# Thread: Homemade desktop CNC - cutting 0.8mm mild steel out the question?

1. I'd like to be able to cut 0.8mm mild steel (think of those little PC blanking plates)

I googled it & found this duscussion..

http://www.cncinformation.com/CNCBlo...ainless-steel/

ok, so they were talking about stainless, but it's similar - mixed opinions, so I thought I'd invoite some mixed opinions closer to home - Do-able or not?

2. nothings impossible with the right cutter, power and rigidity... you'll need to use a small, e.g. 3mm, cutter to bring the revs required into a possible range...

rough calcs...
cutting speed Vc for steel = 30m/min, so for a 3mm cutter revs required at spindle, N = 1000 * Vc/(pi * d) = 1000 * 30/(3.14 * 3) = 3000rpm
Assume feed per tooth Vz = 0.1mm/rev so feed rate Vf = Vz * flutes * N = .1 * 2 * 3000 = 600mm/min
Removal rate Q = width of cut * depth of cut * Vf/1000 = 3 * .8 * 600/1000 cc/min = 1.44cc/min
Power P = KQ where K = 70W/cc/min for steel so power = 70 * 1.44 = 100W (at output = 200W input)
Torque T = P * 60/(2pi N) = 100 * 60/(6.28 * 3000) = 0.3Nm

So relatively little turning force required at 3000rpm on spindle and a typical router should be up to the job and feed rates are not so high... use plenty of cutting fluid and dont go too deep into the sacrificial and it should be possible... but you'll need a decent carbide endmill with no more than 2 flutes. Dont go too low on feed rate or you'll end up rubbing and burning out the cutter.... if you can go a little faster than 600mm/min and you have the spindle power at those revs then worth trying a tad faster.

3. ## The Following User Says Thank You to irving2008 For This Useful Post:

4. Thanks Irving - a great reply.

Fortunately, my router (a Proxxon BFW 40e), has a range 900rpm-6000rpm, so dropping the RPMs is not an issue.

That said, it's only 250W...which I guess isn't great wrt cutting steel - I guess it'll be a suck & see job ....need to order up a 2 flute cutter & give it a go.

Would it be better to go with an even thinner sized endmill? (say 2mm diameter )....my thinking here is the less steel it has to channel out around the part, the less stress there'll be on everything? But then again, I guess you've then got to start wondering about the physical strength of the endmill at such smaller diameters (ie snapsville)?

5. Well, I just had a go - I only had a 4 flute 2mm dia end mill to hand - I went with 4 cuts @ 0.2mm cut depth per perimeter run, squirting a bit of wd40 (it was all I had!) once in a while - the end result was very reasonable (though a degree of deburring will be in order. I couldn't bring myself to use the higher feed rates, so went with 150mm per minute.

That said, I could telll that my machine/spindle wasn't particularly happy (I understand it better than my wife now) - it's used to acrylic! But at the end of the day, there was no real drama (unlike with my wife). Material clamping is an issue though, ie that last bit where the part is fully cut out from the material - it's tin helmet time. Not pleasant.

Nice to know though - ie that for the odd thin steel widget, my humble DIY machine will grudgingly comply.

6. double-sided tape underneath - stick it down to the sacrificial... or the spray-on quicksetting glue... easy to seperate afterwards with some acetone or other solvent..

7. Originally Posted by irving2008
double-sided tape underneath - stick it down to the sacrificial... or the spray-on quicksetting glue... easy to seperate afterwards with some acetone or other solvent..
That was with double sided tape underneath! The 'break' is one helluva lot more viscious with steel than acrylic that's for sure!! I'll ponder some quick setting glue.

tks once again

8. Program tabs into the job and leave about 0.25 mm in about 3 or 4 places.
This will hold it but allow you to snap it out the sheet easily.

.

9. ## The Following User Says Thank You to John S For This Useful Post:

10. Originally Posted by HankMcSpank
a degree of deburring will be in order... that last bit where the part is fully cut out from the material - it's tin helmet time.
Is the part particularly small? No possibility of running a couple of bolts through it?

If I had to guess I'd say the last .2mm of your tool is now exceedingly blunt and flex in the system is giving you a stop-go cut as it builds up a cutting pressure.

If you haven't got/can't use a bigger cutter I'd suggest, wind the speed down to about 1500rpm, the feed down to 60 mm/min or less, cut clearance on your sacrificial plate so can cut in one pass to a cut depth that uses the middle of the flutes and invest in a bottle of Rocol RTD liquid (apply generously) :naughty:

11. ## The Following User Says Thank You to Robin Hewitt For This Useful Post:

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•