-
I want to thank all the members that have upgraded your accounts. I truly appreciate your support of the site monetarily. Supporting the site keeps this site up and running as a lot of work daily goes on behind the scenes. Click to Support Signs101 ...
CNC .080 mister?
- Thread starter skyhigh
- Start date
rjssigns
Active Member
I am by no means an expert, but the first thing I would ask is how big is the job? If it is small and are using it as a test then give it a shot. Otherwise there are other factors to consider like the rigidity of the gantry etc. There is tooling for regular CNC equipment that is designed to run without coolant. In fact if you do not get it into operating temp (some are 1700F!) they will start to seize in the material.
If it is a large job that has to look good, set up the file for your local water-jet shop. Stuff comes off the 'jet with nicely finished edges. No clean-up. Just my 2 cents.
If it is a large job that has to look good, set up the file for your local water-jet shop. Stuff comes off the 'jet with nicely finished edges. No clean-up. Just my 2 cents.
CES020
New Member
I've personally talked to people that say they do this all day long every day, without coolant. I've gotten the same bits, the same speeds and feeds from them, tried it, and had no luck on some jobs and good luck on others.
What we have found is that the RPM's are critical. If we get above 8000 RPM, then problems start to happen.
WD-40 works decent, if you wanted to just get through this job, a couple cans of that and keep the RPM's below 8000 and you could probably make it through it. The important part is that if you do see a big burr starting to roll up (the chips have welded themselves to the cutter), stop the machine right that second and recover from it. The burr it will roll is a nasty one and a pain the butt to remove.
What we have found is that the RPM's are critical. If we get above 8000 RPM, then problems start to happen.
WD-40 works decent, if you wanted to just get through this job, a couple cans of that and keep the RPM's below 8000 and you could probably make it through it. The important part is that if you do see a big burr starting to roll up (the chips have welded themselves to the cutter), stop the machine right that second and recover from it. The burr it will roll is a nasty one and a pain the butt to remove.
skyhigh
New Member
What bits do you recommend CES020 & RJ?
Star sign..... are we talking plain water in the sprayer? Would clamping the air hose from the compressor, and having that blow on the bit be a better option? Perhaps a combination?
How big of a bite into the aluminum should I take? What bit? And is everyone in agreement to keep under 8k rpm?
Local water jet guy wanted $550 the last time I did just 2 of the "Land Management" panels (politely....he's hard to deal with). My local "laser" guy wants $325 to do these panels. Ok, $300 bucks isn't too bad...but better in my pocket.....especially when I maybe/should be able to do them myself. Of course, it dosen't take too many bits to hit the $300 mark. Perhaps its an investment in the "learning process"????
Star sign..... are we talking plain water in the sprayer? Would clamping the air hose from the compressor, and having that blow on the bit be a better option? Perhaps a combination?
How big of a bite into the aluminum should I take? What bit? And is everyone in agreement to keep under 8k rpm?
Local water jet guy wanted $550 the last time I did just 2 of the "Land Management" panels (politely....he's hard to deal with). My local "laser" guy wants $325 to do these panels. Ok, $300 bucks isn't too bad...but better in my pocket.....especially when I maybe/should be able to do them myself. Of course, it dosen't take too many bits to hit the $300 mark. Perhaps its an investment in the "learning process"????
J Hill Designs
New Member
i probably wouldnt even mist .080 personally...I only start misting/multi-passing at 1/8" alum or thicker
skyhigh
New Member
Again, I'm surprised. You usually do .080 in one pass? What rpm and feed rate? What bit would you recommend?
I'm feeling really
J Hill Designs
New Member
if the material thickness is less than half the bit diameter, than yes one pass...
approx 13krpm, approx 25IPM
approx 13krpm, approx 25IPM
Westcoast Sign Guy
New Member
What you need the Vortex Cool Tool.
Just Another Sign Guy
New Member
the biggest 'tip' i could offer in regards to routing aluminum is to pre drill all of the entry points, i jog through and plunge each entry point and then clear the 'bur' off of the bit before jogging to the next entry point.
i have improvised and seen some amazingly creative improvisations in regards to 'misting systems' the professional models usually are a mix of air and misting fluid (depending on what is being machined) but i have also seen many people get by with the garden sprayer and wd40 and even non aerosol wd40 placed in a garden sprayer. have also seen people use automotive anti freeze.
there are router bits specifically for aluminum, brass, copper, etc., = solid carbide spiral o flute .
other than that follow the basic rules of running your machine, ie don't cut deeper than 1/2 the width of your tool, etc.
i have improvised and seen some amazingly creative improvisations in regards to 'misting systems' the professional models usually are a mix of air and misting fluid (depending on what is being machined) but i have also seen many people get by with the garden sprayer and wd40 and even non aerosol wd40 placed in a garden sprayer. have also seen people use automotive anti freeze.
there are router bits specifically for aluminum, brass, copper, etc., = solid carbide spiral o flute .
other than that follow the basic rules of running your machine, ie don't cut deeper than 1/2 the width of your tool, etc.
Westcoast Sign Guy
New Member
Not sure what you mean by plunging into the aluminum, I'd lead into it in a radius.
Just Another Sign Guy
New Member
no I don't ramp in , I jog to each entry point & drill to zero at every entry point. In my experience the only times I have build up accumulate on the bit (assuming you are running at proper speeds) is from the entry. You could ramp in but I ve found it is less problematic to simply jog through & predrill your entry points. If your material requires that you route in multiple passes this wouldn't be of benefit but if you can machine it in one pass I've found it to be less problematic. Ymmv
I think you are going to get a few different answers here. But my experience is as follows...
For .090 alum (whatever alloy Harbor sales sells) with a spiral single 0 flute, upcut is:
1/4" bit = 12,000 RPM's @ 1 IPS and the Z @ .40 IPS
1/8" bit = 16,000 RPM's @ .40 IPS and the Z @ .40 IPS
Ramp-in the toolpath.
I get the best edges cutting up to .040 and .063 as a single pass strategy.
Two passes for .080. .090.
I have vac hold down. And still use clamps, screws, whatever it takes to make sure that the sheet doesnt move even the slightest little bit.
I get the most awesome cut with... Onsrud 1/4" SE UPCUT SPIRAL SUPER 0 FLUTE PN: 65-025
Onsrud 63-622's are cheaper and they work too but don't last me quite as long in aluminum. Belin makes a similar.
Watch the chips that are thrown off the whole time you cut. They should look like "little smiles".. not tiny specs and not full piggly tails. When I see smiles, it makes me smile.
I tried cutting fluid, wd40, water, over the years cause i thought I was "supposed" to from reading on the internet. Honestly it never made a difference for me other than to make a big mess of metal shavings in an oily slurry.
But, this is all what works for me.
For .090 alum (whatever alloy Harbor sales sells) with a spiral single 0 flute, upcut is:
1/4" bit = 12,000 RPM's @ 1 IPS and the Z @ .40 IPS
1/8" bit = 16,000 RPM's @ .40 IPS and the Z @ .40 IPS
Ramp-in the toolpath.
I get the best edges cutting up to .040 and .063 as a single pass strategy.
Two passes for .080. .090.
I have vac hold down. And still use clamps, screws, whatever it takes to make sure that the sheet doesnt move even the slightest little bit.
I get the most awesome cut with... Onsrud 1/4" SE UPCUT SPIRAL SUPER 0 FLUTE PN: 65-025
Onsrud 63-622's are cheaper and they work too but don't last me quite as long in aluminum. Belin makes a similar.
Watch the chips that are thrown off the whole time you cut. They should look like "little smiles".. not tiny specs and not full piggly tails. When I see smiles, it makes me smile.
I tried cutting fluid, wd40, water, over the years cause i thought I was "supposed" to from reading on the internet. Honestly it never made a difference for me other than to make a big mess of metal shavings in an oily slurry.
But, this is all what works for me.
asd
New Member
this is how I cut aluminum on my homemade set up
I use a piece of blue styrofoam between the table and aluminum. why styrofoam and not a scrap of sintra because sinrta is hard and when your are cutting at such low speeds it tends ot melt and stick to the bit
attached the blue foam to table and use double sided banner tape to hold down the aluminum (make sure you have tape under the piece that will be cut out so it does not get thrown at you.
Bit = 1/4"upcut spiral - gives you a cleaner cut
coolant = alcohol cools the metal better than water and is easier to clean up your pieces
speeds = 15 ipm x,y and 5 ipm for z
router speed = around 18000 rpm
i do 2 passes so I don't brake the bit
I use a piece of blue styrofoam between the table and aluminum. why styrofoam and not a scrap of sintra because sinrta is hard and when your are cutting at such low speeds it tends ot melt and stick to the bit
attached the blue foam to table and use double sided banner tape to hold down the aluminum (make sure you have tape under the piece that will be cut out so it does not get thrown at you.
Bit = 1/4"upcut spiral - gives you a cleaner cut
coolant = alcohol cools the metal better than water and is easier to clean up your pieces
speeds = 15 ipm x,y and 5 ipm for z
router speed = around 18000 rpm
i do 2 passes so I don't brake the bit