Anybody got tips for the routing of 0.8mm stainless steel?

[Rodney Gold]

The cutter must have a lot of back clearance (for chip removal) amd you should use high speed steel and not tungsten carbide , a single flute V cutter is best and it should be a little less than halved to stop chipping and add rigidity , the point should be a flat. the included angle of the cutter is best at 40+ degrees , Ie not a SHARP V.
You must run at highish speeds (a few pases depending on router power) and use a cutting fluid like Dihatsol or Shell Dromus (or tapamatic or the like – tho tapamatic is expensive and not water soluble – it also doesnt wick away heat as well as a water based cutting fluid)
The problem is running too slow with high RPM and in general with SS is that it tends to overheats and work hardens , trying to route the work hardened metal leads to more overheating and it becomes a viscious circle , eventually the cutter breaks and trying to recut is even worse cos of the work hardened area.
If you use a slot drill or the like , consult a feed and speed table or ask the supplier what they recommend for your router power
We run at high feed rates , with slow rotational speed and mist cool the stainless – I dont really like cutting it much tho.

[signdevil]

This is our router http://www.signdevil.com/pages/routing&engraving.htm so it is capable of pretty much anything. I have to go straight through the stainless into a sacrificial bed and I need a flat edge so a v cutter is not an option. Can I run a 1/8″ cutter (less mat’l removal) or does it have to be a 1/4″ cutter (more removal thus more energy/work)? You say high feed rates and low rotational speeds. Can you elaborate on these parameters for 0.8mm thick s/s?

Cheers

[Henry Barker]

Hi there,

Not sure how to advise you, as I haven’t cut stainless steel here in the shop with my router, we have a guy locally that can do that easily with waterjet cutting.

Having said that, I was at Sign UK to talk to AXYS and look at different cutter manufacturers ITC do a 3 flute solid carbide square end with corner radius, 30degree right hand helix, centre cutting. specifically for Stainless steel , which is abit different what Rodney said…

They recommend running the machine at 4000rpm feed at 2-3mm sec and plunge at half feed rate The cutter is a DC03.

http://www.itc-ltd.co.uk

There was a norwegian company there too who have a new swiss made engraver for SS but that’s not what your after. http://www.crown-norge.no

maybe thats some help.

[Rodney Gold]

I would most likely run it with a single flute half cutter , but thats cos I grind my own.It depends on radii as to what you cutter you run. For example if you are cutting a heart , the split between the “cheeks” at the top of the heart wont be very sharp with a 1/4″. Big tools are problematic at high speeds tho , Is that the 2.2kw perske on the gerber?
The problem with tungsten carbide is that its brittle and chips the cutting edge, a titanium coated HSS 3mm slot drill would most likely be my next choice. Otherwise go with what Henry says 😉 We try to stay away from very expensive specialized cutters , cos albeit they do the job better , the cost of a tool can make the job unprofitable or even if the tool is not THAT expensive , a breakage and replacement can eat up the profit.
Cutting metals is a 2 part process with any cutter , there is an initial shear and then a chip , guillotine cut metal illistrated this well. If you look at the edge there is a bright bit and then a “shattered” dull bit , the shear generates a LOT of heat so the best cutting strategy is to generate minimal shear and maximum chip. The leading edge of the tool slams into the metal and should chip almost instantly , there should be enough clearance after that to eject the chip and not have it caught and “recut” , the next cutting edge should came into play as the tool advances to the next metal surface which is a function of the speed and feed and is dependant on no of flutes , chip removal rate , dept of cut etc etc.
Very difficult to give a straight answer to what speed and feed. However not all stainless is equal. There is a very nice “free machinig” stainless that is a little more expensive than 312 or the like abut cuts clean quickly , much like engravers brass which cuts dry without burrs vs half hard (normal) brass which requires a lubricant , can burr and cuts slower.
Same with Aluminum , 50 and 60 grade cut way better than 1200H.

[elitesigns]

the dc03 as mentioned by henry is the bit for the job, if you talk to itc and ask for Sally she’ll beable to advise speeds etc. although henry seems fairly close to what we use, we run the spindle at 80hz, feed 4.72ipm plunge 2.36ipm. The s/steel must be firmly stuck to a sacrificial sheet, (we put application tape on the s/steel, then spray adhesive to mdf), and the cut must be all the way through, also plenty of coolant.
We cut stainless all the time with very few problems.

[signdevil]

Thanks for the advice guys 😉

Hey Henry, saw you at the ITC stand at Sign UK. I had one of those moments when you see somebody you think you know but do not know where from. So if you saw somebody staring and looking very confused, that was me 😀 😀

[Henry Barker]

It was Terry Colley http://www.vintagesign.com that put me in touch with ITC and Sally, so I was picking her brains while I was there, going to talk to her next week and order some stuff.

I met a few “new” faces…I stood next to Peter of Star Signs thinking I know you from somewhere….and then asked him after abit of time if he was who I thought he was!

[Bill Dewison]

No mistaking you though Henry. Minute we all saw you walking towards us, at least 3 ppl in the group I was stood with said “Hey look, its Henry!” 😀

Still can’t get over how cheap the transport is between UK and Sweden, you know its cheaper to visit you than it is to drive down to London! 😮 Got any free bunkbeds for a gang of misfits then? 😉 😆 😆

Cheers, Dewi