Welcome to ModelEngineMaker !If you have problems registering or logging in, please use the contact menu option to request assistance.
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 Kim
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!
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 HSSlooks a nice spindle and should be better and quieter than the more router based one you had before.
But it was working well so I continued, without changing the program.
As I often use a router for woodworking I can understand why you would want to move away from that as I would not want to be using it for an extended period of time even when wearing ear protection, the KX3 is not bad and you can easily have a conversation next to it when at 5000rpm. The was a member over on ME forum who won a Shapeoko gantry type machine and he found it very noisy with a Dewalt router and as there was not much speed control had to use small diameter cutters to avoid overspeeding at the cutting edge which just made the noise worse.Like Mike I am limited to a 5000rpm maximum speed which with my usual 6mm dia cutters is OK with steel and cast iron as I can run at the right sort of speeds of 4-5K rpm but I am not fast enough to get the optimum speeds for aluminium of smaller diameter tools.I do try to run at the makers or suplliers suggested spindle speeds where I can but our less powerful and less rigid machines mean the feed rates and to some extent the depths of cut have to be adjusted to the individual machine. I tend to mostly use 0.02mm per tooth (Fz)in steel and cast iron and 0.03-0.04mm/tooth (Fz) in aluminium depending on whether there are any tight internal corners where I will run slower as the cutter engagement is higher and a risk of chatter,So for a carbide 6mm dia 3-flute cutter with a 0.03-0.04 Fz at 5000rpm I would be feeding at 450-600mm/min which is actually not that different to your figures as at 18,000 that would be 1800-2160mm/min. However if it were an HSS cutter I doubt I would want to run it so fast and my 5000rpm would be about the max I would take it to even if I had a faster spindle. Just looking at my YG-1 catalogue for s 3-flute uncoated HSS-bo at 5mm dia they suggest 6300rpm for both slotting and side cutting and the other supplier I use a lot suggests 7000prm which is what made me ask about your chosen speed. Your Fogbuster will help with the speed and is something I still have to sort out though I do now have a better compressor.I can't remember what your mill started life as but that will have the biggest effect on how much you can take off, I would tend to take heavier than you have shown here typically with the usual 3-flute 6mm cutter for the first surfacing I would be 1mm deep and say 5mm wide. Then for adaptive the numbers would be 6mm Ap height x 1mm Ae stepover. I may alter this to suit the job but would tend not to go much over that "area" of metal removal so may also use 12mm Ap and 0.5Ae for example. I tend to leave 0.3mm radial on these cuts and then do a finish contour with one roughing pass of 0.2mm Ae and finish pass of 0.1mm Ae.The bit of your cut that I gave ringed does look a bit "ugly" could it be that the fogbuster is nor reaching the back of the tool?I really need to sit down wit ha big block of 6082 and just try a few more variables out to really see what my machine can do. What I detailed above it is quite happy with and does not sound under any strain plus I can keep up with clearing the swarf and brushing on some lubrication, no doubt it could be pushed harder but as I only use it a few times a month am happy to stick with what I have found works, it would be different if I had a batch to do or was using it several times a week. No doubt you will go though a similar process with the new spindle to find out what works best on your setup. It's all good fun.
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.
The fz values (tooth feed in mm/ tooth/ revolution) are coming from this chart.https://webseite.sorotec.de/download/fraesparameter/schnittwerte_en.pdfThe 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.
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)
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.
It's interesting to compare the Hoffmann and Guhrung information.
Have you tried lower Ae values yet?Mike
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
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
Hi Mike, good to know that your experiment was so successful..............To clarify for the future is this speed issue for HSS cuttersIs 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.
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.[youtube1]https://youtu.be/FxdaV9fjsdo[/youtube1][youtube1]https://youtu.be/tvnde64xjcU[/youtube1]I've been having a play and "peeling" at 1000m/min, video later