[racecraft]

I'm trying to engrave our company logo into a piece of 3/16" grade 50 sheet steel.

Here is what i have:

Haas Tm-2 Mill
4,000 max rpm

I have a .0625" 2-flute ball nose cutter that is ALTIN coated and i am trying to pencil engrave into the plate .015" depth of cut.

I am flooding it with coolant.

My linear feedrate is 1.00 IPM and plunge is .75 IPM, I am maxed with the spindle at 4,000 rpm.

My tool is lasting about 5 minutes worth of cut time and my finish is HORRIBLE!

Where am I goin wrong? Please Help.

[sambo67]

are you using carbide or hss

[racecraft]

i am using carbide.

[sambo67]

try using a multi flute endmill . on steel the more flutes the better.Also because you are using the tip of the radius you do not have any chip clearance, therefore your endmill will try and load up.Remember. this type of cut you are climb and conventional milling.try using smaller depths at least a finish cut of about .005 you also need to ramp in ball nose endmills do not like to plunge and plunging will dull the end flutes.you also may want to speed feedrate up to about 4.0 IPM

[racecraft]

I will give this a try.

I did also try a solid carbide 60 Deg "V" engraving tool. This didn't seem to help at all. They wore out just as fast and were about 5 X's the cost of the ball nose.

I have another part running right now but as soon as that is done i will try your suggestions and post how they worked out.

Thanks so much for the help.

[racecraft]

Nah.... still not running very smooth. sambo67, your advice helped, but i still only made it through 1 1/2 parts per tool.

Not a big deal.

We'll just take the hit and switch to some 1018 CRS bar stock. That should do the trick.

Thanks for the help!

[diecutter]

I will give this a try.

I did also try a solid carbide 60 Deg "V" engraving tool. This didn't seem to help at all. They wore out just as fast and were about 5 X's the cost of the graving cutters. Often a single tip lasts for hours. I cut manually at approx. 3 ipmball nose.

I have another part running right now but as soon as that is done i will try your suggestions and post how they worked out.

Thanks so much for the help.

racecraft, I engrave in die steel every day with 60 degree carbide (split point) en and at about 8000 rpm and use a flood of heavy sulphated cutting oil only at the engraving area. Your depth of .015 is right on for good results.

My results are very crisp with the v- bit and rely on the relief angle being correct (25 degrees), and the proper amount and angle when tipping the cutter. My cutters are not that expensive at under $10 each for double ended .125 shank diameter, considering they can be resharpened in a couple minutes in my Deckel SO tool grinder as many as 20 times each end before needing replacement. Hope this info helps.

[diecutter]

racecraft, If you don't have any success switching steels, send a scrap of that grade 50 steel and your logo file and I'll be able to find out real quick whether a split point is the right tool to use. I'm not familiar with grade 50, but have engraved most high alloy die steels without a problem.

[racecraft]

That could maybe be a plan. Where are you located and how much would it run me to have you try something like that?

Remember: We are limited at 4,00 RPM and i would like to go .015" deep in one pass to keep cycle times to a minimum (which is still a long one)

[DareBee]

The problem with the 50W is the hard scale on the surface.
I have engraved in many steels (tool steel as well - occasionally).
I use a $2 centerdrill with good results.
I personally wouldn't expect any better tool life out of that hot rolled.
I usually engrave 8 - 10 thou deep, 8500RPM 15IPMish.

[racecraft]

DareBee,

This is grade 50 but the material is "pickled & oiled" meaning it has been de-scaled. It is still hot-rolled material. Therefore, i think a lot of the problem is the tool is running into "hard" spots in the material. The material is not consistent at all.

On the other hand, are u talking just a HSS #2,3,4 etc. center drill?

Thanks.

[diecutter]

racecraft, If you don't have any success switching steels, send a scrap of that grade 50 steel and your logo file and I'll be able to find out real quick whether a split point is the right tool to use. I'm not familiar with grade 50, but have engraved most high alloy die steels without a problem.

racecraft, I looked up grade 50 steel and it appears it was originally designed for stressed structural members on ocean oil rigs. Most likely it will be engravable with a split point. If I could see the logo size and general shape I may have some tips on cutting it even if nothing is:cheers: sent to me for testing. My offer was simply one company helping another through CNCzone with no cost involved. If you want me to try engraving a sample PM me and I'll give you info to ship it.

[DareBee]

Usually a #2 HSS.
Tried it one day when I didn't have an engraving cutter in stock and haven't bothered going back. If I did a lot of engraving, I would likely get an engraving bit, but for the little I do it is very effective (not to mention cheap).
P&O still has a hard skin. The material will be consistent (not like "Black Max").

[racecraft]

Diecutter,

Attached is a pic of what im cutting. This one was with a brand new cutter and the adjust processes sambo67 suggested. This ONE looks real nice.

I actually reverted back to sambo67's advice and because i can not ramp in very decent because i have no straight lines, i chose to do a "peck" plunge. I am still going .015" deep and did increase the feedrate to 3.2 IPM. Flood the hell out of it with coolant and let it run. After about 2 parts the finish is still deteriorating but ive made it through 5 parts now and no broken tools..... yet!

Maybe i could just buy myself one of the split-point cutters youre talking about and try it myself? Not sure what brand of cutter or part number though?

Thank you very much for your help! :cheers:

[DareBee]

Very nice.
Those cutters tend to be called "Mill/Drills".
The tip grind is very much like a center drill, but they can be used effectively to a much greater depth while side cutting.
There is also diamond engraving bits that are multiflute but they are meant to be run at router type speeds.

[diecutter]

Looks great in the photo. 4,000 rpm is way too slow for a 0.0625 tipped split point carbide cutter. 8 to 12k is more like it and would allow you to increase your feedrate. For cutters I use www.gesswein.com. Antares and MSC also carry good quality split points.

Did some checking and Gesswein is out because they only sell blanks which you have to sharpen yourself. MSC only has .005 tipping on their cutters so you would have to tip them to 0.0625. That leaves www.antaresinc.net 800-355-5250. I have dealt with them and they have excellent tech support and can custom sharpen the split points they sell you for your exact application. You should get a wealth of info when calling them as I did.

[sambo67]

racecraft, what horsepower is your machine?