefer the one line xxx.shx fonts in Fusion, which can be selected at the sketch menu already.
So no extrusion is necessary and a one line text will be visible in the model only, to be selected than by the 2D trace command.
A German idiom translated would say: Many streets will lead to Rom.
In your country the people would say: There is more than one way to skin a cat,  or similar if I am right.
   
Title: Re: CNC mill spindle up grade
Post by: fumopuc on October 17, 2021, 09:02:14 AM
First of all thanks to Jason for his experiment with the high speed milling and the video documentation.
Really nice to the chips flying.

For my further spindle test I have put the 4th axis on the table against.
A piece of the AW 2007 Aluminium bar, d=45 mm, was also still available.
The raw part size/lengths  has been a bit increased to get a safer position against the chuck.

For the roughing out I have selected the 6 mm HSS Co8 cutter again, as used in spring already.
Not as much as Mike and Jason did, but my Ap was also increased and Ae decreased.
With my HSS cutter here I don´t want to go a full risk.
Cutting parameter for this job now:
N= 14.000 U/min
Vc= 264 m/min
Vf= 1.000 mm/min
Fz= 0,238 mm
Ap= 3 mm
Ae= 1,5 mm
The 3D adaptive cleaning strategy in Fusion does make first an Ap step by 3 mm and than the cutter will be lifted up again by 0,2 mm and remove the material between the last pass and the shape of the part. This will be repeated so long until it will reach the level of the 3 mm Ap pass before.
Hopefully the picture below will make it clear.
So the Ap/Ae story is relevant here for the big 3 mm steps here only.
The roughing out toke something about 3 hours.
Much more quicker than in first time in spring.
I have never had the feeling that the mill is doing real work.
The spindle is so silent, your hear nearly the cutting noise only and this is a kind of smooth also.
The chips looking more like needles.
I have done some minor experiments with the finishing process but nothing spectacular.
By hand and with the Dremel it was a bit polishing at the end.

So I will order some VHM/Carbide  end mill  cutters next week and than start to be more encouraged for milling with 1D or bigger values for Ap if possible and reasonable for a part. 

Thanks for the journey so far.
Mike, Jason, a very interesting learning curve supported by both of you.
Back to model engines now.
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 17, 2021, 10:14:25 AM
I will have to take a look in Alibre to see if they have those single line fonts which would be easier for basic engraving. Even if not I could still add the text in Fusion onto the imported part.

Figures look good and so do the chips

I have some 20mm thick steel to profile soon so will do some test cuts on that as well though I don't think I will be attempting the full 20mm depth, at least not for the adaptive cuts.
Title: Re: CNC mill spindle up grade
Post by: Dave Otto on October 17, 2021, 04:26:29 PM
You can download some basic single line fronts from the CamBam site. Once saved to the Windows font directory they can be access by any program. I have used the a number of times over the years.

Dave
Title: Re: CNC mill spindle up grade
Post by: Jasonb on October 17, 2021, 06:22:53 PM
Thanks Dave, I'll bear that in mind if there is nothing in Alibre