Author Topic: CNC mill spindle up grade  (Read 1732 times)

Offline Vixen

  • Full Member
  • ****
  • Posts: 2305
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #30 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.




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
« Last Edit: October 12, 2021, 12:42:23 PM by Vixen »
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: 2868
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #31 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.
Kind Regards
Achim

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8056
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #32 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.

Offline fumopuc

  • Full Member
  • *****
  • Posts: 2868
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #33 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.
Kind Regards
Achim

Offline Vixen

  • Full Member
  • ****
  • Posts: 2305
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #34 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
« Last Edit: October 12, 2021, 12:30:11 PM by Vixen »
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: 2868
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #35 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.

Kind Regards
Achim

Offline fumopuc

  • Full Member
  • *****
  • Posts: 2868
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #36 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.
Kind Regards
Achim

Offline Vixen

  • Full Member
  • ****
  • Posts: 2305
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #37 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
« Last Edit: October 12, 2021, 12:45:48 PM by Vixen »
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: 2868
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #38 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.
Kind Regards
Achim

Offline Jasonb

  • Full Member
  • *****
  • Posts: 8056
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #39 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

Offline fumopuc

  • Full Member
  • *****
  • Posts: 2868
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #40 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.
Kind Regards
Achim

Offline Vixen

  • Full Member
  • ****
  • Posts: 2305
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #41 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.




You can see the pocketing progress in the following sequence.












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
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: 8056
  • Surrey, UK
Re: CNC mill spindle up grade
« Reply #42 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

Offline Vixen

  • Full Member
  • ****
  • Posts: 2305
  • Hampshire UK
Re: CNC mill spindle up grade
« Reply #43 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
« Last Edit: October 14, 2021, 05:10:22 PM by Vixen »
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: 2868
  • Munich, Germany, EU
Re: CNC mill spindle up grade
« Reply #44 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.                                                    



Kind Regards
Achim