A572 Grade 50 Steel...!!!

[cterry352]

Machining some A572 Steel, which is around .21-.23 carbon.. Hight strength, low alloy steel... .750in Thick... Just drilling some holes, but in production.. having to drill three 13mm holes (.5118) As of now im using a Accupro 135 Deg split point TiN coated drill.. Running 858rpm at 6.86ipm.. Then Drilling a 59/64 (.921) hole with a HSS drill.. Running 415rpm at 4.56ipm... Cant seem to find a good feed and speed... Also using a 95 Haas VF3 15hp.. no coolant through spindle, or air blast... Just coolant. Right now using a peck cycle and bringing th bits about the part .625 above the part to hopefully get the coolant to flush chips and cool hole before next peck.. (not working to great) Any help on some feeds and speeds or new tooling would be great..
THANKS, CLIFF

[txcncman]

What is the actual problem?

Are you burning up drills too fast?

Wanting to speed things up?

How much peck are you doing?

[cterry352]

All of the above...LOL

Yes the 59/64 HSS drill is burning up.. Only pecking .275 on the drill.. Chips are strings and dark blue... Really hot.. But its only running 415rpm and 4.56ipm.. I think its two slow.. but thats at a 100sfm..

The 13mm drill is running at 858rpm and 6.86ipm pecking .200 and is doing ok until it gets about .625 deep then kind of starts looking bad.. But same issue dark blue string chips..

But yes im looking to speed up things.. Getting into a high production with these parts.. maybe 200-300 a week.. which don't sound like a lot but we only run first shift 8hrs.. so its high production for us...

[txcncman]

Well, my first recommendation is to switch to carbide. Iscar makes a nice set up in their Chamdrills.

My next recommendation is to try to slow the RPM and increase feed until you have a problem with drill walk. Also, I usually start my peck increment at 1/8 of the drill diameter. Probably 0.625 clearance is unnecessary. 0.100 to 0.300 should be ok. If your chip thickness is right, they should clear themselves without much help from the coolant. Stringers are usually a bad sign in any color. Make multiple drill cycles if you have to and use chip break as deep as you can, then change to full retract pecking. Keep your return to bottom of hole clearance as small as is reasonable to speed things along. I usually do 0.010. I think you have to set this in parameters.

If you want help to tweak your G-code, post what you have now an I will take a look at it.

[RICHARD ZASTROW]

Have you ever used "Chipbreaker" drills? They do as their name implies, break chips.

The blue color indicates two things may be happening.
1.) speed too fast for material
2.) coolant not getting to the cutting zone all the time. Stringy chips may be preventing the coolant from flowing in behind the drill. Chipbreaker would eliminate much of this problem.

Dick Z

add: General Chipbreaker Drill Co. Available thru most tool suppliers. Have coolant thru tool as well, that would help solve the blue strings as well.

[txcncman]

As Dick has indicated, there are physical happenings down in the hole that have to be considered. The stringy chips is one. That was why I recommended using a small peck increment. This "forces" chip breakage. Using a drill with a geometry that "forces" chip breakage is also a possible answer.

Another thing to consider is that, the spiral flute on a drill does what as it is spinning in the hole? Acting as an auger, and trying to pull anything that is in the hole out. This includes coolant. Slowing the RPM down, can reduce some heat and allow coolant to get down in the hole a little easier which increases lubrication and cooling, thus reducing heat build up even more. I have seen too many time that machinist want to spin tools/material even faster with the idea that it increases the speed of production.

There is a point you reach called "the point of diminishing returns". Running more RPM causing tools to wear out/break cost time to change out tool, cost of the tool, and the cost of part scrap or rework time. Some place is a "happy medium". Where that place is, each machinist has to calculate and find out on their own for their own situation. And the situation changes from job to job.

"Good" and experienced machinists tend to do this intuitively. And it is almost impossible to explain it to management-types and bean counters. At some point, management-types and bean counters need to back off and let machinist do the best they can.

[cterry352]

Ok i will post the program tomorrow.. around 7am est.. But its just a simple peck cycle out of Feature Cam.. Im trying to get some materials set up in the software but its not workin out to great.. Really when you don't have time bc they want production running all day... but its got
G54 G98 G83 Z-1.125 R.125 Q.275..

I think the material is a lot of the problem, i used to be in Tool and Die and drilling in H-13 or P20 was never a problem.. But this low alloy carbon stuff just ain't good.. Its just a soft material. And it would be nice to go all carbide but getting the company to fork out the money is another story.. Right now the best i can get is some HSS coated tools

Well, my first recommendation is to switch to carbide. Iscar makes a nice set up in their Chamdrills.

My next recommendation is to try to slow the RPM and increase feed until you have a problem with drill walk. Also, I usually start my peck increment at 1/8 of the drill diameter. Probably 0.625 clearance is unnecessary. 0.100 to 0.300 should be ok. If your chip thickness is right, they should clear themselves without much help from the coolant. Stringers are usually a bad sign in any color. Make multiple drill cycles if you have to and use chip break as deep as you can, then change to full retract pecking. Keep your return to bottom of hole clearance as small as is reasonable to speed things along. I usually do 0.010. I think you have to set this in parameters.

If you want help to tweak your G-code, post what you have now an I will take a look at it.

[cterry352]

But starting with what I got can anyone give some speeds and feeds maybe a good peck. I would like to use the G52 with the G83 I J K and use a good first peck then step down pecks after that.. But its only a .750 hole lol how hard could it be...lol guess getting into a production part will let me find out..

[txcncman]

All the charts I checked call for 110 SFM for high speed steel in A572. For your 0.5118 drill this comes out to 821 RPM. So at 858 you were in the zone. For the 0.921 drill it comes out to 456. So your 415 might be a little low, but it is also still in the zone.

At 456 RPM, being aggressive at 0.007, 6.38 IPM would be the feed.

At 821 RPM, being agressive at 0.006, 9.85 IPM would be the feed.

[cterry352]

Ok well i got all the SFM's out of an machinist handbook, and from the accupro.. so i will make some minor changes and see what happens.. maybe getting the coolant on the drills is a problem... what about pecks anything you would start with?

Also im having to mill out the .921 hole to 1.5 with a tolerance of +.005 -.000

So i use a 3/4 4flute carbide endmill... to rough out the dia, then a .500 six flute carbide endmill to finish the dia.. but having some problem with keeping a good finish.. i have tried all kinds of feeds and speeds from 200-300sfm for the .750 and 300-400 for the .500 Any suggestions on that?

The problem is finding some good feeds and speeds to run some productions right now im olny running about 30-40 parts before drills burn up or endmills chip..

[txcncman]

As I stated earlier, I would start with a peck of 1/8 of drill diameter.

For 0.921 drill, this would be 0.115. Now, you might not need the 0.115 peck until you get deeper in the hole. I do not recall the G-codes for the Haas drilling cycles. But I recommend using a chip break only cycle (drill stays in the hole) for, say, maybe the first half of hole depth (probably at the 0.275 peck). Then switch to a full retract chip clearing cycle for the rest of the hole depth (switching to the 0.115 peck). Even if you can't figure out the G-codes for this and have to hand code each line, it will be worth it to you in the long run on saved drills and probably increases production.

Same on the 0.5118 drill. Stay with your 0.200 peck, but change to a chip break only cycle to the 0.625 depth you mentioned. Then switch to the full retract cycle and change to a 0.064 peck.

Remember, this might seem slower with the increased number of times the drill goes in and out of the hole. But you are also increasing your feed rates (by about 50%). And if this saves you changing out drills so often, you pick up even more time savings there.

Also a word on coolant. I know Haas have the programmable coolant nozzle. But, if there is any way you can add one or more extra coolant nozzles so you can blast right at the hole, that will help.

[txcncman]

On your end mills, what are you running for axle DOC and radial DOC?