Thread: It's begun....
Ah yes DOC - I tried a 1mm and 3mm DOC and its 6082 T651 Ali
Try 1mm @ 800mm/min 10,000rpm and take it from there.!!. . . . I cut @2.5-3mm Doc @800mm/min 9-10,000 rpm 8mm 3 flute ripper using blown air.
Each machine is different so you'll need to play with settings to find the sweet spot for yours. If you push too hard to start with you'll just cause premature wear and possible damage machine so start off easy with DOC and Feed rate then use the Feed override to change feed rate on the fly while cutting, also play with spindle rpm has well.
By doing this you'll find the sweet spot quicker and get the best finish and tool wear.
I thought that was a little aggressive - I'm not too fussed about the length of the job (or at least won't be once I have my mist working and don't have to stand there puffing WD40 at the tool and brushing chips away for hours). I'll report back with results and must get some pics or video up.
I finished cutting my first part today after a bit of trial and a fair bit of error.
The part was a replacement gantry mounting bracket, which I had hand cut originally and thought I would get something a little more precise on the machine. I am using 15mm thick 6082 T651 Ali.
Firstly I quickly ran up the part on Vectric's Cut 2D and placed 8x5mm through holes to fix to the bearing blocks and 4x6mm holes with 4mm deep and 11.5mm dia counterbores, which fix to the bottom of the gantry. The previous mishap when drilling holes in extrusion meant I was out of 5mm carbide end mills, so opted for a 4mm carbide 3 flute which was running at 18,000 rpm 0.5mm DOC, 750m/min feed and 515m/min plunge (these were suggested by GWizard). The cuts were inside edge profiles, so spiral cutting.
This operation ran fine with no mishaps.
Then I modelled an outside profile cut to cut the part from the plate, using a 6mm end mill and tried 10,000 rpm, 0.8mm DOC, 750 m/min feed, 515 m/min plunge.
This ran fine until it got to ~10mm into the material and then the tool bogged down (probably on chips), went a little hysterical where it was stuck and before I could hit the estop. Once I had bought the spindle to a rest I figured it was another stepper/driver glitch and looking at the tool it appeared to be fine with no gummed up ali on it. So I rewound the job and started again. This time, once the job had reached material it ran fine for a couple of cycles and then again bogged down, and jammed, then snapped the tool.
I was using WD40 every so often and also using my airbrush to try and clear the chips, which was only partially successful and looking back on it I reckon the tool got bogged down in chips in the slot and this caused the jam/snapped tool.
So I figured I would tone stuff down and with Jazz's advice on feeds and speeds in previous posts, tried again with an 8mm end mill and this time used the airbrush exclusively, with some coolant to act as a mister. I also reran GWizard and with this time tried 12165 rpm, 0.2mm DOC, a 750m/min feed and 250m/mm plunge (although this time I opted for a ramp rather than stright plunge). I found the conservative/aggressive slider this time in GWizard and went for the former.
This time the job completed without mishap, but I do need to do a few things in the future and the first of those is to rig up the airbrush/mister so its on constantly rather than me chasing the tool around and trying not to tangle the airline from the compressor.
I do have chatter lines on the sides of the job, so I think I will have to bite the bullet and retro-fit a second ballscrew on the x axis, which should help with this.
I did a quick check over of the machine when I was done and the X and Y locking nuts had come loose. Not sure the set screws/grub screws are man enough for the job. so will have to think about solving that as I don't want one of the ballscrews breaking free or breaking the coupler. I was thinking about replacing the helical cut ones with the interlocking kind (don't know the name for them but have seen them on various sites).
Also my PC is far enough away from the machine that its a pain to have to keep going backwards and forwards if I want to feedhold and restart, but I'll likely live with it until I move home in the next week or so.
Once I have got a better hang of feeds and speeds and the new ballscrew in I think I'll have a go at cutting some gantry sides out of plate as well, although I'm eager to have a crack at something not fo rthe machine itself....
More to come...
0.2mm DOC is disappointing. 12165rpm sounds a bit fast for an 8mm carbide cutter in aluminium. I use around 9800rpm (600mm/min, 1.5 DOC,8mm single flute). Looks like that was a 3 flute cutter since you've set the plunge to a third of feedrate which is what Gwizard suggests? If so then 750mm/min is slow, you wont be getting a big enough chipload. Use more like 1800mm/min if it's 3 flute.
If you want a quick way of guessing the feeds and speeds then scale it proportionately off one you know works. For instance I know that 9800rpm, 600mm/min, 1.5 DOC works well with the 8mm single flute, so if I used a 2 flute cutter I would just use twice the feedrate (1200mm/min), as its got twice the number of flutes and maybe decrease the depth of cut to reduce the force on the cutter. Using that logic, your 4mm 3fl should be run at 19600rpm and 1800mm/min...clearly this isn't the most accurate way to determine the settings, but it's a good start.
Sounds like you're describing and oldham coupling. They're pretty good, but you should be able to mount the motor accurately enough to use a solid coupling.
You could try using a finishing pass to eliminate the chatter marks - just take off 0.1-0.2mm at full depth.
Thanks for the feedback Jonathan,
I went a bit shy on the DOC on the 8mm, after breaking the 6mm earlier and you're right it was 3 flute. I have the other mounting bracket to do tomorrow, so I'll pluck up the courage to up the feed rate, but I'm a bit wary of the sturdiness of my machine until I get that 2nd ballscrew on, so maybe a lighter DOC than 1.5mm (that and get an order in for more end mills ;-) ).
Another thing I need to figure out is an estop for the spindle/VFD and two pole that into the big red button for the control box.
For these pieces I'm not fussed about the chatter marks, they were quite light anyway, but a finishing pass will be in order for the other parts I'm making.
Solved my locking nut problem by binning the supplied M4 grub screws and chopping some M4 button head bolts to size (they had hardly any "hex" on the head and seemed to be made of silly putty). Ah yes Oldham Couplings - will go find some now.
Since my last update I've been doing some research on feeds and speeds and trying to understand the relationship between the two (amongst all the other variables).
I've used GWizard and also FSWizard to compare results and tried to compare to the advice I've had and I certainly need to use 2 flute (or even single flute) cutters to bring the speeds and feeds down (ordered a bunch and they should be here Monday or Tuesday).
Also I am a bit mystified on one thing: HSS vs Carbide end mills - Carbide F/S results from the wizards above seem to be way way higher than HSS and I know that carbide is alot stiffer, but do the carbide end mills actually need to be run at the multiples higher than HSS given the same geometry should result in the same chip loading? Or is there some other factor I'm not grasping?
Off to try and make a mount for my airbrush/mister :-)
Just gone back and looked at the first post in this thread and I see the basic frame but can you post pics of the finished machine.?
Reason I ask is that you mention single screw and from the pic I'm thinking you must just have it down one side and not central to the gantry.? If I'm correct then your wasting your time using any calculator has the machine is so compromised with this set up they will be massively off target. Esp in aluminium.!!
EDIT: scrap that request looked a bit further up and found it.!! . . . Give it up untill you have the other screw you've no chance.!! It will turn into another beast with 2 screws.!!!
Looking at the machine and it's stubby size and strength then with twin screws it will easily cut aluminium with 3 flute cutter at 2.5mm DOC and 1500mm/min or more.
My machine is much wider and I easily cut at these figures and just today using 8mm size of this cutter (E5711 series) http://www.cutweltools.co.uk/files/ww/SM%20A160.pdf I was playing with DOC and cutting at 5mm Doc @900mm/min 9-10k rpm full slot without any trouble what so ever. I will try even deeper with 45% step over when pocketing and the tool spec says ok upto 1.5 dia @700mm/min 8K rpm.
HSS or carbide is mainly down to strength and the fact Carbide tends to work better when loaded up and can handle much greater heat and forces. To be honest I find I get better finish from HSS in Alu and actually prefer to use them for jobs where don't want to apply finish pass. With Carbide I can hog away put always have to do a finish pass for an acceptable finish.!
Last edited by JAZZCNC; 09-12-2012 at 04:00 PM. Reason: wrong link
Yeah I figured the single x axis ballscrew was causing weakness - I'll get a mail over to Chai for a new ballscrew with appropriate machine end and go the pulley/belt route (seems less prone to error than two steppers). I'm looking at Zapp/Gary for the belt and pulleys if I can decipher what length belt to order (whether the length is for the whole belt or the loop if folded in half - if that makes sense).
As always thanks for the sage advice and assesment of the machine once its been upgraded (I like the sound of "beast" :-) ).
The machine will be a beast at this size and strength. To give some idea my machine Y axis travel is 1100mm, so technically more likely to be weaker or more flexy than yours.
Smack bang in the centre at 3/4 Z extension so possible 120-130mm extension below Z axis. I've just cut a oval pocket 70mm x 30mm length single pass at 8mm Doc 45% step over @800mm/min 12Krpm in 6082 T6 Aluminium just using blown air no misting or coolant(quick initial squirt of WD40).
In doing this, it first spiralled down to depth, it then had to cut full slot for about 40mm and while it moaned slightly more than the when cutting 45% stepover it still handled it no problem and the actual 45% stepover was a doddle and I'm sure I could have easily pocketed at 45% step the full 10mm depth of material.
While bit extreme on DOC and not something I do often at full slot width. I Can't see why your machine couldn't do this kind of cutting and like mine will most certainly easily handle half this DOC at higher feeds.
BUILD LOG: Web Goblin cnc has begunBy Web Goblin in forum DIY Router Build LogsReplies: 147Last Post: 12-02-2012, 07:49 PM