Phenolic - Speeds & Feeds???

[mmphoenix]

I'm setting up to machine some 2.0" thick Phenolic Sheet. I have not machined any of this stock in the past. I know it should machine pretty easy but I was curious about a good starting point for speeds, feeds & DOC. I'm going to use a 1.0" 2flt Carbide EM for roughing some thru pockets and would like to take at least 0.500" DOC per pass. I figured I would start out at 4600 RPM (1200 SFM) and 73 IPM (0.008 FPT). Does this sound close or is this to conservative? Any advice would be greatly appriciated.

 

Thanks

[Trevor Bailey]

is it paper based or cloth? big difference in cutting speeds.

[mmphoenix]

2.0" Phenolic Sheet CE (Canvas Electrical) - Thats all the info I have @ this time.

[Tim Johnson]

We run our carbide end mill at 600 sfm at about .01 fpt fo a 1" (.250 doc). Pnenolic is abrasive as heck. If you're going to run more than a few get ALL of your tooling coated. We use BALINIT® HARDLUBE (Balzers). Also phenolic stresses out and chips on the edge easily so a .500 doc might not work on a large sheet.

[Mcam Nut]

quote:

---

at least 0.500" DOC per pass

---

Good luck with that Phenolic is hard $hit, unless you are only taking 10% dia of your cutter, this probally wont work all that great. We usually run it similar to the speeds and feeds of stainless. The speeds and feeds is way to high as well. start somewhere around 1000 rpm and maybe a .01 fpt

[wildpair]

ran alot of phenolic last year for race teams. we used 1/4 carbide (garr) 10000 rpm 250 ipm for surface machining and contouring. I got good parts and also good tool life. only problem is this stuff sticks (lol) and turns everything yellow. I also used 1/2 emill same speed and feed worked great also.

[MACHINEMASTERG]

we also use a vacumme system to suck up the chips as you go its nasty stuff to inhale so dont

[lynnz]

I agree with Greg. Lots of yellow dust.

A vacuum is a must.

 

lynnz

[Mcam Nut]

quote:

---

10000 rpm 250 ipm for surface machining and contouring

---

That has to be a difernt stuff then what im talking about. The first time I machined it I ran a 3" face mill at 6500 rpm 100ipm .01 doc, and it burned the inserts off in 1 pass, just made a mess.

[Trevor Bailey]

The key here is WHAT KIND of phenolic are you cutting. If it is paper based, high feeds, low speeds. If it is cloth based with any glass at all, quit and look for another job. Reason being, the bosses will never understand why you are going thru so many cutters, carbide or HSS.

[mtnflyr]

Amen to that Trevor!

Another thing to look forward to. Cutting this stuff it smells like burning $hit.

 

Chris

[Mcam Nut]

quote:

---

If it is cloth based with any glass at all

---

Yeah thats the stuff, I didnt realize that there was other types before now

 

quote:

---

Cutting this stuff it smells like burning $hit.

---

When I see a order coming through the door to machine this stuff I am some glad to be a programmer, and not the sucker out on the floor pushing cycle start

[Programinator]

im cutting this crap today and it stinks bad and hurts your lungs.

 

i hate this crap. the mask does not seem to help much.

 

Did i say i hate this crap. well i do and im the only one in the shop today suffering. no ventalation system in the shop so there is like a cloud in here.

 

I go outside every 1/2 hour for some air but its so stinkin cold out there.

 

I cant win.

 

Why am i the only stupin one working today

[Thee Dragracer1951]

I turned a bunch of cloth abssed FR4. What a nasty mess.... And flat burned up some cutters.

Couldn't go fast enough to make any money and couldn't go slow enough to not loose my A$$ in tooling.

[Programinator]

my lungs still hurt and my nose is burning.......good thing i have the weekend to recoop.....then its back at it on monday....cant wait to get back to steel and aluminum ( which just kills you slowly)

[Jim at Gentex]

Well it's time to revive this thread!

I will have a job upcoming to cut some square grooves into a piece of phenolic for our Electrical Engineering folks.

The grooves are .020" wide x .100 deep.

I have some .020 x .125 end mills, but I have no clue where to start with speed, feed, depth-of-cut.

I'm not sure which type it is, but it is pretty dense and the edges show white bands running through it which leads me to believe it is the cloth based stuff with glass reinforcement.

Any suggestions on speed/feed/d.o.c. to start?

[Matthew Hajicek - Singularity]

Slow.  And lots of air if you can't run coolant.

[Jim at Gentex]

Yeah I'm not sure if I can run coolant on this stuff, although I would like to.  I thought the material would absorb the coolant, which for this application would definitely not be good.  My understanding is that copper electrodes of some kind are to be nested into these grooves, and that current will pass through them.  So if we were to have residual coolant weeping out from the piece of phenolic, this would most likely be an issue.   

The good news is that this will be a 1-off piece rather than a production type of job, so time will be less critical than accuracy.

I'm also wondering if a slitting saw may be better than an end mill for this particular application, but I would also not have a clue to speed and feed for that either.

Any more suggestions?

Thanks. 

[Tim Johnson]

It's been many years since I've ran phenolic but here is what I used for slotting.

 

9.  END MILLING-SLOTTING   DEPTH OF CUT   SPEED   CUTTER DIA.   FEED PER TOOTH
                      HSS     .030        500       3/8"             .003
                              .030        500       1/2"             .004
                              .030        500       3/4"             .008
                              .030        500       1-2"             .010
                              .125        450       3/8"             .003
                              .125        450       1/2"             .004
                              .125        450       3/4"             .008
                              .125        450       1-2"             .010
                              DIA/2       400       3/8"             .002
                              DIA/2       400       1/2"             .003
                              DIA/2       400       3/4"             .006
                              DIA/2       400       1-2"             .008
                              DIA/1       350       3/8"             .001
                              DIA/1       350       1/2"             .002
                              DIA/1       350       3/4"             .004
                              DIA/1       350       1-2"             .006
                    CARBIDE   DIA/4       540       1/8"             .001
                              DIA/4       540       3/16"            .002
                              DIA/4       540       1/4"             .003
                              DIA/4       540       3/8"             .004
                              DIA/4       540       1/2"             .006
                              DIA/4       540       5/8"             .008 
                              DIA/4       540       3/4"             .010
                              DIA/4       540       1-2"             .015 
                              DIA/2       480       1/8"             .001
                              DIA/2       480       3/16"            .002
                              DIA/2       480       1/4"             .003
                              DIA/2       480       3/8"             .004 
                              DIA/2       480       1/2"             .006
                              DIA/2       480       5/8"             .008 
                              DIA/2       480       3/4"             .010
                              DIA/2       480       1-2"             .015 
                              DIA/1       ---       1/8"             -----
                              DIA/1       320       3/16"            .001
                              DIA/1       320       1/4"             .0015
                              DIA/1       320       3/8"             .002
                              DIA/1       320       1/2"             .003
                              DIA/1       320       5/8"             .004 
                              DIA/1       320       3/4"             .005
                              DIA/1       320       1-2"             .008 

I think this came from the Machining Data Handbook

[Matthew Hajicek - Singularity]

Carbide slitting saw I think would definitely beat the endmill, so long as it's nice and sharp.  Your worst enemy will be the low thermal conductivity of the material, so whatever heat you generate will stay in the slot; the saw will move the heat out better as the hot part rotates out of the cut and the cool part enters the cut.

[Jim at Gentex]

Thanks again for the input, guys.

Helpful as always! 

It looks as though this particular job may be getting booted over to our Tool Room, so I may not need to worry about it after all. 

I will pass the info from here over to our Lead Toolmaker since it looks like this will probably become his headache.   

[Tim Johnson]

There's nothing like walking in to the smell of cancer first thing in the morning.

[jeff]

7 hours ago, Jim at Gentex said:

Yeah I'm not sure if I can run coolant on this stuff, although I would like to.

I wouldn't. It will just swell up and deform. 

At least the phenolic that we run does. 

[Mike@Lustre]

Myself  I  would not be blowing the stuff around  .

 

I would use a vacuum to suck the waste up from it , less contamination to the machine and environment . I have manually machined tons of the stuff used to make bushing and thrust washers with the reddish brown version of it . If the stuff is hard on tooling , imagine what it will do to the ball/lead screws and the ways .

I would also use some form of a respirator as well , early versions of the material where known to be carcinogenic and contained asbestos . Always nice to find out years after you spent many a hour in front of a mill or lathe getting covered in the stuff .  

[Zbuilder]

The dust isn't the only issue. I think the CE & LE phenolics are made with and release when cut....  "Includes, but is not limited to, phenol-formaldehyde, phenol-furfural and resorcinol-formaldehyde."

source... https://www.epa.gov/stationary-sources-air-pollution/manufacture-aminophenolic-resins-national-emission-standards

My nose burns when the a lot of parts are being cut on the saw. Inhaling too much of it makes my nostrils burn. Ventilation is required. When parts get to CNC milling & turning, not a problem because we use synthetic coolants. Don't use oil based on phenolics or it with get absorbed into the material by the fibers. Not good for insulating materials. CE & LE also come in the color black, by added graphite. Makes it more abrasive.