HSS Engraving Cutters

Engraving Stainless Steel with fine point carbide engraving cutters is a hit and miss affair - as far as this newbie is concerned. You fit a new cutter and hope that the tip won't chip before the engraving is finished even if you are only engraving to a depth of 0.1mm. My learning curve has included going from 30 degree angle 2 face cutters to 45 degree 3 face pyramid cutters, reducing both feed rate and penetration rates from 400 and 100 mm/min down to 250 and 40mm/min respectively. But I still get breakages. I should try the softer Stainless Steels but much of the stainless steel that you buy on ebay in the quantities I use, the seller doesn't know what type of stainless steel they are selling. Micro-grain carbide cutters are said to be more chip-resistant - but I still chip them.
HSS engraving cutters are recommended for stainless steel - but can I find any anywhere - even MSC's huge catalogue doesn't have any. After that preanble - here are the questions:
1) Does anybody know where I can get HSS engraving cutters - or failing that:-
2) Is it possible using stock HSS rod (say 3 or 4mm diameter) to grind my own pyramid 3 face cutters - anybody have a website or video site showing best way to do this

stainless is always hard to cut. it's soft and gummy(best i can explain) and tends to just
"tear" rather than cut. do you use coolant ? i always use that and my cut and engravings come out ok.
hope this helps

Hi Piasdom,

In my initial naivety - coolant - no. But then I read online somewhere using mist coolant, etc. - 3-in-1 oil was also mentioned. I do have normal coolant for my lathe/milling work - but I thought I would try the 3-in-1 method first. So I made a bund from Newplast modelling clay around the keyrings I was engraving and filled the enclosed keyring tag with 3-in-1 oil. Seemed to work OK - but I still managed to break the carbide tip on my 3rd keyring tag. I will try the same method with coolant once my next batch of micrograin carbide pyramidal cutters arrive. I'm also thinking of using small diameter (0.2mm) mill end cutters instead - although I think the ones I have are "down" cutters and I think I ought to be using "up" cutters to limit the load on these very narrow cutters.

sounds like you're getting close. you may need to still work on the speed and feed.
stainless needs to be cut slow anyway. Good Luck !
show work !

Hi Piasdom,

I have been getting conflicting messages about speed. My CNC machine has a top speed of 14000 rpm and I have been engraving at 12000 rpm because I read somewhere that you needed 24-30000 rpm - even this beginner thought that was far too high. Anyway I've attached one of the keyring tags I have made - showing result before the tool tip chipped - after which the engraving lines were much wider.

i have a Roland engraver(max 30,000) i usually engrave at 20,000 with a 68mm feed..
i also have a CNC Msater mill( 5400 max) and i engrave at 4200 with 4InchPerMin.
looks like you're feed is too fast for the rpm. leave the rpm at 12,000 and just adjust the feed.

Download the free trial of G-wizard . It is for win only, if you use win. If not give me your tool geometry and I can run it for you to get a recommended feed and speed.

Hi Nitromethane,

I don't do enough or understand enough yet to justify the outlay of the annual prices for G-Wizard - so if you could run the following I would be grateful.

So far I've used 3 different cutters. The first I tried - and I realise that the included angle of 30 degrees is probably too steep - was a normal V-shape carbide single fluke cutter.
Flat bottom 0.3mm cutting edge diameter
Shank diameter 3.175mm

2nd: same V-shape: tungsten cemented carbide single fluke cutter
Included angle 60 degrees
Knifepoint 0.1mm

3rd: 3 edge pyramidal cutter: micro-grain carbide
4mm shaft
45 deg cutting angle
Cutting width 0.1mm

These descriptions are from the sellers on Ebay where I got them from.

Thanks - Micromet

Also if you are using a pool of lube on the keyring then it is not evacuating chips away from the cutter. In stainless steel you must get the chips away from the cutter. They are work hardened and are much harder than the original material. Use some compressed air and a light mist of coolant to keep blowing the chips away and to keep the cutter tip cool.

carbide single fluke cutter.
Flat bottom 0.3mm cutting edge diameter
Shank diameter 3.175mm

At an RPM of 12000 this should have a max feedrate of 2.6 ipm. This may cause too much tool deflection causing chatter and tool failure. This has a chip load of 0.0005" per tooth any lower feedrate may cause rubbing and premature tool failure.

2nd: same V-shape: tungsten cemented carbide single fluke cutter
Included angle 60 degrees
Knifepoint 0.1mm

At an RPM of 12000 this should have a max feedrate of 4.7 ipm. Chip load of 0.0009" per tooth.

3rd: 3 edge pyramidal cutter: micro-grain carbide
4mm shaft
45 deg cutting angle
Cutting width 0.1mm

At an RPM of 12000 this should have a max feedrate of 16.5 ipm. Chip load of 0.0013" per tooth. May want to back the feed off a little to start with and work your way up. More teeth get a higher feedrate. Gullets may be too small for that much chip load.

These are what G-wizard kicked out and I cannot vouch for them otherwise.