Questions on using a moving gantry style mini-mill...

[JAZZCNC]

Where i am roughing with the 5mm tool, i have 2.5mm rads in all the internal corners, the finish tool of 2mm will plough into these at full speed - recipe for breakage here ??

Well first you'll finish at lower feed than roughing and because of the Rad the stress on the 2mm tool is progrssive with the highest stress being fraction of the cut.
Give it big blast of lube/air when entering corner and it will fine.

[Davek0974]

Oh well, not there yet

I spent a while assembling a fogless coolant thingy, plans as found all over the 'net, pretty easy build, seemed ok.

This was my setup - pre-drilled the cut-to-size plates so i had a fixed position, jig style setup.


First run was at FS calc speeds, new 5mm high helix carbide tool, that ended up in a right mess very rapidly, boy did it complain! The fact that it managed to carry on ripping through the metal with a fully loaded tool was quite impressive - tough little some-bitch this machine!

The tool did not break!

After the "what the f*** was that?" moment passed I hit the e-stop! On examining the aftermath, it appears the new coolant system stopped the coolant and was just on air only, this allowed the tool to load up and that was the end.

After an hour of messing i got most of the gunk off the cutter - that stuff was welded up!



Upon removing the plate from machine I could see the carnage below, the load-up had pulled the tool from the collet and happily chewed my nice new bed



I cleaned that up with a flat file and tried again. Same cutter but this time I altered the parameters from one ramped full depth roughing pass to stepped multiple passes of 0.81mm at 1500mm/min.

I also cranked up the coolant but it sucks big time and is the typical fogger system that i did not want - the whole room filled with oil/paraffin mist, I can still taste it! Totally unsuitable but i pressed on as i did not want to be beaten on this.

I got a video of it roughing out - https://youtu.be/A9ZqR9chMwg

Things seemed a bit happier, fingers were crossed.

Then came final pass on the 2mm tool - again nice new solid carbide, the small holes were run at 1000mm/min at 0.62 DOC, ramped - these worked perfectly and i was impressed here.

The pre-finish on the three loops at the bottom again worked perfectly.

The final pass on the outside edges was at full-depth and 0.1mm cut, 1000mm/min - this is where it all fell apart again - the corners of the cutouts where the larger rads were left made a bit of a squeal but first cuts worked ok, the left side of the main part cut ok on one side of one notch but the second broke the tool and that was it for the day.



I had ordered spare cutters but some were crap and had to go back, that left me with just one 5mm and one 2mm from another supplier - the 2mm is trash and the 5mm is still gummy after about 1mm depth.

The final part is above - onion skinning will not work as there is a slight variation in bed heights and the part cannot be removed fully. I think tabbing and a sacrificial sheet of hard card or something under the plate will work better.

I also have an odd issue where mach3 went into reset when on the line before a tool-change - it would stop the spindle, lift up to clearance height then sit there in reset, pressing reset again allowed the spindle to come to park position for tool-change and then carried on normally. This happened a few times. My only suggestion here is interference from the M05 spindle-stop triggering the reset and this stopping the code right before the M06 command. I have a filter for the VFD and will bung that in.

So, unless I can find some tooling in the Bridgeport cabinet, I'm stuffed for the weekend.

I also need a coolant system as paraffin mist must be bad for health, it certainly tastes like crap!

[routercnc]

It's easy done when you start cnc machining (and from time to time when you've been doing it a while)
You need to get used to the machine and dial it in accordingly. You'll get there

I've been machining a number of parts recently and have supported the work piece using parallels (on their side) to lift it slightly off the bed. Then pushed a piece of thin MDF under the work to reduce the vibration. The parallels keep the work flat relative to the bed and you can cut at least 1.0mm through to make sure it is free without hitting the bed. I used tabs to hold it.

Just before each pass (when it is ramping down) I vacuum around the profile to clear the previous chips and give a bit of WD40 spray and repeat until done. I don't have a compressor so this is my way currently

Good luck with the fog buster development as I think that is a good long term approach

[Davek0974]

I'm not getting any more tooling from eBay, just ordered some 2mm and 5mm single-flute carbide tools, more swarf clearance and a stiffer tool, from Cutwell - part E5E47020 was one of them. Recommended for Aluminium and plastics.

The previous eBay ones I ordered three 2mm high helix 6mm flute, I got one that was 5mm long and two others of a random length and unknown but obviously wrong helix angle, they refunded them but it left me short on cutters.

Hopefully I can find some tooling in the cupboard to get me going again of the weekend.

As for the coolant, i'm going to drill out the jet from 0.6 to 1mm and try that - it should lower the air velocity and increase droplet size hopefully.

There is one other remote possibility - Aluminium warehouse have goofed up again and sent a soft grade of alu when I wanted 6082 T651, they have done this once before and i spent a weekend trying to figure out what was wrong with the plasma cutter when all it needed was the correct aluminium. :(

I will switch to tabbing as well, can't be any worse ;)

[Davek0974]

Been digging through the cutter drawer, found loads of 3mm carbide 3 flutes, some 4.5mm and 5mm 3 flute cobalts as well plus a 2.5mm cobalt.

I isolated some of the features on my part and run them in the scrap from yesterday - i hate wasting metal ;)

I also tweaked the F & S sliders in HSMAdvisor to suit my machine rpm and also a lower feed-rate (i had not done this yesterday so it was running full production rates or at least trying).

Using the 5mm 3-flute and a 3mm 3-flute, plus the modified coolant (much better with nozzle cut off) I set some different paths and all seemed ok, 1mm DOC was quite happy on the 5mm with 30% step-over
on the pockets, the 3mm was ramped down to a full 5mm cut at 0.1mm deep and that seemed ok too, the end result...



4 perfectly cut features. I even got a bit of video.. https://youtu.be/uIuylK4Y7qs

Annoying bit is that I can't try cutting a real job as the job is designed for 2mm finish tooling and it fails in CAM if i try using the 2.5mm cutter so I will have to wait until new cutters arrive now.

I think the single flutes will do well - lots of chip clearance and slower feeds. I have also re-cammed the job for full cut + 0.05mm and added some tabs, it will be cut on a 0.3mm spacer sheet.

[Davek0974]

Educational....

As i have ordered some cutters from a reputable supplier now, I asked them what the recommended cut specs were for rpm, chip load and feed. They instantly sent me a nice chart with it all on, feeding the data into HSMAdvisor shows up where i was probably going wrong a bit :)

Things alter rapidly when you give the calculator the correct data - i was running too fast, too deep, too much chip. Adjusted specs for a 2mm single-flute carbide would be...
18,000rpm
2.5mm DOC
600mm/min feed

I recall when i snapped the 2mm on the weekend I had it set at something like 1400mm feed and 5mm DOC :)

Helps having correct data i guess.

[Davek0974]

Wow! This sh1t gets expensive fast ;)

This sorry saga relates to the part shown in the OP.

Waited a week for the cutters to arrive, first 5mm carbide bit the dust in 30 seconds! The speed calculated at 12000rpm and using my lookup table i set 14500rpm as my speeds are off. The cut started and as soon as the cutter ramped in about 0.5mm of the 2.5mm set the motor bogged down like it was totally powerless and ping went £10 :(

So, back indoors, reprogrammed for about 20,000+ rpm and started again on my reserve tool, all started ok, 1st pass was flinging sizeable chips across the room, ramps down for second pass and even though i set 0.4mm holding tabs in various places, the first part broke free and fell out thus ruining that bit. Thinking the cut was too heavy i backed off the feed a bit in Mach3 and let it go, 75% of the last roughing pass and the part breaks free and takes the cutter to the bin with it. It's irrelevant but thats £25 of bits in 15 minutes, plus another sheet of 5mm Alu in the bin. :( :( Talk about pissed off!

Right, observations...

1 - Is this job actually possible?
2 - is there any point at all at running less than 100% RPM - these spindles seem to have zero power.
3 - It seems to be cutting 0.2mm below the set height - I need to tweak the Z height routine a bit, set the plate thickness a bit off to lift the tool 0.2mm
4 - How thick should holding tabs be - I set 0.4mm but clearly not enough.
5 - I set 2.5mm DOC for the roughing on a 5mm bit, go less, 1mm??

Exceedingly vexed at the moment :(

[Ger21]

3 - It seems to be cutting 0.2mm below the set height - I need to tweak the Z height routine a bit, set the plate thickness a bit off to lift the tool 0.2mm

No, you need to find out why it's off by .2mm.
It should be right on, every time.

[Davek0974]

I will get the indicator out and re-check the steps-per setting, can't think of anything else I can do?

[routercnc]

I use 6mm 2f carbide 45deg alum carbide bits at 12000 rpm 900 mm/ min 1.0mm DOC. Any more DOC and the motor sounds loaded and risk of gumming up is pretty high.

I also drop the feedrate manually when deep into a profile cut as the chips are harder to clear.

I often manually drop the feedrate on the first cut as the surface seems to be harder than the core. Also my ramps in and pretty slow.
I've seen others post more aggressive rates but it does not work for my machine.

My tabs are about 3mm as you are not just holding the part but stopping it vibrate on the finish pass to get the best surface finish. Means you need to cut them out with a pad saw not just push them out .