Not too new but it got serious - be keen for some input?

[boydage]

Not new to the DIY CNC game I was one who caught the bug and went DIY CNC throughout my hobby life. Typical story, built the first machine, used it to build the second, used the second to build the final 3rd CNC router. Then I converted a lathe. ha

My CNC Router is heavy, with a big heavy gantry. I use twin steppers on the Y pushing it with long lead screws. Using closed loop steppers it runs very well. The 2.2kw spindle is a little too small and fast, but sitting on the 45kg gantry works well off the stable platform it is sitting on. I have been using it mostly for timber, with a bit of alloy in between when needed. I use a 2 flute carbide cutter on just over half speed (approx 13000 RPM for alloy. Small cuts, and it sings through alloy nicely spitting bits of swarf out well.

I have been asked to produce some parts out of alloy, and want to setup proper to do the job well. The alloy stock is going to be quite thick. So I have a couple of questions, I think I know the answer but if someone is experienced here I would really like to hear thoughts:

1: On the above machine, I need to mill some pieces of alloy out 40mm thick. Using my 6mm 2 flute bit, it only has 25mm of flute depth (some endmills even less), the remainder being shank. Do I just continue to drop down into the work-piece with a cutter like this, or do I need to go out and buy a 2 flute bit with a 40+ mm cutting section? Know what I mean? Whats normal here?

2: I have a nice easy system of probing. Using the machine earth, and a moveable plate, I set my tool Z zero, and the X/Y by putting this plate between the workpiece and the end-mill using mach 3. Very effective, well for timber anyway. Anyone know of a probe with a spring ball on the end that would sit in a ER20 chuck? One that I can wire into my BOB? I will need this to setup alloy stock blocks on the table.

3: Anyone ever heard of a quick change chuck or tool-change assy that would go onto an ER20 spindle? That would be COOL!!! Imagine, your little spindle, click click, new different end mill without haveing to undo the collet.

Be good to hear thoughts
Boydage

Similar Threads:

• Problem- MDI input T32
• Keen - New Zealand Earthquake
• Need input
• 3 phase input VFD for single phase input?

[zvizdic]

I do CNC machining for living 30y and tried all. I like to use 4 flute endmills on steel 2 flute on aluminum and yes sometime I vent past the flute but not on many parts just to save time (picking up new endmil) one of parts.
If I have to use short flute endmils on deep cuts sometime i would grande shank slightly so it is not rubbing on finished surface providing you have folding coolant or air blow to prevent a chips from claiming up the endmil.

[boydage]

Hi. I always have a lot of respect for people who have been in trades for a longtime. Thanks for that. Funny, it didn't even occur to me to do that. ha. Yep, 2 flutes on alloy seem to be just about right. Small depth cuts. I am keen to look more into pocketing where I hit depth in the centre first, and then move out sideways instead of lowering down into the pocket each level.

So in an ideal world, you would use a cutter with flutes at full depth? I am restricted to 1/4" bits on account my spindle is low torque at low speeds. Minimum being 12000. But it does the job. I wonder if there is a decent carbide 6mm bit with a cut length of 40-50mm?

One thing I am doing is learning Fusion 360 - Cambam just doesnt cut the mustard on the larger jobs. One thing I need to learn is finishing. Thats a new topic.

[v2tiller]

Hi.
Have a look at Drewtronics 3d probes. He sells them on ebay.
Can you flip the part, do 20mm each side. I have just started cutting thicker ally and just made a part which was 40mm thick. Using an endmill with 20mm length i cut it in two parts.

[ger21]

You should try single flute "O" flute bits for aluminum (aluminium?). You can run them at higher RPM, where your spindle has more power.

You'll likely run into vibration issues with longer tools, but it may be your only option.

[boydage]

I thought it might nice to add some success stories.

1) Fusion 360 has taught me that my machine is able to take aggressive lateral cuts out of alloy by means of pocketing. It was scary at first to watch but man, it took a while to sweep up all the litter.

2) It is well plausible to mill cast iron with a high speed spindle. Today I needed to pocket out a tool holder bed off my lathe. Its Chinese cast iron, possibly not the best. But I pocketed out a 30mm dia 6mm deep hole, using a 2mm 2 flute carbide bit. Nice and slow, small step, and it just ground it away. I would imagine doing the large jobs might be a challenge, but it you need too, it is an option.

3) I would like to see if my Mach 3 Lathe and Mach 3 Router can be taught to use Fusion 360s probing. I dont know if I am being reckless, but I have my whole machines chassis connected to the earth/negative - kind of like a MENs system on your home wiring (in NZ anyway). I have a separate wire to a pin that goes to a fixed plate, and also a move-able plate. If I touch the plate to any part of the chassis, or the spindle for that matter, my BOB senses a closed circuit on the input pin I have it connected up too. I use this for probing, I can put the plate between my workpiece and the bit in the collet, and it probes that way. Its fast, easy, and I am yet to damage a bit. Is this a big no-no of CNC machining? I would like to be able to pop a proper ball probe into my spindle and run the probing program that Fusion 360 has. Has anyone done this with Mach 3?

Regards Boydage

[dazp1976]

Hi. I always have a lot of respect for people who have been in trades for a longtime. Thanks for that. Funny, it didn't even occur to me to do that. ha. Yep, 2 flutes on alloy seem to be just about right. Small depth cuts. I am keen to look more into pocketing where I hit depth in the centre first, and then move out sideways instead of lowering down into the pocket each level.
.

That's what I've started playing with at the moment on my mill. done some pockets 30mmx11mm deep.
Using a 6mm cheap bit I use 'smooth profile' rather than 'helix' ramping at 2.5degrees downward so it cuts around 1.1mm doc every 360degrees straight down the middle.
Then I cut outward sideways at a woc of 0.4mm. I'm leaving stock of 0.2mm on the bottom if not cutting all the way through and 0.4mm on the side edge.
Then swap to a nicer bit with a final 0.2mm 2 pass finish.
I'm doing this with a 3 flute bit at 2500rpm and 710mm/min table speed. Then a 4 flute bit at 2500rpm at 450mm/min finishing. Seems to work really well and is pretty quick. In fact I reckon it could go a bit quicker with larger woc but would break the tool if I ramped deeper.

I've tried the initial part with a 40mm long 3 flute 8mm bit as well at the same speeds with a 0.6mm woc and it worked well too. Then did the finish with the 4 flute.

If I was going deeper pocket (say 30mm) I would do it in 3* 10mm deep stages and the same goes for the finishing. Will go a long way towards having no tool flex.

If I used a carbide for this it would most likely break a tooth at my speeds so I use HSS-AL first and then HSSC08 cobalt for the final. This is only because of my limitations of rpm available to me.