@JohnSheak I will try to answer your questions as best I can and forgive me if I am a bit long winded in some answers…
So first my setup: These images are from my Shapeoko and it was working with the following at the time: 500x500 Shapeoko 2 with 48v 400W DC Spindle. Acme Z Axis, NEMA 17, Full metal slotted bed, TinyG going through Chilipeppr. No real mods other than limit switches and large 3D printed spindle mount VS the stock mount. Currently the Shapoko has two changes, I now run a PLanet CNC MK3/4 controller with Leadshine DSP drivers and I switched the X Carve spindle mount over to the Shapeoko and it has been a good improvement.
My X Carve is a 500 x 500 with the same full metal slotted bed, Acme Z Axis, upgraded NEMA 23 180oz motors, Planet CNC MK 3 controller with Leadshine DM442 DSP drivers, .8KW 1hp VFD water cooled spindle and lastly a chip clearance system to blow the chips out of the toolpath.
Q: have you done any stiffing mods to the gantry, if so; what method?
A: I have not yet but plan to test a system shortly which will replace the main gantry for a stiffer one.
Q: what method do you use for cam ( fusion360, cambam, other) and for output to the machine… ie your workflow?
A:I use HSMxpress currently. Might switch to FUSION360 shortly. The images above were from the TinyG and Chilipeppr. My current system has a proprietary gcode sender/interface for the Planet CNC controllers. It is basically a cross between Chilipeppr and MACH3 overall. I find it far better than either one for my needs.
So I design my parts in CAD, use HSMxpress for CAM then send the Gcode to the controller with the CNC USB controller software interface from Planet CNC
Q: what bits and sources for them are you using (bitman1, toolstoday)? what are your feeds and speeds for those bits?
A: I mainly use Destiny 3 flute bits from Drillman1 ( http://www.ebay.com/itm/381351391953?_trksid=p2057872.m2749.l2649&ssPageName=STRK%3AMEBIDX%3AIT) I also use a 4 flute 1/8" 45 degree chamfer on all the edges. I use a 1/16" 2 flute flat end mill from Drillbits unlimited ( http://drillbitsunlimited.com/ ) I also use a 2.5mm 1/8" shank drill bit for the M3 tap holes. 95% of my bits come from Drillman1 or Drillbitsunlimited.
Q: are you using a feeds and speeds/DOC calculator ( which one) and what adjustments (usual ) do you have to do when using (it). ie… as it is known you usually have to pair the speeds and DOC down a bit because most of the calculators expect that you are using a mill or HAAS…
A: 2 part answer. Part one for the OKO with the DC spindle: There is not near enough power to remotely use a calculator with a DC spindle on the OKO or the X Carve. Milling aluminum on the stock DC or an upgraded DC spindle on the X Carve or the OKO is NOT a fast process and is closer to “scratching” than true milling of aluminum. BUT it does work if you allow it enough time. The OKO and DC spindle with the 3mm Destiny 3 flute end mill did a DOC of .12mm and feedrate of about 135mm/M for the shots you see above. The 1/16th 2 flute endmill ran about .1mm DOC and around 75mm/M. Chamfer was ran around 75mm/M. These shallow DOC and slow feeds are due to the lack of power in the DC spindles and the overall weaknesses of the older Shapeoko design in relation to flex on gantry and the spindle mount. It was subject to a great deal of flex if pushed too hard and would break end mills.
Part 2 the X Carve and the .8KW VFD spindle: Yes and no for the calculator. I am using the Gwizard calculator and it is a great tool by all means, but still manages to break end mills. This is due mainly to far more aggressive DOCs though and failure to clear chips fast enough. Dry milling aluminum is NOT a good idea and it WILL bite you every chance it can. But it can be done as all my aluminum milling on the Shapeoko and X Carve are done dry. I have installed a custom chip clearance system on my X Carve to fix this issue and so far it has allowed me to come within about 85% of the Gwizard DOC and feed rates. For those wondering, I have told Gwizard that I have a .6KW spindle with a 24000 upper and 1500 rpm lower limit. I am still working to dial in the settings in relation to an X Carve as like you said, it is more suited to a HAAS style mill than a X Carve.
Above all there are three important steps for milling aluminum. One is a fully calibrated SPU mill in all axis. This means using a dial indicator to check your SPU (steps per unit) on each axis down to .001". The stock settings for the X and Y Axis rarely are truly correct due to belt tension. For milling aluminum with fine end mills this is a hugely important step. If you are able to allow for backlash also like in the Planet CNC controller, all the better. Both my X Carve and Shapeoko have about .0550mm on the X and Y axis of backlash. Which on a fine trace PCB can ruin a board.
The second one is ALWAYS to mill a sacrificial waste board for each project to make sure you stock is 100% flat and level in respect to the mill. Otherwise a .12mm DOC could jump to a .25mm DOC due to an uneven waste board or mill and this will snap your small end mills. A small piece of plain pine board works great and is cheap. They can be refaced for more than one job to reduce costs.
Third and equally important is to ALWAYS use a touch plate or probe your Z height/Zero. Being off even .1mm will change your DOC to something the DC spindle or the small end mill can not handle at a given feed rate and snap your end mill.
) but I have seen a lot of these threads here and at a few other sites and folks seem to hold onto those settings like they are car setups in Iracing. Figured I would get the question and answer session going… But that was a great bit of info. thanks.
