Need Help!- Engraving Stainless speeds/feeds?

[GMTool]

We have been having a good deal of trouble engraving 304 stainless steel. We have tried various split style engraving cutters and most break down after 2-5 pieces. (according to my estimate via BobCAD) ~35" of cutting each piece.

What we are doing is engraving just a single line for letters and a square figure table, on a piece of stainless, this later gets filled with a black paint, and baked. Depth of cut is only ~.008" Deep. And we are cutting on a Hardinge/Bridgeport VMC (GX 650B) Max RPM 8000. It is however plenty rigid enough, and should be able to give a good line.

We recently purchased some Antares carbide spiral flute engraving cutters for stainless steel, but really don't know what speed/feed we should be looking at? Would it be better to run 8000RPM with .0001"/tooth, or something more like 3000RPM and .001"/tooth to give a better chipload to the carbide? Also should we do it in one .008"Deep pass, or break it up to a .005" & .003" passes? Oh and what about the plunge down into the material feed?

While Speed isn't essential, the quicker this all goes, and the longer the tool lasts, the better. Any suggestions would be greatly appreciated.

[peaceandcalm]

hi there, i know its a bit late to reply, i am having the same problem, i wonder did ya find selution?
i would lke to know you found any selutuions..
cheers

[Jason3]

Peaceandcalm, have you tried a ball end cutter? Perhaps try a 1mm two flute carbide ball end mill, 7500 rpm, 500 mm/min and feed in Z about 200 mm/min, up to about 0.5 mm deep you should be ok in one pass.

Best regards,

Jason

[peaceandcalm]

hi there jason, no i havnt tried, but if i go 0.5mm deep the engraving would be very wide and customer dont want that, i have to use 0.5 tip which is what engraving cutters are for, for big letters i have no problem they last ok and i can use ball nose carbide, but 1mm is just to huge radius...
cheers

[BobWarfield]

Originally Posted by GMTool We have been having a good deal of trouble engraving 304 stainless steel. We have tried various split style engraving cutters and most break down after 2-5 pieces. (according to my estimate via BobCAD) ~35" of cutting each piece. What we are doing is engraving just a single line for letters and a square figure table, on a piece of stainless, this later gets filled with a black paint, and baked. Depth of cut is only ~.008" Deep. And we are cutting on a Hardinge/Bridgeport VMC (GX 650B) Max RPM 8000. It is however plenty rigid enough, and should be able to give a good line. We recently purchased some Antares carbide spiral flute engraving cutters for stainless steel, but really don't know what speed/feed we should be looking at? Would it be better to run 8000RPM with .0001"/tooth, or something more like 3000RPM and .001"/tooth to give a better chipload to the carbide? Also should we do it in one .008"Deep pass, or break it up to a .005" & .003" passes? Oh and what about the plunge down into the material feed? While Speed isn't essential, the quicker this all goes, and the longer the tool lasts, the better. Any suggestions would be greatly appreciated.

Sounds to me like you are probably work hardening, and then the cutter wears very poorly as it deals with the work hardened material.

Keep the chipload up and use fewer passes to try to minimize the work hardening. I'd really avoid that 8K rpm with a tenth chipload, and I'd also try to do one pass. Since you're baking paint into the engraving, it will cover some sins if the surface finish isn't wonderful.

Best,

BW

[peaceandcalm]

are you all speaking from experiance? becasue i been tryig for half a year all sorts of feeds and speeds, and nothing last as some people claim they last...
my feeds were 6000rpm 70mm/m plunge and 150 feed..
i have heared i need to go 64000 rpm that would fix the problem they said..i dont think so but my mahcine goes up to 15000 max...

[travla]

Hi peacesandcalm,

I use a router spindle that bolts onto my engraver & I run it at around 60000rpm, I use a quarter round bit, with a feed rate of 3-4mm a second & multiple shallow passes. I also have a misting unit to lubricate the bit as it cuts, this is esental to extend tool life. I would also recommend sourcing a machine grade stainless, as this is slightly softer than 304 & much easier to work with.

Help this helps

Travis Ashford
Braille Sign Supplies
http://www.braillesignsupplies.com.au

[peaceandcalm]

the question is how long will it last like engraving down to 0.3mm and what is your plung feed? and do you use vacum table or spring loaded tool?
my work here i cant get sheets 303 i wish i can, but here in NZ they provide 304 2mm sheets which is very unpredictble material..anyhow let me know how long will it last lets say engraving 200 leters on a panel about 8mm width of a letter?
i can give example if needed as dxf file..
cheers

[travla]

I did a job recently in 304, I had to hog out the word toilet multible times & an assortment of Male, Female & Accessible Symbols, I was getting about 5 hours of cutting from each bit. I used a plunge rate of 10mm a second, feed of 4mm a second & 2 passes of 0.3mm. I also had the material clamped down to my t-slot table.

Travis Ashford
Braille Sign Supplies
www.braillesignsupplies.com.au

[peaceandcalm]

which brand and company cutters do you use? isnt 10mm plunging should be 1/4 speed of feed? did ya use like spring tool? and how many sheets did ya do per cutter? and what was spindle speed?

[Cutting Edge 1]

Greetings,

We do a bunch of stainless steel engraving. All of it is done on our old Horton pantograph engraving machines. We don't currently run CNC however will be in the nee future.

Anywho when engraving stainless we get the best results taking no more then .010 a pass.

Lubricate the area first and after the first line fill engraving with as much lubrication as possible. Continue. You don't want the cutter to get too hot.

As far as feed rate for us it's by feel however I would say we feed really slow with generally higher speed for the spindle.

Single flute 30 degree carbide cutters with a .020 relief.
The tip of the cutter should always be as wide as possible. The finer the tip the easier the tip is to chip or break.

Spring loaded cutters generally are for contoured parts, glass, or diamond drag. Not necessary with deep engraving in stainless.

[Cutting Edge 1]

Greetings,

We do a bunch of stainless steel engraving. All of it is done on our old Horton pantograph engraving machines. We don't currently run CNC however will be in the nee future.

Anywho when engraving stainless we get the best results taking no more then .010 a pass.

Lubricate the area first and after the first line fill engraving with as much lubrication as possible. Continue. You don't want the cutter to get too hot.

As far as feed rate for us it's by feel however I would say we feed really slow with generally higher speed for the spindle.

Single flute 30 degree carbide cutters with a .020 relief.
The tip of the cutter should always be as wide as possible. The finer the tip the easier the tip is to chip or break.

Spring loaded cutters generally are for contoured parts, glass, or diamond drag. Not necessary with deep engraving in stainless.