the best profilometer numbers you have seen with carbide

bill jones · Post by **bill jones** » Fri Apr 01, 2005 6:04 pm

-Concerning carbide cutters only----to you guys who actively use profilometers:
-what is the smoothest numbers (RA?)you have seen using carbide cutters like when milling block decks and or cylinder heads?
-what diameter cutter wheel?
-How many cutters being used on that cutter?
-what rpm of the cutter wheel?
-what feed rate of the cutter across the part being machined?
-what depth of cut works best for the last pass?
-like how many minutes to make a pass across a SBC head?
-what about coolant?
-does a cast iron surface end up with the exact same numbers or do the metals require different speeds and feeds?
----------------------------------------------------
-I am milling heads and blocks on 10"x54" mill with a 6 segment cutter diameter of about 11" and .0012" tilt in the head over that 11" and I run the cutter rpm at 160 and the feed rate fairly slow like about 1 inch per minute.
-I keep hearing you all talk about the numbers but I have never seen any positive proof of any tests ever been done on any local machine work I've been involved with in 40 years, as we have just done what works.
-I do see some guys who cut way too coarse and that is why I when to doing my own milling which I'm not having any problem with.
-BUT---it is looking like I may need be paying pretty close attention for the MLS head gaskets that apparently need a super smooth finish.
-------------------------------------
-I'm not really wanting to change to CBN or whatever to get the super finishes if I don't have to because of what it entails for me to build my own cutter head.

enichols · Post by **enichols** » Fri Apr 01, 2005 8:10 pm

hello
i know and use jamison equipment cbn conversion head on our old winona van norman surfacer
our main reason for switching to cbn was so we could cut aluminum and cast heads in the same machine with less setup time

bill jones · Post by **bill jones** » Fri Apr 01, 2005 11:01 pm

-a couple of things here:
#1 is I do both cast iron heads and aluminum heads with the exact same carbide cutters and I don't recognize any particular problems.
-------------------------------------------------
#2-I use a milling machine (that has a #30 taper in the quill) to machine the heads and blocks, not an automotive machine piece of equipment, so if I want to convert to anything I have to custom build the cutter because nobody makes anything like that for a #30 taper.
---------------------------------------------------
#3-I'm not really interested in milling with CBN but I'm wanting to know about just where the limits are with using carbide.
-If and when I am convinced that I can't live without the CBN cutters and if I feel that I can run the proper speeds and feed on my mill I will probably make the change.
---------------------------------------------
-I do appreciate your response but it doesn't address my question and my wonderments.
--------------------------------------------
-I'd also be interested in what the price range and the brand name and part numbers are of the profilometers you guys use, and how often you are using that piece of equipment.

Post by **ou812** » Sat Apr 02, 2005 2:51 am

I use an 85B storm vulcan with the speed reducer, and I get an ra on aluminum heads of around 15-18 and about the same for cast. If you want a finer finish, just slow the speed down, but it takes forever. In super slo-mo im guessing cause the only profilometer ive used is a borrowed unit from a rep, that its about 10-12. The best finish ive seen is from a ground surface which was super smooth for mls gasket...I think the ra was like 4 or 5! But grinding with coolant is messy and I have not had any problems with 15-18 ra using mls gaskets.
Brian

d4490 · Post by **d4490** » Sat Apr 02, 2005 12:16 pm

Bill,

Sanvik makes a milling head that has standard carbide inserts and it also includes what is called is a wiper. The wiper take the small ridges that cause the higher ra values. I have used them in a machine shop that builds machinery. The milling cutter produces a ground-like surface finish. I don't have a part number, but I think you should have a Sanvik rep in your area. The should have something in a 30 taper also.

bill jones · Post by **bill jones** » Sat Apr 02, 2005 3:18 pm

-I would be wanting as large a diameter cutter that I feel I can use and that's about 12".
-I haven't seen any machine tool companies that make anything much larger than about 6" and I definetly don't want to be making multiple paths across the head or block.
-The 30 taper is a like a b-stard child in the mill taper industry, and it is hard to find much for the 30's so I usually just make my own special tapered shank tools.
-Thanks for your responses-----

Donovan · Post by **Donovan** » Sat Apr 02, 2005 5:12 pm

Bill, I have not machined a lot of cylinder heads or blocks but we do own a precision grinding shop and I have a profilemeter. If you want anything checked I would be happy to do it for you only thing is I am in Colorado. Let me know if you do want it checked.

Donovan
www.ramgrinding.com

Harbinger · Post by **Harbinger** » Sat Apr 09, 2005 11:13 am

-Concerning carbide cutters only----to you guys who actively use profilometers:
-what is the smoothest numbers (RA?)you have seen using carbide cutters like when milling block decks and or cylinder heads?
-what diameter cutter wheel?
-How many cutters being used on that cutter?
-what rpm of the cutter wheel?
-what feed rate of the cutter across the part being machined?
-what depth of cut works best for the last pass?
-like how many minutes to make a pass across a SBC head?
-what about coolant?
-does a cast iron surface end up with the exact same numbers or do the metals require different speeds and feeds?

Bill, our shop does a great deal of milling in cast iron for various industries. We can achieve surface finishes (Ra) in the 2-5 micron range utilizing a wiper without much trouble. Although this is achievable with carbide inserts, it's just not feasible in a production environment. We use CBN and get 8-10x the tool life over carbide and almost 3x the productivity.

The cutter we use is a Mitsubishi FBP415 specifically designed for facing cast iron. You can get that model in sizes up to 12.61", which will utilize 34 cutting inserts. I program finishing speeds for these cutters at 2400 sfm, which would put your 12.61" cutter at 727 rpm. To achieve 2-5 micron finishes you need a chip load (inch/tooth) of .002-.004. At .003 inch/tooth, 727 rpm and with 34 cutting teeth you are feeding at 74 inches per minute. I typically use a finish pass depth of .004-.008.

This is on 50 taper OKK CNC mills with dual contact spindles. Very rigid machines.

I never use coolant for CBN or carbide for that matter. Your insert life will suffer dramatically due to thermal shock. Carbide can handle the heat and your AlTiN coated carbides are designed to work better when hotter, so run them dry.

As far as aluminum is concerned, I use a different cutter for facing. Higher rake and 15º more positive on the insert. Carbide speeds are 2000-3000 sfm and PCD inserts go 3000-4000. 2-5 micron surface finishes are achievable at .003-.006 inch/tooth.

HTH

bill jones · Post by **bill jones** » Sat Apr 09, 2005 12:29 pm

-I certainly appreciate the responses.
-I'm curious as to what this Mitsubishi cutter and the 34 cbn inserts cost?
-The rigidity of my mill certainly isn't any thing like what a 50 taper machine would be, my maximum table travel is about 1/3rd of 74 inches per minute.
-You guys have mentioned a "wiper" and I'd like to know more about exactly what that is.
-D4490 explained it pretty good but does that mean it's a leading or trailing edge from sides of the main point of the cut contact point or a flat trailing edge that is directly behind the cutting edge?-
---------------------------------------------
-Does anybody use diamond edged wheels to grind cast iron and aluminum?

Wolfplace · Post by **Wolfplace** » Sat Apr 09, 2005 1:55 pm

HI Bill,
I have used the "wiper" in carbide made by KenaMetal. It has a trailing edge that "wipes" the peaks off the finish cut. Flattens them.
I don't have the number in front of me but with 12 cutters on a 14" head they did a pretty fair job on my boring mill.
Also, don't have RA numbers as I didn't have my profilometer when I was using them.

I have since gone to a single round CBN cutter for cast iron & can put the RA about any where I wish with it.
The final pass is typically at .002"
I run the machine at 525 RPM & 8-10" / minute & typically see around 30 to 35 RA which is completely compatible with Cometic MLS gaskets.

On Aluminum heads I use a single 3/8" PCD cutter at I believe 22-2400 RPM with a 14" head on a different machine & typical RA's are in the teens.
Again, very compatible with any gasket out there.
I would need to measure the feed but it is about 10-12" / minute
With either machine I can slow the feed if I had need to lower the RA.
At approximately half the feed the aluminum RA is 3 to 5 RA which is just not necessary but it sure looks purdy,,,
No coolant with either machine or cutter.

BTW, I also use a lot of brazed type cutters for the lathe in PCD for aluminum & TPG inserts for flycutting pistons, intake face of aluminum heads etc in the mill & you will love them.
They last forever, (well almost) & again, no coolant & leave a finish that is outstanding.
I used a TPG CBN cutter in the mill for blocks for a while & it actually worked very well but needed to be run about 4-6"/min as I recall & didn't last as long as the round pucks.
These cutters have outstanding life but are VERY FRAGILE.
You cannot "back one up" even slightly or it will break the tip off instantly.

I have a card around here somewhere that has the name of a guy that sells & sharpens the stuff I will try to find & send his name to you.
Just got it recently & haven't tried him but his prices seemed pretty fair.

I was buying the TPG type inserts from another outfit that was reasonable too but I haven't ordered any for a year or so so I will need to see if I can find there number if you want it.
They also had round CBN & PCD

Motorman 407 · Post by **Motorman 407** » Sat Apr 09, 2005 2:26 pm

Harbinger
you might be the man to answer this. We have a Sumitomo 10" face mill with a #40 arbor that we bought used. We are using Sumitomo insets marked 53R A30N on the inserts and N9212 HTA 01996 CSP53R on the boxes they came in. They are square and looks like the Storm Vulcan inserts the way they are cut.
The problem we are having is they wear out quickly (1 block) cutting cast iron even at low rpm (150 - 200 rpm) but cut good in aluminum. I been trying to locate the Mitsubichi inserts for this application but had no luck. Any suggestions would be greatly appreciated or if somebody else has any information.

Harbinger · Post by **Harbinger** » Sat Apr 09, 2005 4:19 pm

Motorman-
The problem you're having with that cutter is right there in "A30N". That's ISO grade P30, a cemented carbide used for milling low-mid carbon steels and alloys. I can't cross reference the other numbers but based on your comments about aluminum machining, that insert geometry may be too positive as well. It's not going to last too long in cast iron, even with a more ideal clearance angle.
If you want to stay with Sumitomo, you should look to their G10E or EH20 grades for cast iron. Those are cemented carbide grades and in all honesty, you'd be better off spending a little more for a cermet like T110A, T2000Z or 1200A. Sumitomo's CBN grades are BN100, BN500, BN600 and BN700.

Inserts use an ISO identification code, so it shouldn't be too difficult to find the same style insert in another brand. However, the code order you listed doesn't give me a clue to the type of insert. Are you sure that "CSP53R" isn't "SPC_"? That would indicate a square insert "S" with an 11º "P" clearance angle with class "C" tolerance. The "R" might specify that this insert uses a clamp, no hole.

Feel free to e-mail me if you want. I'd be more than happy to talk with you more about this.

Bill-
That being the case, I would stay with carbides. You won't gain much in going to CBN if you can't take advantage of the increased surface footage.
The title of the thread reads, "what's achievable" but like Mike mentioned in regards to "required surface finish", a 2-5 Ra finish, while achievable, may not be necessary.

The Mitsu cutter I mentioned is around $1500, then you have to put inserts in it. CBN is about $50+ a piece. So all said and done, you have better than $3k spinning in the air.

With regard to wiper inserts, a cutter of that size (12.6") would only need 5 or 7 wipers. I always use an odd number to reduce any chance of the cutter chattering. Whatever you do, you will want to use wipers and you will also want to make sure those wipers are within .0005 of each other. You can check this with a test indicator at the machine or in a dedicated tool pre-setter.
A few wipers will make even a bad cutter (one with different insert heights) finish well, as long as the wipers protrude further than the inserts. Again, if you can't see paying for CBN, then use a cermet. Better wear and fracture resistance than coated carbide.

Best of luck.

Chuck

Motorman 407 · Post by **Motorman 407** » Sun Apr 10, 2005 3:28 pm

Harbinger
Thanks for the information, I will try the Sumitomo cermet inserts you suggested. Yes the label reads CSP maybe they have there own # system Its a square insert .625 long with no hole.
I understand that Rottler has had some R&D with Mitsubichi with regards to finding a better insert design for machining cast iron blocks and sleeves but Rottler only carries the triangular and small square style.

*
Bill Jones
check out this place for some inexpensive milling supply maybe you can find what you are looking for.
http://stores.ebay.com/Ajax-Industries/Store-Home.html

jdeleon · Post by **jdeleon** » Sun Apr 10, 2005 6:41 pm

I notice most of you using CBN.. cut dry as recommended. Do you get a smear on the surface of aluminum? How bout when you cut across the intake seats?
I use a water based coolant when I cut aluminum with a CBN button, it eliminated the smearing, and I have'nt noticed any loss of insert life due to thermal shock.
Anyone else tried coolants or lubricants?

Wolfplace · Post by **Wolfplace** » Sun Apr 10, 2005 7:58 pm

jdeleon wrote:I notice most of you using CBN.. cut dry as recommended. Do you get a smear on the surface of aluminum? How bout when you cut across the intake seats?
I use a water based coolant when I cut aluminum with a CBN button, it eliminated the smearing, and I have'nt noticed any loss of insert life due to thermal shock.
Anyone else tried coolants or lubricants?

=
I tried CBN on aluminum & found it unacceptable at least to me on a lot of heads even with lubricant as some would still stick to the cutter
Went with a PCD button & never looked back.
There is in my opinion just no comparison between the two cutters no matter what machine manufacturers tell you.

I would just spend the money on a PCD button that will fit your holder & use it on your aluminum.
I think you will love the finish without any coolants or lubricants.

The only exception is as you mentioned, when cutting across an intake seat unless it's copper.
You need to use the CBN with lubricant in this application as the seat will supposedly kill the PCD in short order,, at least according to the cutter gods.
I have cut heads & gotten into the intake seat with PCD & it didn't seem to degrade the cutter but my understanding is this is not a real good idea.

I have cut probably 250-300 heads on the same insert in the mill & have been using the same cemented insert PCD on the lathe for machining various aluminum, brass & bronze items for about a year now & it has a LOT of miles on it & is still alive & kicking,,
I love this stuff for aluminum

Trouble is it spoils you as now I hate it when I have to use any kind of cutting fluids & have to clean up the mess